Eagle library editor

[Phil Hobbs]

I finally bit the bullet and got a copy of Eagle, because I need to do a
bunch of small proto boards. Initial impressions are positive, mostly
because it has a command line at the ready. Score.

The first device I tried creating is an Avago ATF35143 pHEMT, which
comes in a SC70-4 package with the source connected to pins 2 and 4.

There is no obvious way to tell Eagle that both 2 and 4 are connected to
the source.

What's the right way to do this?

Thanks

Phil Hobbs

--
Dr Philip C D Hobbs
Principal Consultant
ElectroOptical Innovations LLC
Optics, Electro-optics, Photonics, Analog Electronics

160 North State Road #203
Briarcliff Manor NY 10510
845-480-2058

hobbs at electrooptical dot net
http://electrooptical.net

[TTman]

"Phil Hobbs" <pcdhSpamM...@electrooptical.net> wrote in message
news:4EF0E47...@electrooptical.net...

>I finally bit the bullet and got a copy of Eagle, because I need to do a
>bunch of small proto boards. Initial impressions are positive, mostly
>because it has a command line at the ready. Score.
>
> The first device I tried creating is an Avago ATF35143 pHEMT, which comes
> in a SC70-4 package with the source connected to pins 2 and 4.
>
> There is no obvious way to tell Eagle that both 2 and 4 are connected to
> the source.
>
> What's the right way to do this?
>
> Thanks
>

are you talking about schematic or PCB representation ?

[George Herold]

On Dec 20, 2:39 pm, Phil Hobbs

<pcdhSpamMeSensel...@electrooptical.net> wrote:
> I finally bit the bullet and got a copy of Eagle, because I need to do a
> bunch of small proto boards.  Initial impressions are positive, mostly
> because it has a command line at the ready.  Score.
>
> The first device I tried creating is an Avago ATF35143 pHEMT, which
> comes in a SC70-4 package with the source connected to pins 2 and 4.
>
> There is no obvious way to tell Eagle that both 2 and 4 are connected to
> the source.
>
> What's the right way to do this?

Well I don't know if this is the 'right' way. But when I have
multiple pins connected to the same 'thing', then in the schematic
symbol I "name" the pins Source@2 and Source@4. I mostly do this with
power pins so it's V+@2 and V+@3.

George H.

[John Larkin]

On Tue, 20 Dec 2011 14:39:40 -0500, Phil Hobbs
<pcdhSpamM...@electrooptical.net> wrote:

>I finally bit the bullet and got a copy of Eagle, because I need to do a
>bunch of small proto boards. Initial impressions are positive, mostly
>because it has a command line at the ready. Score.
>
>The first device I tried creating is an Avago ATF35143 pHEMT, which
>comes in a SC70-4 package with the source connected to pins 2 and 4.
>
>There is no obvious way to tell Eagle that both 2 and 4 are connected to
>the source.
>
>What's the right way to do this?
>
>Thanks
>
>Phil Hobbs

We create a part like that with two visible source pins on the
schematic symbol, and we wire both of them up on the schamatic.

ftp://jjlarkin.lmi.net/FSU02.jpg

John

[Phil Hobbs]

On 12/20/2011 03:17 PM, George Herold wrote:
> On Dec 20, 2:39 pm, Phil Hobbs
> <pcdhSpamMeSensel...@electrooptical.net> wrote:
>> I finally bit the bullet and got a copy of Eagle, because I need to do a
>> bunch of small proto boards. Initial impressions are positive, mostly
>> because it has a command line at the ready. Score.
>>
>> The first device I tried creating is an Avago ATF35143 pHEMT, which
>> comes in a SC70-4 package with the source connected to pins 2 and 4.
>>
>> There is no obvious way to tell Eagle that both 2 and 4 are connected to
>> the source.
>>
>> What's the right way to do this?
>
> Well I don't know if this is the 'right' way. But when I have
> multiple pins connected to the same 'thing', then in the schematic
> symbol I "name" the pins Source@2 and Source@4. I mostly do this with
> power pins so it's V+@2 and V+@3.
>
> George H.

Thanks, George, putting two source pins in the symbol works.

Cheers

[Spehro Pefhany]

That's how I do it too. The internal connection is really just a
visual thing for the user of the schematic. Not sure if Eagle is any
different from Orcad, Altium etc.

How do those physical pins map to the SPICE model?

[Phil Hobbs]

We were talking a few months back about Eagle & LTSpice users chipping
in to get somebody to make an Eagle <--> LTSpice schematic converter.
I'd still be interested if anybody else is.

Cheers

[George Herold]

On Dec 20, 3:31 pm, Phil Hobbs

> hobbs at electrooptical dot nethttp://electrooptical.net- Hide quoted text -
>
> - Show quoted text -

I was just playing around with an opamp with multiple power pins.
Even when I only attched only one in the schematic, they were all
shown connected in the 'rat's nest'.

(The @ symbol is nice 'casue it reminds you of the pin number when you
are connecting the symbol and package together.)

Oh here's a fun editing trick that a coworker recently found in
Eagle. If you hold down the scroll ball on the mouse and then drag
the mouse around it pans the display.

George H.

[lang...@fonz.dk]

On 20 Dec., 21:17, George Herold <gher...@teachspin.com> wrote:
> On Dec 20, 2:39 pm, Phil Hobbs
>
> <pcdhSpamMeSensel...@electrooptical.net> wrote:
> > I finally bit the bullet and got a copy of Eagle, because I need to do a
> > bunch of small proto boards.  Initial impressions are positive, mostly
> > because it has a command line at the ready.  Score.
>
> > The first device I tried creating is an Avago ATF35143 pHEMT, which
> > comes in a SC70-4 package with the source connected to pins 2 and 4.
>
> > There is no obvious way to tell Eagle that both 2 and 4 are connected to
> > the source.
>
> > What's the right way to do this?
>
> Well I don't know if this is the 'right' way.  But when I have
> multiple pins connected to the same 'thing', then in the schematic
> symbol I "name" the pins Source@2 and Source@4.  I mostly do this with
> power pins so it's V+@2 and V+@3.
>

all pins need a unique name, all the @x syntax does is hide the unique
part
so a symbol with several pins that look to have the same name. e.g.
vdd

What Phil is asking for is a symbol with one pin going to multiple
pads

-Lasse

[lang...@fonz.dk]

On 20 Dec., 20:39, Phil Hobbs <pcdhSpamMeSensel...@electrooptical.net>
wrote:

> I finally bit the bullet and got a copy of Eagle, because I need to do a
> bunch of small proto boards.  Initial impressions are positive, mostly
> because it has a command line at the ready.  Score.
>
> The first device I tried creating is an Avago ATF35143 pHEMT, which
> comes in a SC70-4 package with the source connected to pins 2 and 4.
>
> There is no obvious way to tell Eagle that both 2 and 4 are connected to
> the source.
>
> What's the right way to do this?
>
> Thanks
>

before the new version 6 the only way to do it was to have the same
number
of pins and pads and then connect them at the schematic.

in version 6.0, you can connect on pin to mutiple pads, in the library
editor
it is called append

-Lasse

[John Larkin]

It's rare to get a Spice model for PHEMTS. Usually you get
s-parameters, and I assume both sources are grounded for that.

I do have Spice models for a few NEC phemts. The Spice model shows a
single source pin, with package inductance and resistance, and ignores
the fact that the package has two source pins.

John

[Oppie]

Welcome to Eagle. Which version are you uing?
We first bought the professional package starting with version 4 then
upgraded to V5. Version 6 just came out last week and I'm taking my time
about getting an upgrade license. 30 minutes after the release, the first
bug reports came in.
Version 5 has been very stable and I may stay with it for a while yet.

You should definitely check out news://news.cadsoft.de (no login needed)
I've gotten a lot of good information there.

Season's greetings - Oppie

[Phil Hobbs]

Thanks. I'm using Eagle 5.7.0, because it runs in Kubuntu 10.04 LTS.

Cheers

[Oppie]

"Phil Hobbs" <pcdhSpamM...@electrooptical.net> wrote in message

news:4EF169FD...@electrooptical.net...

>> Version 5 has been very stable and I may stay with it for a while yet.
>>
>> You should definitely check out news://news.cadsoft.de (no login needed)
>> I've gotten a lot of good information there.
>

> Thanks. I'm using Eagle 5.7.0, because it runs in Kubuntu 10.04 LTS.
>

I run version 5.11
You might want to check the change log to see if any of the updates are
relevant to your work. If you download the Version 5.12 from
ftp://ftp.cadsoft.de/eagle/program/5.12/
you can either install it (Eagle new installs ALWAYS install in a new
directory so there is no worry about overwriting anything) or use winrar or
winzip to open the install file. Look at the contents of the "doc" directory
and you will find update_en.txt which is the change log. The user manual is
also here.
Having just written that, I have to do likewise to see if there is any
compelling reason to move from 5.11 to 5.12. I have the program set to
check when a new release is available and notify me. Never got a 5.12
notification...

If you have it, the autorouter is pretty good. Just be sure that your grids
are set appropriately or it will never route. There is also a 'follow-me'
router which I really like. No auto-place so just takes experience where to
put things.

Oppie

[Phil Hobbs]

Thanks for the wisdom on the last newbie question. I managed to finish
a simple schematic (1 pHEMT, one SiGe bipolar, and one fast op amp--a
whole 22 parts altogether).

Now for a board layout, and the next question. I figured out how to set
the design rules to make a four-layer board with two cores, with prepreg
in between. Now I need to make a ground plane. So far, I've done:

set layer 2 to be net GND, supply plane box checked in the DISPLAY dialogue

POLY GND
draw the polygon
autoroute (just for test purposes, honest)

The autoroute fails because it's trying to put everything on layer 1,
and it ignores the ground plane almost entirely--it routes the grounds,
and it makes no vias or thermals in the ground plane. Except for
one--it makes a big hole under the Pin 1 mark on the IC package, which
is drawn as a wire in the package editor.

How do I get Eagle to recognize the ground plane as a ground plane?

How do I get the autorouter to use more than one layer?

[David]

On 21/12/2011 20:23, Phil Hobbs wrote:
> Thanks for the wisdom on the last newbie question. I managed to finish a
> simple schematic (1 pHEMT, one SiGe bipolar, and one fast op amp--a
> whole 22 parts altogether).
>
> Now for a board layout, and the next question. I figured out how to set
> the design rules to make a four-layer board with two cores, with prepreg
> in between. Now I need to make a ground plane. So far, I've done:
>
> set layer 2 to be net GND, supply plane box checked in the DISPLAY dialogue

I used Eagle for about 10 years but never used supply plane layer - onlu
ever used poly

>
> POLY GND
> draw the polygon

if you have other pins named gnd then this should work and your plane
will conencto to teh pins automatically. If it is al SMD then you will
manually need to place vias

> autoroute (just for test purposes, honest)
>
> The autoroute fails because it's trying to put everything on layer 1,
> and it ignores the ground plane almost entirely--it routes the grounds,
> and it makes no vias or thermals in the ground plane. Except for one--it
> makes a big hole under the Pin 1 mark on the IC package, which is drawn
> as a wire in the package editor.

there are several parameters to work with in the autorouter I played
with it a few times but never got good results - I'd end up taking as
long tidying it all up as I would laying it out from scratch - but my
boards were never all that big - normally eurocard size.

>
> How do I get Eagle to recognize the ground plane as a ground plane?
>
> How do I get the autorouter to use more than one layer?
>
> Thanks
>
> Phil Hobbs
>

The cadsoft eagle newsgroups used to be excellent for support but it
looks like they've moved to a web based forum and I'm not sure well that
compares

cheers

David

[Joerg]

Phil Hobbs wrote:
> Thanks for the wisdom on the last newbie question. I managed to finish
> a simple schematic (1 pHEMT, one SiGe bipolar, and one fast op amp--a
> whole 22 parts altogether).
>
> Now for a board layout, and the next question. I figured out how to set
> the design rules to make a four-layer board with two cores, with prepreg
> in between. Now I need to make a ground plane. So far, I've done:
>
> set layer 2 to be net GND, supply plane box checked in the DISPLAY dialogue
>
> POLY GND
> draw the polygon
> autoroute (just for test purposes, honest)
>
> The autoroute fails because it's trying to put everything on layer 1,
> and it ignores the ground plane almost entirely--it routes the grounds,
> and it makes no vias or thermals in the ground plane. Except for
> one--it makes a big hole under the Pin 1 mark on the IC package, which
> is drawn as a wire in the package editor.
>
> How do I get Eagle to recognize the ground plane as a ground plane?
>

You'd have to name the polygon "GND" or whatever net name you have
assigned to ground. I never do layouts but I think it's done via the
polygon button while in the layout window.

> How do I get the autorouter to use more than one layer?
>

See if trestrict and brestrict are set correctly (or not set). In the
setup you can (AFAIR) even specify the preferred routing direction for
each layer.

Unless the layout is super RF-critical stuff it is usually more
economical to contract it out. If you need an Eagle layouter drop me a
line, I had a layout done on Eagle a few months ago. If it doesn't have
to be Eagle there is someone at a company in S.F. that you know :-)

--
Regards, Joerg

http://www.analogconsultants.com/

[JeffM]

Joerg wrote:
>if it doesn't have to be [EAGLE]{1}[,]

>there is someone at a company in S.F. that you know :-)
>

...and perhaps she would like to learn another package
beyond PADS.

...and for other EAGLE neophites considering that package:
http://tinyurl.com/TheEAGLE-Virus

Now, for a show of hands here
of anyone who ever got useful results from an autorouter.
...particularly on a project with more than 22 components.
...especially with an ECAD package that cost less than $5k.
.
.
{1} An initialism for Easily Applicable Graphical Layout Editor.

[Phil Hobbs]

On 12/21/2011 04:00 PM, Joerg wrote:
> Phil Hobbs wrote:
>> Thanks for the wisdom on the last newbie question. I managed to finish
>> a simple schematic (1 pHEMT, one SiGe bipolar, and one fast op amp--a
>> whole 22 parts altogether).
>>
>> Now for a board layout, and the next question. I figured out how to set
>> the design rules to make a four-layer board with two cores, with prepreg
>> in between. Now I need to make a ground plane. So far, I've done:
>>
>> set layer 2 to be net GND, supply plane box checked in the DISPLAY dialogue
>>
>> POLY GND
>> draw the polygon
>> autoroute (just for test purposes, honest)
>>
>> The autoroute fails because it's trying to put everything on layer 1,
>> and it ignores the ground plane almost entirely--it routes the grounds,
>> and it makes no vias or thermals in the ground plane. Except for
>> one--it makes a big hole under the Pin 1 mark on the IC package, which
>> is drawn as a wire in the package editor.
>>
>> How do I get Eagle to recognize the ground plane as a ground plane?
>>
>
> You'd have to name the polygon "GND" or whatever net name you have
> assigned to ground. I never do layouts but I think it's done via the
> polygon button while in the layout window.

I did that, but it's still trying to route GND. It may be that it's
confused since I started the schematic on the freeware version and then
bought a license.

>
>
>> How do I get the autorouter to use more than one layer?
>>
>
> See if trestrict and brestrict are set correctly (or not set). In the
> setup you can (AFAIR) even specify the preferred routing direction for
> each layer.
>
> Unless the layout is super RF-critical stuff it is usually more
> economical to contract it out. If you need an Eagle layouter drop me a
> line, I had a layout done on Eagle a few months ago. If it doesn't have
> to be Eagle there is someone at a company in S.F. that you know :-)
>

Thanks. I'm not planning to start laying out all of my own boards,
don't worry. It's just that I'm doing a lot of stuff with 20-GHz SC70
transistors these days, and I'd love to be able to order 20 or 50 tiny
little boards in various version to hack up, rather than go blind trying
to use a Dremel. If I can just get over this little hurdle, I should be
able to do that.

Cheers

[George Herold]

On Dec 21, 3:23 pm, Phil Hobbs

I mostly do two layer boards. I draw the polygon where I want it.
And then I "name" the polygon GND. (Or whatever the name of the net is
that I want the polygon connected as.)

****Warning***
A coworker was laying out a four layer board with some internal ground
and power planes and using the polygon commmand for internal layers
swallowed up his via's.
We run version 4.15 so this may have been fixed in your version.

I think he used the Rectangle (or box?) command and that worked.

I'll send an email and ask,

George H.
(at home, sick with a bug)

[Joerg]

JeffM wrote:
> Joerg wrote:
>> if it doesn't have to be [EAGLE]{1}[,]
>> there is someone at a company in S.F. that you know :-)
>>
> ...and perhaps she would like to learn another package
> beyond PADS.
>

Wots wrong with PADS? Over the last 10 years or so most of my layouts
have been done with PADS and I didn't see anything amiss.

But I am not picky about details. Like with cars. Dealer asks me what
color I like and I tell him it doesn't matter ... "Say WHAT?!"

> ...and for other EAGLE neophites considering that package:
> http://tinyurl.com/TheEAGLE-Virus
>

Ah, the cruzade ... You and your conspiracy theory :-)

> Now, for a show of hands here
> of anyone who ever got useful results from an autorouter.
> ...particularly on a project with more than 22 components.

Nay.

> ...especially with an ECAD package that cost less than $5k.

Don't matter. An autorouter is usually no good when it comes to hot stuff.

> .
> {1} An initialism for Easily Applicable Graphical Layout Editor.

An it is, except for the library editor which really takes some getting
used to. But the major shortcoming of Eagle is the lack of a hierarchy.
They waved it off again for V6 which makes me think there is a deeper
screw-up in the data structure. So I'll sit out that upgrade as well.

[Joerg]

That should not matter. Usually it only gives problems if you re-use a
chunk of schematic from a guy who used a cracked copy. But in the
professional world that can hardly happen.

One problem that can happen with Eagle, a least not in 4.19: You cannot
rename supply symbols. Yeah, it does work on the schematic but the
netlist can still be screwed up. If in doubt spool out a netlist and
take a look. The net has to be exactly named as the one you want.

>>
>>> How do I get the autorouter to use more than one layer?
>>>
>>
>> See if trestrict and brestrict are set correctly (or not set). In the
>> setup you can (AFAIR) even specify the preferred routing direction for
>> each layer.
>>
>> Unless the layout is super RF-critical stuff it is usually more
>> economical to contract it out. If you need an Eagle layouter drop me a
>> line, I had a layout done on Eagle a few months ago. If it doesn't have
>> to be Eagle there is someone at a company in S.F. that you know :-)
>>
>
> Thanks. I'm not planning to start laying out all of my own boards,
> don't worry. It's just that I'm doing a lot of stuff with 20-GHz SC70
> transistors these days, and I'd love to be able to order 20 or 50 tiny
> little boards in various version to hack up, rather than go blind trying
> to use a Dremel. If I can just get over this little hurdle, I should be
> able to do that.
>

For that it should work. There's even board houses that take Eagle files
directly. But the usual cheap Chinese shop won't. Olimex does.

[Joerg]

Phil Hobbs wrote:
> On 12/21/2011 04:00 PM, Joerg wrote:
>> Phil Hobbs wrote:

[...]

>>> How do I get Eagle to recognize the ground plane as a ground plane?
>>>
>>
>> You'd have to name the polygon "GND" or whatever net name you have
>> assigned to ground. I never do layouts but I think it's done via the
>> polygon button while in the layout window.
>
> I did that, but it's still trying to route GND. It may be that it's
> confused since I started the schematic on the freeware version and then
> bought a license.
>

BTW, you can place a post in the Eagle NNTP forum and attach your files
if not confidential. Usually either another user or Cadsoft staff will
answer within 24h and let you know where the missing bolt was.

It's the best support forum east and west of the Mississippi.

[...]

[John Fields]

On Wed, 21 Dec 2011 13:27:34 -0800 (PST), JeffM <jef...@email.com>
wrote:

>Joerg wrote:
>>if it doesn't have to be [EAGLE]{1}[,]
>>there is someone at a company in S.F. that you know :-)
>>
>...and perhaps she would like to learn another package
>beyond PADS.
>
>...and for other EAGLE neophites considering that package:
>http://tinyurl.com/TheEAGLE-Virus
>
>Now, for a show of hands here
>of anyone who ever got useful results from an autorouter.

---
Nay.

--
JF

[John Larkin]

On Wed, 21 Dec 2011 15:23:23 -0500, Phil Hobbs
<pcdhSpamM...@electrooptical.net> wrote:

>Thanks for the wisdom on the last newbie question. I managed to finish
>a simple schematic (1 pHEMT, one SiGe bipolar, and one fast op amp--a
>whole 22 parts altogether).
>
>Now for a board layout, and the next question. I figured out how to set
>the design rules to make a four-layer board with two cores, with prepreg
>in between. Now I need to make a ground plane. So far, I've done:
>
>set layer 2 to be net GND, supply plane box checked in the DISPLAY dialogue
>
>POLY GND
>draw the polygon
>autoroute (just for test purposes, honest)
>
>The autoroute fails because it's trying to put everything on layer 1,
>and it ignores the ground plane almost entirely--it routes the grounds,
>and it makes no vias or thermals in the ground plane. Except for
>one--it makes a big hole under the Pin 1 mark on the IC package, which
>is drawn as a wire in the package editor.
>
>How do I get Eagle to recognize the ground plane as a ground plane?
>
>How do I get the autorouter to use more than one layer?
>
>Thanks
>
>Phil Hobbs

Hi, Phil,

We never autoroute. It usually makes a mess, and isn't smart enough to
do fast stuff.

We have given up declaring power and ground planes (under PADS), too.
We just draw a copper pour or so on a regular routing layer, which is
a lot more flexible and actually easier to manage.

John

[George Herold]

On Dec 21, 4:43 pm, Phil Hobbs

Hmm, once you name the poly, you have to hit the rat's nest button
again to fill the thing in and connect up the poly.

I've never used the autorouter.

George H.

>
>
>
> >> How do I get the autorouter to use more than one layer?
>
> > See if trestrict and brestrict are set correctly (or not set). In the
> > setup you can (AFAIR) even specify the preferred routing direction for
> > each layer.
>
> > Unless the layout is super RF-critical stuff it is usually more
> > economical to contract it out. If you need an Eagle layouter drop me a
> > line, I had a layout done on Eagle a few months ago. If it doesn't have
> > to be Eagle there is someone at a company in S.F. that you know :-)
>
> Thanks.  I'm not planning to start laying out all of my own boards,
> don't worry.  It's just that I'm doing a lot of stuff with 20-GHz SC70
> transistors these days, and I'd love to be able to order 20 or 50 tiny
> little boards in various version to hack up, rather than go blind trying
> to use a Dremel.  If I can just get over this little hurdle, I should be
> able to do that.
>
> Cheers
>
> Phil Hobbs
>
> --
> Dr Philip C D Hobbs
> Principal Consultant
> ElectroOptical Innovations LLC
> Optics, Electro-optics, Photonics, Analog Electronics
>
> 160 North State Road #203
> Briarcliff Manor NY 10510
> 845-480-2058
>

[John Larkin]

On Wed, 21 Dec 2011 13:56:55 -0800, Joerg <inv...@invalid.invalid>
wrote:

>JeffM wrote:
>> Joerg wrote:
>>> if it doesn't have to be [EAGLE]{1}[,]
>>> there is someone at a company in S.F. that you know :-)
>>>
>> ...and perhaps she would like to learn another package
>> beyond PADS.
>>
>
>Wots wrong with PADS? Over the last 10 years or so most of my layouts
>have been done with PADS and I didn't see anything amiss.
>
>But I am not picky about details. Like with cars. Dealer asks me what
>color I like and I tell him it doesn't matter ... "Say WHAT?!"

That does shock them. I ordered one car and told the guy "anything but
green", and he made strangling noises like that.

But I like the blazing red Audi, what with every other car on the
planet being shades of black. I've just lately seen a few car ads with
non-grey cars featured.

>
>> ...and for other EAGLE neophites considering that package:
>> http://tinyurl.com/TheEAGLE-Virus

One neat thing about PADS is that you can import/export anything in
ASCII, including a design and all its library parts. You can do cool
things with that.

John

[John Larkin]

Every now and then I do a board with all sorts of stuff on it: goofy
idea circuits, parts adapters, connector adapters, filters, CPWs,
whatever, usually a 4-layer, order a half dozen, and shear them up as
needed.

John

[John S]

Phil -

Try this:
http://www.cadsoftusa.com/contact/

Under Americas there is a phone number. I used to get Ed Robled...(add
an o), but I don't know if he is still there. If so, he is
knowledgeable. You earned the support with your license.

Cheers,
John

[Doug White]

Phil Hobbs <pcdhSpamM...@electrooptical.net> wrote in

news:4EF2403B...@electrooptical.net:

> Thanks for the wisdom on the last newbie question. I managed to
> finish a simple schematic (1 pHEMT, one SiGe bipolar, and one fast op
> amp--a whole 22 parts altogether).
>
> Now for a board layout, and the next question. I figured out how to
> set the design rules to make a four-layer board with two cores, with
> prepreg in between. Now I need to make a ground plane. So far, I've
> done:
>
> set layer 2 to be net GND, supply plane box checked in the DISPLAY
> dialogue
>
> POLY GND
> draw the polygon
> autoroute (just for test purposes, honest)
>
> The autoroute fails because it's trying to put everything on layer 1,
> and it ignores the ground plane almost entirely--it routes the
> grounds, and it makes no vias or thermals in the ground plane. Except
> for one--it makes a big hole under the Pin 1 mark on the IC package,
> which is drawn as a wire in the package editor.
>
> How do I get Eagle to recognize the ground plane as a ground plane?
>
> How do I get the autorouter to use more than one layer?
>
> Thanks
>
> Phil Hobbs

If you are using the free version, I thought it was restricted to two
layers. Maybe they have given up on that.

Doug White

[Joerg]

True, but I wouldn't bug Ed with this kind of stuff. It can be handled
in the Cadsoft NG. Phil might even have his answer before Cadsoft USA
opens in the morning.

Come to think of it, I've never used Cadsoft phone support. The
occasional question was always answered in the forums.

Ed's crew hispanizised my name on the license. So now I am Jorge. Donde
esta el mesclador de margarita? Que podria utilizar uno ahora mismo :-)

--
Feliz Navidad, Joerg

http://www.analogconsultants.com/

[Tim Williams]

"JeffM" <jef...@email.com> wrote in message
news:3ffddbd5-4e03-4efb...@32g2000yqp.googlegroups.com...

> Now, for a show of hands here
> of anyone who ever got useful results from an autorouter.
> ...particularly on a project with more than 22 components.
> ...especially with an ECAD package that cost less than $5k.

We've done a few small boards, maybe 20-50 components, autorouted in
Altium[1]. It does an okay-passable job on resolving the paths -- it
usually finishes. The results are always ugly though. The one with ~50
components we did in 4 layer. On the next rev, I did it by hand, in two
layer, yielding substantial cost savings (plus the routes are absolutely
gorgeous, if I do say so myself ;-) ).

[1] Which brings me to your second point. Bare Altium I *think* is under
$5k, although a few years of subscriptions will obviously run up the
total.

As far as appealing results, autorouters have no sense of style or
direction and tend to treat branches individually. You can assign rules
for buses and connection styles and widths and so on, but all this gets
very tedious, and it's still very limited, in the grand scheme of things.

Most programs don't have a means to specify branch trace widths, which
means any attempt at autorouting a supply line will end in dismal failure.
Either it's all teensy stuff like you'd run for the logic bits, and your
power bits burn it through, or it's all fat stuff that won't even fit on
the logic bits, or it's some inappropriate compromise between these
extremes that neither fits nor handles the current. Disabling autorouting
on supply nets is usually futile, as you still have to navigate through
the morass left by the autorouter; tools with "push" routing (which Altium
supports) make this somewhat easier, but it will always be tedious (and
leave your PCB swiss-cheesed from vias).

Tim

--
Deep Friar: a very philosophical monk.
Website: http://webpages.charter.net/dawill/tmoranwms

[JeffM]

>>Joerg wrote:
>>>if it doesn't have to be [EAGLE,]

>>>there is someone at a company in S.F. that you know :-)
>>>
>JeffM wrote:
>>...and perhaps she would like to learn another package
>>beyond PADS.
>>

Joerg wrote:
>Wots wrong with PADS?
>
Nothing that I'm aware of
--except its current corporate ownership.

>Over the last 10 years or so most of my layouts
>have been done with PADS and I didn't see anything amiss.
>

I have no specific gripe against PADS.
If I was going to advocate for a *replacement* for PADS,
it certainly wouldn't be in favor of Cadsoft's DRM'd junk.

My reference was to the Brat
expanding/enhancing her knowledge/skillset.
Y'know, making herself more valuable in a lousy labor market.

>>http://tinyurl.com/TheEAGLE-Virus
>>
>Ah, the cruzade ... You and your conspiracy theory :-)
>

Knowledge is power. Forewarned is forearmed.
DRM sucks.
Companies that treat their paid customers
like something they need to scrape off their shoe need to die.
NOW.

>An autorouter is usually no good
>

You could have stopped there.

>when it comes to hot stuff.
>

I think that part goes without saying.

>>Easily Applicable Graphical Layout Editor.
>>

>[And] it is, except for the library editor

>which really takes some getting used to.
>

...and anyone thinking about re-using someone else's symbols,
needs to see "DRM", above. Getting bitten in the butt
then told by the software vendor to go screw yourself
just leaves me completely cold wrt Cadsoft/EAGLE.

DRM **only** hurts the people who **pay** for products;
the *actual* pirates all know how to get around it.
If you're on deadline, EAGLE is **not** the product you want.

>But the major shortcoming of Eagle is the lack of a hierarchy.
>

...if you've never been bitten in the butt by their DRM.

>They waved it off again for V6
>

{Shakes head side to side}
Just pitiful, Cadsoft.

>which makes me think there is a deeper screw-up
>in the data structure.
>

Pitiful.
Makes me think of M$'s "security" model.

>So I'll sit out that upgrade as well.
>

...then there's my advice: Don't get *started* with Cadsoft.
...or any company that uses DRM and
treats customers like something they wouldn't want to step in.

[John S]

On 12/21/2011 5:45 PM, Joerg wrote:

> Ed's crew hispanizised my name on the license. So now I am Jorge. Donde
> esta el mesclador de margarita? Que podria utilizar uno ahora mismo :-)
>

That's easy for you to say.

[Joerg]

JeffM wrote:
>>> Joerg wrote:
>>>> if it doesn't have to be [EAGLE,]
>>>> there is someone at a company in S.F. that you know :-)
>>>>
>> JeffM wrote:
>>> ...and perhaps she would like to learn another package
>>> beyond PADS.
>>>
> Joerg wrote:
>> Wots wrong with PADS?
>>
> Nothing that I'm aware of
> --except its current corporate ownership.
>
>> Over the last 10 years or so most of my layouts
>> have been done with PADS and I didn't see anything amiss.
>>
> I have no specific gripe against PADS.
> If I was going to advocate for a *replacement* for PADS,
> it certainly wouldn't be in favor of Cadsoft's DRM'd junk.
>

IMHO Eagle is the best CAD right now, or could be, _if_ they had a
hierarchy. Beats me why they don't see that importance.

> My reference was to the Brat
> expanding/enhancing her knowledge/skillset.
> Y'know, making herself more valuable in a lousy labor market.
>

In engineering it isn't lousy. Well, at least not in analog. I was
hoping for a couple weeks off over Christmas. Not gonna happen ...

>>> http://tinyurl.com/TheEAGLE-Virus
>>>
>> Ah, the cruzade ... You and your conspiracy theory :-)
>>
> Knowledge is power. Forewarned is forearmed.
> DRM sucks.
> Companies that treat their paid customers
> like something they need to scrape off their shoe need to die.
> NOW.
>

I am 100% of different opinion. Plus I've not seen one lone case of DRM
issues and I am using Eagle since more than five years. And their
customer support is stellar.

>> An autorouter is usually no good
>>
> You could have stopped there.
>

Not really. I have seen autorouters do acceptable work on massively
parallel slow stuff. You don't really want to route a 256 by 256
crosspoint switch by hand. At least I wouldn't.

>> when it comes to hot stuff.
>>
> I think that part goes without saying.
>
>>> Easily Applicable Graphical Layout Editor.
>>>
>> [And] it is, except for the library editor
>> which really takes some getting used to.
>>
> ...and anyone thinking about re-using someone else's symbols,
> needs to see "DRM", above. Getting bitten in the butt
> then told by the software vendor to go screw yourself
> just leaves me completely cold wrt Cadsoft/EAGLE.
>
> DRM **only** hurts the people who **pay** for products;
> the *actual* pirates all know how to get around it.
> If you're on deadline, EAGLE is **not** the product you want.
>

Then why has it never happened with me or any of several clients who
also use Eagle extensively? Of course, one should only deal with
reputable sources. IMHO that goes without saying.

AFAIK library parts or symbols do not cause issues but chunks of
clandestine schematics can.

>> But the major shortcoming of Eagle is the lack of a hierarchy.
>>
> ...if you've never been bitten in the butt by their DRM.
>

I haven't and I am sure I never will be.

>> They waved it off again for V6
>>
> {Shakes head side to side}
> Just pitiful, Cadsoft.
>
>> which makes me think there is a deeper screw-up
>> in the data structure.
>>
> Pitiful.
> Makes me think of M$'s "security" model.
>
>> So I'll sit out that upgrade as well.
>>
> ...then there's my advice: Don't get *started* with Cadsoft.
> ...or any company that uses DRM and
> treats customers like something they wouldn't want to step in.

They've treated me very nicely.

[JeffM]

Doug White wrote:
>If you are using the free version,
>I thought it was restricted to two layers.
>

Traditionally, a successful crippleware model for them.
It is also restricted to 80mm x 100mm (~3.5" x ~4")
and single-sheet schematics.

You can get much more from (Free Software) KiCAD or gEDA.

>Maybe they have given up on that.
>

Not in your lifetime, dude.
Instead, Cadsoft added DRM to the payware version of EAGLE
and told customers^Wsuckers that when they encounter that,
they are on their own.

[John S]

I agree, Joerg. In all points.

The autorouter worked very well for me. Of course, the parameters have
to be set up properly and I had fits with that at first. I could not
have produced all the boards I have done so far without the AR.

[Joerg]

Strangely, they spelled my family name correctly and that's a difficult
one. Almost anyone botches that but I got used to it. At Guide Dogs I am
registered as Jerry and it seems to take an act of Congress to change
this, so I decided to just live with it.

[lang...@fonz.dk]

I believe you can define net classes in eagle and then specify minium
width
and isolation for nets in and between each class

-Lasse

[lang...@fonz.dk]

On 22 Dec., 01:11, JeffM <jef...@email.com> wrote:
> Doug White wrote:
> >If you are using the free version,
> >I thought it was restricted to two layers.
>
> Traditionally, a successful crippleware model for them.
> It is also restricted to 80mm x 100mm (~3.5" x ~4")
> and single-sheet schematics.

they have a slightly less crippled version called freemium
from element14 (farnell)
I believe it is 4 layers and 4 sheets and you'll need to
renew license every 60 days

>
> You can get much more from (Free Software) KiCAD or gEDA.
>

rs-components have DesignSpark don't think there's any limitations
in that either, and there's scripts that will convert eagle
schematics libraries and boards and it seems to work quite well

> >Maybe they have given up on that.
>
> Not in your lifetime, dude.
> Instead, Cadsoft added DRM to the payware version of EAGLE
> and told customers^Wsuckers that when they encounter that,
> they are on their own.

-Lasse

[Joerg]

JeffM wrote:
> Doug White wrote:
>> If you are using the free version,
>> I thought it was restricted to two layers.
>>
> Traditionally, a successful crippleware model for them.
> It is also restricted to 80mm x 100mm (~3.5" x ~4")
> and single-sheet schematics.
>
> You can get much more from (Free Software) KiCAD or gEDA.
>

I've tried both. IMHO they can't compete (yet). Kicad has an ugly frame
embedded in the code so there is no way to use it professionally. gEDA
has major issues with refdeses in multislot parts. But the fact that it
won't easily work on Windows is the real downside, makes it a niche app,
not so useful for the corporate world.

We need something like Orcad-SDT back but nobody seems to make a CAD
with that robustness. Well, other than Cadsoft. They've botched the
hoerarchy but in all the five years is has never crashed or refused to
open a file. New Orcad, OTOH ...

[...]

[lang...@fonz.dk]

On 21 Dec., 23:39, John Larkin

yeh I think the most usual way of doing it now is to have every layer
the same, some of them just happen to be mostly pours of gnd or supply
Planes that are drawn inverted and all that mess must be a left over
from
some old way of making films or something like that

-Lasse

[Peter Bennett]

On Wed, 21 Dec 2011 15:23:23 -0500, Phil Hobbs
<pcdhSpamM...@electrooptical.net> wrote:

>Thanks for the wisdom on the last newbie question. I managed to finish
>a simple schematic (1 pHEMT, one SiGe bipolar, and one fast op amp--a
>whole 22 parts altogether).
>
>Now for a board layout, and the next question. I figured out how to set
>the design rules to make a four-layer board with two cores, with prepreg
>in between. Now I need to make a ground plane. So far, I've done:
>
>set layer 2 to be net GND, supply plane box checked in the DISPLAY dialogue
>
>POLY GND
>draw the polygon
>autoroute (just for test purposes, honest)
>
>The autoroute fails because it's trying to put everything on layer 1,
>and it ignores the ground plane almost entirely--it routes the grounds,
>and it makes no vias or thermals in the ground plane. Except for
>one--it makes a big hole under the Pin 1 mark on the IC package, which
>is drawn as a wire in the package editor.
>
>How do I get Eagle to recognize the ground plane as a ground plane?
>
>How do I get the autorouter to use more than one layer?
>
>Thanks
>
>Phil Hobbs

I've only used Protel, so this may not apply to Eagle.

However, in Protel, anything you draw on a plane layer is not-copper,
so if I declared Layer 2 as a ground plane, then drew a polygon on it
covering the whole board, I would have _removed_ all the copper on
that layer - obviously, the autorouter would know not to use that
non-copper for ground connections.


--
Peter Bennett, VE7CEI
peterbb (at) telus.net
GPS and NMEA info: http://vancouver-webpages.com/peter
Vancouver Power Squadron: http://vancouver.powersquadron.ca

[John Larkin]

On Wed, 21 Dec 2011 15:56:25 -0800 (PST), JeffM <jef...@email.com>
wrote:

>>>Joerg wrote:
>>>>if it doesn't have to be [EAGLE,]
>>>>there is someone at a company in S.F. that you know :-)
>>>>
>>JeffM wrote:
>>>...and perhaps she would like to learn another package
>>>beyond PADS.
>>>
>Joerg wrote:
>>Wots wrong with PADS?
>>
>Nothing that I'm aware of
>--except its current corporate ownership.
>
>>Over the last 10 years or so most of my layouts
>>have been done with PADS and I didn't see anything amiss.
>>
>I have no specific gripe against PADS.
>If I was going to advocate for a *replacement* for PADS,
>it certainly wouldn't be in favor of Cadsoft's DRM'd junk.
>
>My reference was to the Brat
>expanding/enhancing her knowledge/skillset.
>Y'know, making herself more valuable in a lousy labor market.

She keeps pretty busy, working here, running our web site, coaching
softball, doing a little contract PCB layout. I don't think she wants
to do a huge amount of contract work, probably not enough to buy and
learn a bunch of different layout programs.

John

[John Larkin]

Right. You'd send out the mylars to the photo shop. They would invert
your padmaster layer and expand the pads to make your ground plane,
reinsert the pads, and merge that with a separate sheet that has
little bits of tape that connected up the things you wanted grounded.

What a pain: I don't miss any of that. Checking a modestly complex
board might take two people two days. But then, I did fall in love
once, being one of those two people checking a layout for two days.

John

[Joerg]

The learning has to be in a healthy relation to the expected revenue, of
course. But the buying thing can sometimes be avoided via VPN access.

After having used various systems for the various clients there is
usually a routine that comes in, makes new systems less of an effort.
Like renting a car. "Oh, steering wheel on the other side, ok".

[Phil Hobbs]

That might be it, thanks.

Cheers

Phil "Gradually coming up to speed" Hobbs

[Phil Hobbs]

Thanks. I ponied up the $275 for a one-year STD license.

Cheers

Phil Hobbs

[Martin Riddle]

"Phil Hobbs" <pcdhSpamM...@electrooptical.net> wrote in message
news:4EF2403B...@electrooptical.net...

> Thanks for the wisdom on the last newbie question. I managed to
> finish a simple schematic (1 pHEMT, one SiGe bipolar, and one fast op
> amp--a whole 22 parts altogether).
>
> Now for a board layout, and the next question. I figured out how to
> set the design rules to make a four-layer board with two cores, with
> prepreg in between. Now I need to make a ground plane. So far, I've
> done:
>
> set layer 2 to be net GND, supply plane box checked in the DISPLAY
> dialogue
>
> POLY GND
> draw the polygon
> autoroute (just for test purposes, honest)
>
> The autoroute fails because it's trying to put everything on layer 1,
> and it ignores the ground plane almost entirely--it routes the
> grounds, and it makes no vias or thermals in the ground plane. Except
> for one--it makes a big hole under the Pin 1 mark on the IC package,
> which is drawn as a wire in the package editor.
>
> How do I get Eagle to recognize the ground plane as a ground plane?
>
> How do I get the autorouter to use more than one layer?
>
> Thanks
>
> Phil Hobbs
>

Using a PLOY GND should work.
in 4.16 using the command AUTO, there are preferred directions for the
layers. With N/A meaning not to route on that layer.
Just make sure your gnd layer is not a supply layer.
Click on the layer Display icon and double click the layer that is in
question. If the layer name started with a $ it's treated as a supply
layer. The kick is you can draw a poly on a supply layer and get weird
results.

The eagle help has everything you need.. Just type HELP or HELP layer
Supply Layers

Layers 2...15 are treated as supply layers if their name starts with the
'$' character and there is a signal with an identical name but without
the leading '$'.

Any pads or vias belonging to that signal are implicitly considered
connected by the RATSNEST command and the Autorouter.

Supply layers are viewed "inverted", which means that any objects
visible on such a layer will result in "copper free" areas on the board.
The program automatically generates Thermal and Annulus objects to
connect and isolate pads and vias to/from these layers.

You should not draw any additional objects into a supply layer, except,
for instance, wires along the outlines of the board, which prevent the
copper area from extending to the very edges and thus possibly causing
short circuits through a metal casing or mounting screw. Note that there
are no checks whether a supply layer really connects all pads and vias.
If e. g. a user drawn object isolates a pad that should be connected to
the supply layer, there will be no airwire generated for that (missing)
connection. The same applies if several Annulus symbols form a "ring"
around a Thermal symbol (and would thus completely isolate that pad from
its signal). Also note that the size of the annulus symbols used in a
supply layer is only derived from the value given under "Annulus" in the
"Supply" tab of the Design Rules, and that neither the minimum distances
under "Clearance" nor those in the net classes go into this
calculation.

For a safer and more flexible way of implementing supply layers you
should use the POLYGON command.



Cheers

[JeffM]

>>Doug White wrote:
>>>If you are using the free version,
>>>I thought it was restricted to two layers.
>>>

>JeffM wrote:
>>[...]crippleware[...]

>>You can get much more from (Free Software) KiCAD or gEDA.
>>

Joerg wrote:
>I've tried both. IMHO they can't compete (yet).
>

If you have a teeny tiny project
which will work with Cadsoft's crippleware version,
the Free Software stuff competes easily.
...and if you get one of the 2 EE specialist Linux distro CDs
(there may be even more that are current and unknown to me),
you get both and you don't even have to *install* anything.

>Kicad has an ugly frame embedded in the code
>so there is no way to use it professionally.
>

WRT something that bugs you that much,
for less money than you spent on Cadsoft's DRM'd junk,
you could have HIRED a coder to fix that for you.
...instead of whining.

>gEDA has major issues with refdeses in multislot parts.
>

Yeah, that's not so good.
Again, for less than the purchase price of a closed-source app
from a screw-you company, you could have hired a coder
--or have put a bounty on that bug for the gEDA guys.

>But the fact that it won't easily work on Windows
>

Nonsense. Lots of folks have gEDA running under Windoze.
Children and idiots are -not- the target audience.

>is the real downside, makes it a niche app,
>

...if you're a child or an idiot.
...and the **entire** ECAD market is niche;
that's why is so easily abused by the vendors.

>not so useful for the corporate world.
>

Years back, Terry Porter would post links here
to the output of his gEDA efforts.
He was making plenty of money with the tools even then.

>We need something like Orcad-SDT back
>but nobody seems to make a CAD with that robustness.
>

What is needed is OPEN document standards for EDA.
With all vendors then shooting at the same target,
there would be real competition aka a level playing field.
"Proprietary standards" suck.

>Well, other than Cadsoft. They've botched the [hierarchy]

>but in all the five years is has never crashed
>or refused to open a file.
>

...for you.

>New Orcad, OTOH ...
>
The business model in the ECAD marketplace
is to buy up the competition and knife the baby.
Without OPEN file formats and OPEN standards,
giving money to the payware vendors just finances the abuse.

[Joerg]

JeffM wrote:
>>> Doug White wrote:
>>>> If you are using the free version,
>>>> I thought it was restricted to two layers.
>>>>
>> JeffM wrote:
>>> [...]crippleware[...]
>>> You can get much more from (Free Software) KiCAD or gEDA.
>>>
> Joerg wrote:
>> I've tried both. IMHO they can't compete (yet).
>>
> If you have a teeny tiny project
> which will work with Cadsoft's crippleware version,
> the Free Software stuff competes easily.
> ...and if you get one of the 2 EE specialist Linux distro CDs
> (there may be even more that are current and unknown to me),
> you get both and you don't even have to *install* anything.
>

It's not about install. Install worked fine with both. gEDA inside a VM,
of course.

>> Kicad has an ugly frame embedded in the code
>> so there is no way to use it professionally.
>>
> WRT something that bugs you that much,
> for less money than you spent on Cadsoft's DRM'd junk,
> you could have HIRED a coder to fix that for you.

No, you cannot. Well, maybe in Bangladesh. Plus then you've create a
fork that is incompatible with everyone else's and all future releases.
May be ok for hobby but that won't fly in the business world.


> ...instead of whining.
>

Ever looked at the Cadsoft license prices lately? Engineers often only
need schematic editors because layouts are usually contracted out.
Forgot what I paid since I won't upgrade right now but it was truly
miniscule compared to just about any other commercial CAD package. Beats
me why some shady people still crack it.

>> gEDA has major issues with refdeses in multislot parts.
>>
> Yeah, that's not so good.

It makes it useless for any hotshot analog project where offsets or RF
leakage must be controlled.

> Again, for less than the purchase price of a closed-source app
> from a screw-you company, you could have hired a coder
> --or have put a bounty on that bug for the gEDA guys.
>

No. Do the math. These guy will not work for minimum wage, and they
shouldn't.

>> But the fact that it won't easily work on Windows
>>
> Nonsense. Lots of folks have gEDA running under Windoze.

Like who?

> Children and idiots are -not- the target audience.
>

A user whom I'd consider a real expert and who is very versed in gEDA
has tried. Didn't work. Even one of the gurus in the group said there's
some stuff in gEDA that makes that a real challenge. Better check the
facts before making such statements.

Also, an attitude like "we only cater to the arrived" will always be
unsuccessful in such markets. Ever thought about who's going to be the
next generation? To me, mentoring is a large part of what I consider my
duties to give back to society. Sadly, to some it isn't.

>> is the real downside, makes it a niche app,
>>
> ...if you're a child or an idiot.
> ...and the **entire** ECAD market is niche;
> that's why is so easily abused by the vendors.
>

Nonsense. What's abused here? In the more than two decades that I do
circuit design I always bought CAD packages and used them.

>> not so useful for the corporate world.
>>
> Years back, Terry Porter would post links here
> to the output of his gEDA efforts.
> He was making plenty of money with the tools even then.
>

Sure, there is the occasional small company. Take a look around when you
get into the real corporate America, companies with parking lots the
size of Walmart's.

>> We need something like Orcad-SDT back
>> but nobody seems to make a CAD with that robustness.
>>
> What is needed is OPEN document standards for EDA.
> With all vendors then shooting at the same target,
> there would be real competition aka a level playing field.
> "Proprietary standards" suck.
>

Would be nice. There was this EDIF movement. But other than some nice
gala events and champagne, Perrier water and caviar nothing ever came of
it that was worth writing home about. Ain't gonna happen.

>> Well, other than Cadsoft. They've botched the [hierarchy]
>> but in all the five years is has never crashed
>> or refused to open a file.
>>
> ...for you.
>

Oh no. I've talked with clients about it. Same thing, they felt that
Eagle was of cast-iron robustness.

>> New Orcad, OTOH ...
>>
> The business model in the ECAD marketplace
> is to buy up the competition and knife the baby.

Unfortunately that is true :-(

> Without OPEN file formats and OPEN standards,
> giving money to the payware vendors just finances the abuse.

It would be cool, yes, but I do not see that happen. With the gEDA guys
there is a very noticeable MS-phobia which will keep this otherwise
promising CAD tool in the niche area. Plus they do not seem to believe
in the integrated suite concept yet that's clearly where the market is
going since years.

Kicad could probably be fixed fairly easily but the movers and shakers
do not listen to feedback such as mine. So ...

[Peter Bennett]

On Wed, 21 Dec 2011 21:47:14 -0500, Phil Hobbs

Also, in Protel, I normally drew a wide track around the edge of the
board on the plane layers - this kept the plane copper from extending
to the edge of the board - this could be important, especially if the
board will be mounted in metal guides.

[Joerg]

That should be standard design procedure for all rack cards. I remember
a situation where a card puller handle snapped. So the guy took a big
flat blade screwdriver, reached in ... *PHSSSOOOSH* ... that lit up the
lab pretty good.

[lang...@fonz.dk]

On 22 Dec., 19:07, Peter Bennett <pete...@somewhere.invalid> wrote:
> On Wed, 21 Dec 2011 21:47:14 -0500, Phil Hobbs
>
>
>
>
>
>
>
>
>
> <pcdhSpamMeSensel...@electrooptical.net> wrote:
> >On 12/21/2011 08:21 PM, Peter Bennett wrote:
> >> On Wed, 21 Dec 2011 15:23:23 -0500, Phil Hobbs

> >> <pcdhSpamMeSensel...@electrooptical.net>  wrote:

In eagle the isolation set for pours also goes for pour to outline
same for not plated holes for screws etc.

-Lasse

[John S]

As usual, I forgot the smiley face. Sorry. :-)

[John S]

Joerg -

JeffM was, in his opinion, screwed by CadSoft some years ago. He has a
vendetta and looks for any post where he can jump in and post his link
to his years-old complaint. You will get nowhere by replying to him.
Your comments about happy customers are right on. I've used Eagle for
about the last 10 years and have had no problems that were not handled
by their tech support. Stick to your guns.

Cheers,
John S

[John S]

IIRC, the edge of the board can be specified in Eagle so that what you
suggest is not necessary.

John S

[Nico Coesel]

That sounds like a very odd and obfustigated way to get a copper pour.
AFAIK you can define copper pours in most programs by drawing a
polygon. In some software packages (Orcad Layout comes to mind) you
can define a layer as a plane so the layer if filled with copper by
default and anything you 'draw' in it is anti-copper.

--
Failure does not prove something is impossible, failure simply
indicates you are not using the right tools...
nico@nctdevpuntnl (punt=.)
--------------------------------------------------------------

[Nico Coesel]

Joerg <inv...@invalid.invalid> wrote:

>JeffM wrote:
>>>> Doug White wrote:
>>>>> If you are using the free version,
>>>>> I thought it was restricted to two layers.
>>>>>
>

>> Without OPEN file formats and OPEN standards,
>> giving money to the payware vendors just finances the abuse.
>
>
>It would be cool, yes, but I do not see that happen. With the gEDA guys
>there is a very noticeable MS-phobia which will keep this otherwise
>promising CAD tool in the niche area. Plus they do not seem to believe
>in the integrated suite concept yet that's clearly where the market is
>going since years.

One of my customers used Geda and PCB to create a design. IMHO a paid
CAD package is more productive. Jeff's warnings made me not buy Eagle
but spend the cash on a second hand CAD package instead.

>Kicad could probably be fixed fairly easily but the movers and shakers
>do not listen to feedback such as mine. So ...

I tried Kicad but I'm not impressed.

[Nico Coesel]

Joerg <inv...@invalid.invalid> wrote:

>Forgot what I paid since I won't upgrade right now but it was truly
>miniscule compared to just about any other commercial CAD package. Beats
>me why some shady people still crack it.

I thank those people for not having to deal with dongles, tedious
registration schemes, node locks, etc. I always use the cracked
version and leave the original on the shelf. I have a rule: if
software has some kind of registration/licensing scheme I won't buy it
unless there is a cracked version. I don't want to be punished or held
on a leash when buying software.

[Joerg]

Nico Coesel wrote:
> Joerg <inv...@invalid.invalid> wrote:
>
>> Forgot what I paid since I won't upgrade right now but it was truly
>> miniscule compared to just about any other commercial CAD package. Beats
>> me why some shady people still crack it.
>
> I thank those people for not having to deal with dongles, tedious

> registration schemes, node locks, etc. ...


Amen!


> ... I always use the cracked

> version and leave the original on the shelf. I have a rule: if
> software has some kind of registration/licensing scheme I won't buy it
> unless there is a cracked version. I don't want to be punished or held
> on a leash when buying software.
>

I've only bought two of those kinds, and only because of a client.

Regarding Kicad I actually like it a lot. It is a very fine piece of
software. Except for that ugly frame that cannot be removed or replaced
by a more professional one. That relegates this otherwise very fine
software into the hobby corner. The gurus seem to not want to notice, or
care. Oh well, I will stay with Eagle then for the time being. The only
gripe about that one is lack of hierarchy, else I wouldn't even be
looking for any alternatives .

[Joerg]

Nico Coesel wrote:
> Joerg <inv...@invalid.invalid> wrote:
>
>> JeffM wrote:
>>>>> Doug White wrote:
>>>>>> If you are using the free version,
>>>>>> I thought it was restricted to two layers.
>>>>>>
>>> Without OPEN file formats and OPEN standards,
>>> giving money to the payware vendors just finances the abuse.
>>
>> It would be cool, yes, but I do not see that happen. With the gEDA guys
>> there is a very noticeable MS-phobia which will keep this otherwise
>> promising CAD tool in the niche area. Plus they do not seem to believe
>> in the integrated suite concept yet that's clearly where the market is
>> going since years.
>
> One of my customers used Geda and PCB to create a design. IMHO a paid
> CAD package is more productive. Jeff's warnings made me not buy Eagle
> but spend the cash on a second hand CAD package instead.
>

Don't worry. Nothing bad happens if you do not exchange schematics with
shady folks who use cracked software. Since I only use it for business
this has never happened to me.

However, Eagle cannot do hierarchical schematics and that is a major
flaw if you do very large projects. Not so much in my case because most
clients use me to only design the really difficult chunks of a project.
RF, nanoscond stuff, low noise, things like that. So my schematics
rarely exceed 4-5 sheets which can be handled sans hierarchy. Designing,
for example, a whole ultrasound machine on Eagle would be next to
impossible.

>> Kicad could probably be fixed fairly easily but the movers and shakers
>> do not listen to feedback such as mine. So ...
>
> I tried Kicad but I'm not impressed.
>

Other than that ugly fixed frame, what didn't you like about it?

[Rich Webb]

On Fri, 23 Dec 2011 07:58:35 -0800, Joerg <inv...@invalid.invalid>
wrote:

When I need to baseline or checkpoint a Kicad schematic, or otherwise
produce one with the approved frame, I just do a plot to DXF with the
"print page references" (e.g., the frame) un-checked, and then suck that
into CAD for framing, naming, etc..

Everybody can read DXF/DWG or a PDF printed from CAD and I can continue
on with the "working copies" in Kicad. One nice thing about the format
is that I can stick rcs tags ($Id$ or $Revision$) into the frame and
have them automatically updated by rcs.

--
Rich Webb Norfolk, VA

[Nico Coesel]

Joerg <inv...@invalid.invalid> wrote:

>Nico Coesel wrote:
>> Joerg <inv...@invalid.invalid> wrote:
>>
>>> JeffM wrote:
>>>>>> Doug White wrote:
>>>>>>> If you are using the free version,
>>>>>>> I thought it was restricted to two layers.
>>>>>>>
>>>> Without OPEN file formats and OPEN standards,
>>>> giving money to the payware vendors just finances the abuse.
>>>
>>> It would be cool, yes, but I do not see that happen. With the gEDA guys
>>> there is a very noticeable MS-phobia which will keep this otherwise

>>> Kicad could probably be fixed fairly easily but the movers and shakers
>>> do not listen to feedback such as mine. So ...
>>
>> I tried Kicad but I'm not impressed.
>>
>
>Other than that ugly fixed frame, what didn't you like about it?

I tried the PCB package. I didn't like the way you have to edit
traces.

[Joerg]

Nico Coesel wrote:
> Joerg <inv...@invalid.invalid> wrote:
>
>> Nico Coesel wrote:
>>> Joerg <inv...@invalid.invalid> wrote:
>>>
>>>> JeffM wrote:
>>>>>>> Doug White wrote:
>>>>>>>> If you are using the free version,
>>>>>>>> I thought it was restricted to two layers.
>>>>>>>>
>>>>> Without OPEN file formats and OPEN standards,
>>>>> giving money to the payware vendors just finances the abuse.
>>>> It would be cool, yes, but I do not see that happen. With the gEDA guys
>>>> there is a very noticeable MS-phobia which will keep this otherwise
>>>> Kicad could probably be fixed fairly easily but the movers and shakers
>>>> do not listen to feedback such as mine. So ...
>>> I tried Kicad but I'm not impressed.
>>>
>> Other than that ugly fixed frame, what didn't you like about it?
>
> I tried the PCB package. I didn't like the way you have to edit
> traces.
>

Ok, I usually don't do layouts and mostly I looked at the schematic editor.

[Joerg]

> on with the "working copies" in Kicad. ...


DXF/DWG no, but PDF yes. However, I need to be able to edit a custom
title block right there in the schematic. Having to roach one on and
edit as an "afterthought" is kludgy, and in some highly regulated
markets very much frowned upon by the agencies that audit us. Because it
is de-facto separated from the data file.


> ... One nice thing about the format

> is that I can stick rcs tags ($Id$ or $Revision$) into the frame and
> have them automatically updated by rcs.
>

That is nice. But it won't help if one cannot have a frame that matches
the corporate standard. Many of us have to work by standard operating
procedures and then this kind of software can be a no-no.

[Peter Bennett]

On Fri, 23 Dec 2011 11:43:53 GMT, ni...@puntnl.niks (Nico Coesel)
wrote:

I think you misunderstood me, and/or didn't read my first post.

In Protel, you can define a layer as a plane (like Orcad, I expect),
but the copper plane extends to the horizon. You draw a wide track on
the board edge on the plane layer to keep the copper away from the
actual board edge.

You can also place filled polygons on the normal routing layers if you
want a large copper area there. If you place a filled polygon on a
plane layer, you get a hole in the plane.

[Baron]

Nico Coesel Inscribed thus:

> One of my customers used Geda and PCB to create a design. IMHO a paid
> CAD package is more productive. Jeff's warnings made me not buy Eagle
> but spend the cash on a second hand CAD package instead.

Jeff has a grudge ! In your case he achieved his aim...
If it was a legitimate complaint there would be dozens of people
complaining, but there aren't. In fact its just the opposite, many
satisfied users.

--
Best Regards:
Baron.

[Nico Coesel]

Perhaps, but when there is smoke there is fire. Nobody has provided
any solid proof that Jeff is telling lies. Besides if he is telling
lies then he would have been sued by the owners of Eagle for slander a
long time ago.

Sometimes I need to push software or equipment to its limits and that
is where lesser products (even the ones with many happy users) fail.
When it comes to the risk of losing productivity (wasting time) I
don't take any chances.

[Nico Coesel]

I read it and I already had a feeling I pressed the send button too
quickly.

>In Protel, you can define a layer as a plane (like Orcad, I expect),
>but the copper plane extends to the horizon. You draw a wide track on
>the board edge on the plane layer to keep the copper away from the
>actual board edge.
>
>You can also place filled polygons on the normal routing layers if you
>want a large copper area there. If you place a filled polygon on a
>plane layer, you get a hole in the plane.

Orcad Layout has a similar feature. I think I used it once on a PCB
but I have never used it since. Its not very usefull because it offers
very little control over where the copper goes. In most of my PCBs I
can't use a single plane anyway.

[k...@att.bizzzzzzzzzzzz]

If you only do the high-speed sections, how do you integrate your designs into
the larger boards?

...almost wishing for OrCAD again. <sniff>

[Joerg]

The client transcribes my schematic into theirs. Has to happen almost
regardless of which CAD system I use because there does not exist any
common standard but there are a dozen or so CAD systems in widespread
use. EDIF was just a big joke.

Sometimes I work on their CAD system.

> ...almost wishing for OrCAD again. <sniff>

Same here ... <sniffle, sigh>

[John Devereux]

Baron <ba...@linuxmaniac.net> writes:

> Nico Coesel Inscribed thus:
>
>> One of my customers used Geda and PCB to create a design. IMHO a paid
>> CAD package is more productive. Jeff's warnings made me not buy Eagle
>> but spend the cash on a second hand CAD package instead.
>
> Jeff has a grudge ! In your case he achieved his aim...

I agree he has a grudge and he has been jumping all over any mention of
Eagle with this tale.

And there is nothing wrong with that! I appreciate it.

I have my own List of companies I will not deal with. I don't have the
time or the energy to sue them or even write letters to the complaints
department or whatever. But I can not deal with them and I can take
every opportunity to tell people about them when their name is
mentioned.

Slagging off companies on the internet is one of the few practical
methods of redress. How else are we supposed to discourage this sort of
high-handed contempt for legitimate buyers of their products?

Deliberately and permanantly breaking the design files of legitimate
users because they incorporate a circuit fragment from what turned out
to be a pirated copy? Years after the fact after an update?

Yes this would rarely happen in the corporate environment. So what?
Eagle is (was?) squarely aimed at the hobbiest/amateur user where such
sharing is not at all unlikely, look at all the LTSpice schematics that
get shared here. What would people here think if a rogue circuit posted
here could silently "infect" your installation, so that years later
after an update all your design files suddenly become permanently and
irretrievably useless? Not a by a random virus, but because of a
deliberate strategy by the people who sold you the program?

> If it was a legitimate complaint there would be dozens of people
> complaining, but there aren't. In fact its just the opposite, many
> satisfied users.

--

John Devereux

[Jamie M]

On 12/20/2011 11:39 AM, Phil Hobbs wrote:
> I finally bit the bullet and got a copy of Eagle, because I need to do a
> bunch of small proto boards. Initial impressions are positive, mostly
> because it has a command line at the ready. Score.
>
> The first device I tried creating is an Avago ATF35143 pHEMT, which
> comes in a SC70-4 package with the source connected to pins 2 and 4.
>
> There is no obvious way to tell Eagle that both 2 and 4 are connected to
> the source.
>
> What's the right way to do this?
>
> Thanks
>
> Phil Hobbs
>

Hi Phil,

I've been using eagle for about 10 years but never use the command
line! :) I know this was answered but I wouldn't recommend using the
'@' symbol to distinguish between the two source pins, usually I just
would name them "source1" and source2" etc, this is just my personal
preference since it keeps all pin info available.

ps. if you need a contractor to do eagle cad I would be interested!

cheers,
Jamie

[k...@att.bizzzzzzzzzzzz]

Or you use the same software as your client. This sorta negates any advantage
of your software having hierarchy, though, since you're stuck at the lowest
common denominator. EDIF works for what it was intended. Pretty pictures
ain't it.

>Sometimes I work on their CAD system.

Have you ever looked at their license agreement? Cadence doesn't allow
off-site contractors to use the license.

>> ...almost wishing for OrCAD again. <sniff>
>
>
>Same here ... <sniffle, sigh>

I thought I'd never have anything nice to say about OrCAD.

[Joerg]

> common denominator. EDIF works for what it was intended. ...


Huh? So what good does it do?


> ... Pretty pictures ain't it.
>

No, the intention was that CAD data becomes exchangeable between CAD
system. That clearly did not materialize.

>> Sometimes I work on their CAD system.
>
> Have you ever looked at their license agreement? Cadence doesn't allow
> off-site contractors to use the license.
>

I know. That's why I had to rent a license earlier this year. The reason
was not me being a consultant but because the company was not in the US
and they obviously have the ancient turf-protection sales system.

>>> ...almost wishing for OrCAD again. <sniff>
>>
>> Same here ... <sniffle, sigh>
>
> I thought I'd never have anything nice to say about OrCAD.

Not about the new Orcad, I personally would never buy that. It pretty
much broke the record in the number of crashes per week on my computer.
Orcad-SDT, in contrast, was of cast-iron quality. Then they were bought
and the new owners appear to have broken it. Happens a lot in the world
of software.

[Baron]

John Devereux Inscribed thus:

> Baron <ba...@linuxmaniac.net> writes:
>
>> Nico Coesel Inscribed thus:
>>
>>> One of my customers used Geda and PCB to create a design. IMHO a
>>> paid CAD package is more productive. Jeff's warnings made me not buy
>>> Eagle but spend the cash on a second hand CAD package instead.
>>
>> Jeff has a grudge ! In your case he achieved his aim...
>
> I agree he has a grudge and he has been jumping all over any mention
> of Eagle with this tale.
>
> And there is nothing wrong with that! I appreciate it.

If you are going to slag a company off its only fair to tell both sides
of the tale. Jeff isn't going to admit that he was lazy or dishonest
in the first place.

> I have my own List of companies I will not deal with. I don't have the
> time or the energy to sue them or even write letters to the complaints
> department or whatever. But I can not deal with them and I can take
> every opportunity to tell people about them when their name is
> mentioned.

So do I ! But I don't make a career out of it.

> Slagging off companies on the internet is one of the few practical
> methods of redress. How else are we supposed to discourage this sort
> of high-handed contempt for legitimate buyers of their products?

If there are good grounds for doing so, fine.

> Deliberately and permanantly breaking the design files of legitimate
> users because they incorporate a circuit fragment from what turned out
> to be a pirated copy? Years after the fact after an update?

I've used many circuit fragments from various unaccountable sources
without any issues what so ever ! So I find Jeff's complaint
as "creating a bandwagon" !

> Yes this would rarely happen in the corporate environment. So what?
> Eagle is (was?) squarely aimed at the hobbiest/amateur user where such
> sharing is not at all unlikely, look at all the LTSpice schematics
> that get shared here. What would people here think if a rogue circuit
> posted here could silently "infect" your installation, so that years
> later after an update all your design files suddenly become
> permanently and irretrievably useless? Not a by a random virus, but
> because of a deliberate strategy by the people who sold you the
> program?

I've seen no evidence of a deliberate strategy, but if it has occurred
because of a side effect of protecting intellectual property, then that
is very unfortunate ! I can understand Jeff's angst.

>> If it was a legitimate complaint there would be dozens of people
>> complaining, but there aren't. In fact its just the opposite, many
>> satisfied users.
>

Seasons Greetings to All.
--
Best Regards:
Baron.

[JeffM]

Baron wrote:
>Jeff isn't going to admit
>that he was lazy or dishonest in the first place.
>

Eat shit and die, asswipe.
If you're going to comment on the topic,
at least become informed about what the facts are.
Ignorant dumbass.

[Baron]

JeffM Inscribed thus:

Point proved !

--
Best Regards:
Baron.

[John Devereux]

Baron <ba...@linuxmaniac.net> writes:

> John Devereux Inscribed thus:
>
>> Baron <ba...@linuxmaniac.net> writes:
>>
>>> Nico Coesel Inscribed thus:
>>>
>>>> One of my customers used Geda and PCB to create a design. IMHO a
>>>> paid CAD package is more productive. Jeff's warnings made me not buy
>>>> Eagle but spend the cash on a second hand CAD package instead.
>>>
>>> Jeff has a grudge ! In your case he achieved his aim...
>>
>> I agree he has a grudge and he has been jumping all over any mention
>> of Eagle with this tale.
>>
>> And there is nothing wrong with that! I appreciate it.
>
> If you are going to slag a company off its only fair to tell both sides
> of the tale. Jeff isn't going to admit that he was lazy or dishonest
> in the first place.

(My rant was not aimed at you particularly by the way) :)

IIRC I don't actually think Jeff was even directly affected, let alone
"lazy" or "dishonest". So that is uncalled for.

>> I have my own List of companies I will not deal with. I don't have the
>> time or the energy to sue them or even write letters to the complaints
>> department or whatever. But I can not deal with them and I can take
>> every opportunity to tell people about them when their name is
>> mentioned.
>
> So do I ! But I don't make a career out of it.
>
>> Slagging off companies on the internet is one of the few practical
>> methods of redress. How else are we supposed to discourage this sort
>> of high-handed contempt for legitimate buyers of their products?
>
> If there are good grounds for doing so, fine.
>
>> Deliberately and permanantly breaking the design files of legitimate
>> users because they incorporate a circuit fragment from what turned out
>> to be a pirated copy? Years after the fact after an update?
>
> I've used many circuit fragments from various unaccountable sources
> without any issues what so ever ! So I find Jeff's complaint
> as "creating a bandwagon" !

Actually to me this supports the argument that the companies behaviour
is reprehensible. There *are* people that, in good faith, use circuit
fragments from anaccountable sources. What would you think if the next
update rendered all those designs permanenly useless?

>> Yes this would rarely happen in the corporate environment. So what?
>> Eagle is (was?) squarely aimed at the hobbiest/amateur user where such
>> sharing is not at all unlikely, look at all the LTSpice schematics
>> that get shared here. What would people here think if a rogue circuit
>> posted here could silently "infect" your installation, so that years
>> later after an update all your design files suddenly become
>> permanently and irretrievably useless? Not a by a random virus, but
>> because of a deliberate strategy by the people who sold you the
>> program?
>
> I've seen no evidence of a deliberate strategy, but if it has occurred
> because of a side effect of protecting intellectual property, then that
> is very unfortunate ! I can understand Jeff's angst.
>
>>> If it was a legitimate complaint there would be dozens of people
>>> complaining, but there aren't. In fact its just the opposite, many
>>> satisfied users.
>>
>
> Seasons Greetings to All.

Likewise!

--

John Devereux

[Baron]

John Devereux Inscribed thus:

> Baron <ba...@linuxmaniac.net> writes:
>
>> John Devereux Inscribed thus:
>>
>>> Baron <ba...@linuxmaniac.net> writes:
>>>
>>>> Nico Coesel Inscribed thus:
>>>>
>>>>> One of my customers used Geda and PCB to create a design. IMHO a
>>>>> paid CAD package is more productive. Jeff's warnings made me not
>>>>> buy Eagle but spend the cash on a second hand CAD package instead.
>>>>
>>>> Jeff has a grudge ! In your case he achieved his aim...
>>>
>>> I agree he has a grudge and he has been jumping all over any mention
>>> of Eagle with this tale.
>>>
>>> And there is nothing wrong with that! I appreciate it.
>>
>> If you are going to slag a company off its only fair to tell both
>> sides of the tale. Jeff isn't going to admit that he was lazy or
>> dishonest in the first place.
>
> (My rant was not aimed at you particularly by the way) :)

I understood that.

> IIRC I don't actually think Jeff was even directly affected, let alone
> "lazy" or "dishonest". So that is uncalled for.
>
>
>>> I have my own List of companies I will not deal with. I don't have
>>> the time or the energy to sue them or even write letters to the
>>> complaints department or whatever. But I can not deal with them and
>>> I can take every opportunity to tell people about them when their
>>> name is mentioned.
>>
>> So do I ! But I don't make a career out of it.
>>
>>> Slagging off companies on the internet is one of the few practical
>>> methods of redress. How else are we supposed to discourage this sort
>>> of high-handed contempt for legitimate buyers of their products?
>>
>> If there are good grounds for doing so, fine.
>>
>>> Deliberately and permanantly breaking the design files of legitimate
>>> users because they incorporate a circuit fragment from what turned
>>> out to be a pirated copy? Years after the fact after an update?
>>
>> I've used many circuit fragments from various unaccountable sources
>> without any issues what so ever ! So I find Jeff's complaint
>> as "creating a bandwagon" !
>
> Actually to me this supports the argument that the companies behaviour
> is reprehensible. There *are* people that, in good faith, use circuit
> fragments from anaccountable sources. What would you think if the next
> update rendered all those designs permanenly useless?

Part of this seems very odd for a product that, despite various
limitations can be obtained and used for free ! I see that the file
format can be taken and converted for other applications. So I'm more
inclined to belive that there were other factors involved.

>>> Yes this would rarely happen in the corporate environment. So what?
>>> Eagle is (was?) squarely aimed at the hobbiest/amateur user where
>>> such sharing is not at all unlikely, look at all the LTSpice
>>> schematics that get shared here. What would people here think if a
>>> rogue circuit posted here could silently "infect" your installation,
>>> so that years later after an update all your design files suddenly
>>> become permanently and irretrievably useless? Not a by a random
>>> virus, but because of a deliberate strategy by the people who sold
>>> you the program?
>>
>> I've seen no evidence of a deliberate strategy, but if it has
>> occurred because of a side effect of protecting intellectual
>> property, then that is very unfortunate ! I can understand Jeff's
>> angst.
>>
>>>> If it was a legitimate complaint there would be dozens of people
>>>> complaining, but there aren't. In fact its just the opposite, many
>>>> satisfied users.
>>>
>>
>> Seasons Greetings to All.
>
> Likewise!
>

Thanks.

--
Best Regards:
Baron.

[JeffM]

>JeffM wrote:
>>If you're going to comment on the topic,
>>at least become informed about what the facts are.
>>Ignorant dumbass.
>>

Baron wrote:
>Point proved !
>
True. You're as ignorant as you were before.
Try to put words in my mouth that I didn't say
and I'm coming after you, shithead.

...and John S is another one who makes it up as he goes along.

[k...@att.bizzzzzzzzzzzz]

It's a netlist transport format. If all you want is to move a netlist, EDIF
is the way to go. Chip makers use it as you would a Gerber.

>> ... Pretty pictures ain't it.
>>
>
>No, the intention was that CAD data becomes exchangeable between CAD
>system. That clearly did not materialize.

Maybe that was your wish. No one else had that fantasy, though. ;-)

>>> Sometimes I work on their CAD system.
>>
>> Have you ever looked at their license agreement? Cadence doesn't allow
>> off-site contractors to use the license.
>>
>
>I know. That's why I had to rent a license earlier this year. The reason
>was not me being a consultant but because the company was not in the US
>and they obviously have the ancient turf-protection sales system.
>
>
>>>> ...almost wishing for OrCAD again. <sniff>
>>>
>>> Same here ... <sniffle, sigh>
>>
>> I thought I'd never have anything nice to say about OrCAD.
>
>
>Not about the new Orcad, I personally would never buy that. It pretty
>much broke the record in the number of crashes per week on my computer.

...and that's its most enduring feature. ;-)

>Orcad-SDT, in contrast, was of cast-iron quality. Then they were bought
>and the new owners appear to have broken it. Happens a lot in the world
>of software.

Not just software. "Buy it to bury it." ...except they can't even do that
right. I'm learning Zuken, these days. What an absolute nightmare, compared
to OrCAD. The Germans are *nutz*. Well, at least it doesn't crash, much.

[Joerg]

There we use GDS-II, probably goes all the way back to the days I wore
diapers.

A common format just for netlisting isn't very useful, I never felt the
urge for a standard there. Typically I spool out a PADS netlist and that
can be read in by almost any layout software.

>>> ... Pretty pictures ain't it.
>>>
>> No, the intention was that CAD data becomes exchangeable between CAD
>> system. That clearly did not materialize.
>
> Maybe that was your wish. No one else had that fantasy, though. ;-)
>

That goal was all over the trade publications back then. I never
believed it would come to fruition though, and it didn't.

>>>> Sometimes I work on their CAD system.
>>> Have you ever looked at their license agreement? Cadence doesn't allow
>>> off-site contractors to use the license.
>>>
>> I know. That's why I had to rent a license earlier this year. The reason
>> was not me being a consultant but because the company was not in the US
>> and they obviously have the ancient turf-protection sales system.
>>
>>
>>>>> ...almost wishing for OrCAD again. <sniff>
>>>> Same here ... <sniffle, sigh>
>>> I thought I'd never have anything nice to say about OrCAD.
>>
>> Not about the new Orcad, I personally would never buy that. It pretty
>> much broke the record in the number of crashes per week on my computer.
>
> ...and that's its most enduring feature. ;-)
>

I still remember a support call where finally someone on their side
exclaimed "I can't believe this is happening!".

>> Orcad-SDT, in contrast, was of cast-iron quality. Then they were bought
>> and the new owners appear to have broken it. Happens a lot in the world
>> of software.
>
> Not just software. "Buy it to bury it." ...except they can't even do that
> right. I'm learning Zuken, these days. What an absolute nightmare, compared
> to OrCAD. The Germans are *nutz*. Well, at least it doesn't crash, much.

I thought that's a Japanese CAD system. German software is usually
pretty good, like Eagle which never crashes. The marketing side over
there is often rather weird though. I will never understand why Cadsoft
isn't going more after corporate users where they could sell dozens of
licenses in one fell swoop. Without a hierarchy they are leaving tons of
money on the table.

[k...@att.bizzzzzzzzzzzz]

Tell chip makers that! EDIF *was* our product. FPGA software uses EDIF, as
well.

>>>> ... Pretty pictures ain't it.
>>>>
>>> No, the intention was that CAD data becomes exchangeable between CAD
>>> system. That clearly did not materialize.
>>
>> Maybe that was your wish. No one else had that fantasy, though. ;-)
>>
>
>That goal was all over the trade publications back then. I never
>believed it would come to fruition though, and it didn't.

You gotta stop reading that crap.

trade magazines ~= New York Times

No intelligence there.

>>>>> Sometimes I work on their CAD system.
>>>> Have you ever looked at their license agreement? Cadence doesn't allow
>>>> off-site contractors to use the license.
>>>>
>>> I know. That's why I had to rent a license earlier this year. The reason
>>> was not me being a consultant but because the company was not in the US
>>> and they obviously have the ancient turf-protection sales system.
>>>
>>>
>>>>>> ...almost wishing for OrCAD again. <sniff>
>>>>> Same here ... <sniffle, sigh>
>>>> I thought I'd never have anything nice to say about OrCAD.
>>>
>>> Not about the new Orcad, I personally would never buy that. It pretty
>>> much broke the record in the number of crashes per week on my computer.
>>
>> ...and that's its most enduring feature. ;-)
>>
>
>I still remember a support call where finally someone on their side
>exclaimed "I can't believe this is happening!".

I could make 16.1 crash at will. Simply select good chunk of a page, and
drag. Sometimes one component was enough but half a page would do it every
time. 16.3 *mostly* fixed that. Perhaps they didn't want the problem so
easily reproduced.

>>> Orcad-SDT, in contrast, was of cast-iron quality. Then they were bought
>>> and the new owners appear to have broken it. Happens a lot in the world
>>> of software.
>>
>> Not just software. "Buy it to bury it." ...except they can't even do that
>> right. I'm learning Zuken, these days. What an absolute nightmare, compared
>> to OrCAD. The Germans are *nutz*. Well, at least it doesn't crash, much.
>
>
>I thought that's a Japanese CAD system.

I hadn't actually looked. It's starting to make a *whole* lot more sense (the
Japanese are ;).

>German software is usually
>pretty good, like Eagle which never crashes. The marketing side over
>there is often rather weird though. I will never understand why Cadsoft
>isn't going more after corporate users where they could sell dozens of
>licenses in one fell swoop. Without a hierarchy they are leaving tons of
>money on the table.

Hierarchy? I'd be happy to be able to print more than one page at a time. :-(

[John S]

Whoa! Make up wot? I've seen your complaints now for years. Same old
story. I never said that you were lying. I believe your story.

Now, show me where I made something up about you, Mr. Useless Scum Bag.

[Joerg]

Then why do ours always use GDS-II? FPGA stuff is usually highly
proprietary to the respective product line, I wouldn't know what would
be exchangeable or standardized there. The only thing you have is
conversion services, in case your volume goes up and you want it all
poured into an ASIC.

The whole sob story is summed up here and the word that, not
surprisingly, darts out is "problem":

http://en.wikipedia.org/wiki/EDIF

Quote "The vendor companies did not always feel it important to allocate
many resources to EDIF products, even if they sold a large number of
them. There were several stories of active products with virtually
no-one to maintain them for years. User complaints were merely gathered
and prioritized. The harder it became to export customer data to EDIF,
the more the vendors seemed to like it".

>>>>> ... Pretty pictures ain't it.
>>>>>
>>>> No, the intention was that CAD data becomes exchangeable between CAD
>>>> system. That clearly did not materialize.
>>> Maybe that was your wish. No one else had that fantasy, though. ;-)
>>>
>> That goal was all over the trade publications back then. I never
>> believed it would come to fruition though, and it didn't.
>
> You gotta stop reading that crap.
>
> trade magazines ~= New York Times
>
> No intelligence there.
>

You don't ever read EETimes, EDN and stuff? I don't spend a lot of time
there but occasionally it nets me a hint to a product I might otherwise
have missed because it was geared towards a very different market.

>>>>>> Sometimes I work on their CAD system.
>>>>> Have you ever looked at their license agreement? Cadence doesn't allow
>>>>> off-site contractors to use the license.
>>>>>
>>>> I know. That's why I had to rent a license earlier this year. The reason
>>>> was not me being a consultant but because the company was not in the US
>>>> and they obviously have the ancient turf-protection sales system.
>>>>
>>>>
>>>>>>> ...almost wishing for OrCAD again. <sniff>
>>>>>> Same here ... <sniffle, sigh>
>>>>> I thought I'd never have anything nice to say about OrCAD.
>>>> Not about the new Orcad, I personally would never buy that. It pretty
>>>> much broke the record in the number of crashes per week on my computer.
>>> ...and that's its most enduring feature. ;-)
>>>
>> I still remember a support call where finally someone on their side
>> exclaimed "I can't believe this is happening!".
>
> I could make 16.1 crash at will. Simply select good chunk of a page, and
> drag. Sometimes one component was enough but half a page would do it every
> time. 16.3 *mostly* fixed that. Perhaps they didn't want the problem so
> easily reproduced.
>

I crashed it several times a day using integrated PSpice.

>>>> Orcad-SDT, in contrast, was of cast-iron quality. Then they were bought
>>>> and the new owners appear to have broken it. Happens a lot in the world
>>>> of software.
>>> Not just software. "Buy it to bury it." ...except they can't even do that
>>> right. I'm learning Zuken, these days. What an absolute nightmare, compared
>>> to OrCAD. The Germans are *nutz*. Well, at least it doesn't crash, much.
>>
>> I thought that's a Japanese CAD system.
>
> I hadn't actually looked. It's starting to make a *whole* lot more sense (the
> Japanese are ;).
>
>> German software is usually
>> pretty good, like Eagle which never crashes. The marketing side over
>> there is often rather weird though. I will never understand why Cadsoft
>> isn't going more after corporate users where they could sell dozens of
>> licenses in one fell swoop. Without a hierarchy they are leaving tons of
>> money on the table.
>
> Hierarchy? I'd be happy to be able to print more than one page at a time. :-(

Ugh. That sounds bad. That software goes on my "not to do" list :-)

[JeffM]

>JeffM wrote:
>>...and John S is another one who makes it up as he goes along.
>>

John S wrote:
>Whoa! Make up wot? I've seen your complaints now for years.
>

Reading comprehension problems, then?
Lousy memory?
Never actually clicked the link I always post?

>Same old story. I never said that you were lying.
>

Right. Instead, you made up your own narrative and claimed it is
mine.

>I believe your story.
>
You'd have to KNOW it first.

>Now, show me where I made something up about you,
>Mr. Useless Scum Bag.
>

news:jd0pjc$sq9$1...@dont-email.me
http://groups.google.com/group/sci.electronics.design/msg/2f5ecdd92d4b4ce2
:JeffM was, in his opinion, screwed by CadSoft some years ago.
:
Fabricated out of whole cloth by you.

Cadsoft never got the opportunity to abuse me with their DRM.
I am, however, VERY angry that I had previously been responsible
for the scumbags getting some money from my previous company.

Surreptitious bombs purposely put into software by its vendor
just makes me see red.
When that is in a tool that could blow up in your face
when you're on deadline, the steam comes out my ears.
When the company then tells you
"Go fuck yourself, Mr. Paid-Up customer", that's the limit.
Anyone who endorses that kind of corporate behavior
would also sell out to any slimeball who is the highest bidder.

[josephkk]

On Wed, 21 Dec 2011 13:56:55 -0800, Joerg <inv...@invalid.invalid> wrote:

>JeffM wrote:

>> Joerg wrote:
>>> if it doesn't have to be [EAGLE]{1}[,]
>>> there is someone at a company in S.F. that you know :-)
>>>
>> ...and perhaps she would like to learn another package
>> beyond PADS.
>>
>
>Wots wrong with PADS? Over the last 10 years or so most of my layouts
>have been done with PADS and I didn't see anything amiss.
>
>But I am not picky about details. Like with cars. Dealer asks me what
>color I like and I tell him it doesn't matter ... "Say WHAT?!"
>
>
>> ...and for other EAGLE neophites considering that package:
>> http://tinyurl.com/TheEAGLE-Virus
>>
>
>Ah, the cruzade ... You and your conspiracy theory :-)
>
>
>> Now, for a show of hands here
>> of anyone who ever got useful results from an autorouter.
>> ...particularly on a project with more than 22 components.
>
>
>Nay.
>
>
>> ...especially with an ECAD package that cost less than $5k.
>
>
>Don't matter. An autorouter is usually no good when it comes to hot stuff.
>
>
>> .
>> {1} An initialism for Easily Applicable Graphical Layout Editor.
>
>
>An it is, except for the library editor which really takes some getting
>used to. But the major shortcoming of Eagle is the lack of a hierarchy.
>They waved it off again for V6 which makes me think there is a deeper
>screw-up in the data structure. So I'll sit out that upgrade as well.

Wow. That would take a massive malfunction in the architecture to
prevent developing code for hierarchal schematics and layouts. Hell they
go hand in hand.

?-)

[John S]

On 12/24/2011 8:07 PM, josephkk wrote:
> On Wed, 21 Dec 2011 13:56:55 -0800, Joerg<inv...@invalid.invalid> wrote:
>
>> JeffM wrote:
>>> Joerg wrote:
>>>> if it doesn't have to be [EAGLE]{1}[,]
>>>> there is someone at a company in S.F. that you know :-)
>>>>
>>> ...and perhaps she would like to learn another package
>>> beyond PADS.
>>>
>>
>> Wots wrong with PADS? Over the last 10 years or so most of my layouts
>> have been done with PADS and I didn't see anything amiss.
>>
>> But I am not picky about details. Like with cars. Dealer asks me what
>> color I like and I tell him it doesn't matter ... "Say WHAT?!"
>>
>>
>>> ...and for other EAGLE neophites considering that package:
>>> http://tinyurl.com/TheEAGLE-Virus
>>>
>>
>> Ah, the cruzade ... You and your conspiracy theory :-)
>>
>>
>>> Now, for a show of hands here
>>> of anyone who ever got useful results from an autorouter.
>>> ...particularly on a project with more than 22 components.
>>
>>
>> Nay.
>>
>>
>>> ...especially with an ECAD package that cost less than $5k.
>>
>>
>> Don't matter. An autorouter is usually no good when it comes to hot stuff.

If you set it up correctly, the Eagle Autorouter works very well. I used
it to autoroute high-current (20 amps or so) and low current (mA) on the
same board with no problems. Please note that you can route traces
individually.

[John S]

On 12/24/2011 7:58 PM, JeffM wrote:
>> JeffM wrote:
>>> ...and John S is another one who makes it up as he goes along.
>>>
> John S wrote:
>> Whoa! Make up wot? I've seen your complaints now for years.
>>
> Reading comprehension problems, then?
> Lousy memory?

No worse than yours.

> Never actually clicked the link I always post?

Yes, I did, more than once. More than enough.

>> Same old story. I never said that you were lying.
>>
> Right. Instead, you made up your own narrative and claimed it is
> mine.
>

Made up? Post my made-up narrative.

>> I believe your story.
>>
> You'd have to KNOW it first.

I only read your link a few times. Is that knowing?

>> Now, show me where I made something up about you,
>> Mr. Useless Scum Bag.
>>
> news:jd0pjc$sq9$1...@dont-email.me
> http://groups.google.com/group/sci.electronics.design/msg/2f5ecdd92d4b4ce2
> :JeffM was, in his opinion, screwed by CadSoft some years ago.
> :
> Fabricated out of whole cloth by you.

In what way was it fabricated? Show me.

> Cadsoft never got the opportunity to abuse me with their DRM.
> I am, however, VERY angry that I had previously been responsible
> for the scumbags getting some money from my previous company.

None of this is your fault, of course. The fact that you used some
unknown piece of an (illegal, according to Eagle) Eagle layout for your
own purpose is not your fault.

> Surreptitious bombs purposely put into software by its vendor
> just makes me see red.

Of course. That's your vendetta. Have you learned to stay away from the
bombs? It seems that yours is the only complaint. Do you have links to
others who have complained similarly?

> When that is in a tool that could blow up in your face
> when you're on deadline, the steam comes out my ears.

Of course. That's your vendetta.

> When the company then tells you
> "Go fuck yourself, Mr. Paid-Up customer", that's the limit.

Of course. That's your vendetta.

> Anyone who endorses that kind of corporate behavior
> would also sell out to any slimeball who is the highest bidder.

I don't endorse it. You have, in my opinion, a legitimate complaint.
Most of us are just sick of you jumping in and ranting on every post
that has Eagle or Cadsoft. We already know about you and your hate
thing. Give it a rest.

[k...@att.bizzzzzzzzzzzz]

On Sat, 24 Dec 2011 18:07:32 -0800, josephkk <joseph_...@sbcglobal.net>
wrote:

Yet even Cadence couldn't get it to work in OrCAD until last year. Allegro
doesn't really use hierarchy either.

[k...@att.bizzzzzzzzzzzz]

Different animals completely. GDS ~= Gerber. EDIF is a netlist standard.

>FPGA stuff is usually highly
>proprietary to the respective product line, I wouldn't know what would
>be exchangeable or standardized there. The only thing you have is
>conversion services, in case your volume goes up and you want it all
>poured into an ASIC.

Within the tools the netlists are in EDIF. EDIF is used for third-party
tools, as well.

>The whole sob story is summed up here and the word that, not
>surprisingly, darts out is "problem":
>
>http://en.wikipedia.org/wiki/EDIF
>
>Quote "The vendor companies did not always feel it important to allocate
>many resources to EDIF products, even if they sold a large number of
>them. There were several stories of active products with virtually
>no-one to maintain them for years. User complaints were merely gathered
>and prioritized. The harder it became to export customer data to EDIF,
>the more the vendors seemed to like it".

You're talking about different "vendors" than I'm familiar with, at least at
that end of the business. Of course, EDIF isn't important for board level
tools.

>>>>>> ... Pretty pictures ain't it.
>>>>>>
>>>>> No, the intention was that CAD data becomes exchangeable between CAD
>>>>> system. That clearly did not materialize.
>>>> Maybe that was your wish. No one else had that fantasy, though. ;-)
>>>>
>>> That goal was all over the trade publications back then. I never
>>> believed it would come to fruition though, and it didn't.
>>
>> You gotta stop reading that crap.
>>
>> trade magazines ~= New York Times
>>
>> No intelligence there.
>>
>
>You don't ever read EETimes, EDN and stuff? I don't spend a lot of time
>there but occasionally it nets me a hint to a product I might otherwise
>have missed because it was geared towards a very different market.

Nope, not for at least thirty years. They're a complete waste of time.

As I mentioned, I'm just learning the tool (a couple of weeks in on a hot
design) so there may be things I'm missing but so far no one has been able to
show me how to print multiple pages. They tell me that to print PDFs, they do
one page at a time and then use Acrobat to stitch them together. Yeah, major
ugh! It does look like the tool supports hierarchy, though. No one uses
hierarchy or, I think, knows what to do with it, so I'll have to play with it.

[Joerg]

k...@att.bizzzzzzzzzzzz wrote:
> On Sat, 24 Dec 2011 17:08:41 -0800, Joerg <inv...@invalid.invalid> wrote:
>
>> k...@att.bizzzzzzzzzzzz wrote:
>>> On Sat, 24 Dec 2011 14:21:28 -0800, Joerg <inv...@invalid.invalid> wrote:
>>>

>> The whole sob story is summed up here and the word that, not
>> surprisingly, darts out is "problem":
>>
>> http://en.wikipedia.org/wiki/EDIF
>>
>> Quote "The vendor companies did not always feel it important to allocate
>> many resources to EDIF products, even if they sold a large number of
>> them. There were several stories of active products with virtually
>> no-one to maintain them for years. User complaints were merely gathered
>> and prioritized. The harder it became to export customer data to EDIF,
>> the more the vendors seemed to like it".
>
> You're talking about different "vendors" than I'm familiar with, at least at
> that end of the business. Of course, EDIF isn't important for board level
> tools.
>

So, then, which vendors are we talking about? Last time a move between a
Mentor system to a Cadence system was contemplated the talk turned
towards the effort of file conversion (schematic level, for a large IC).
This effort was considered major. So far for EDIF ...

>>>>>>> ... Pretty pictures ain't it.
>>>>>>>
>>>>>> No, the intention was that CAD data becomes exchangeable between CAD
>>>>>> system. That clearly did not materialize.
>>>>> Maybe that was your wish. No one else had that fantasy, though. ;-)
>>>>>
>>>> That goal was all over the trade publications back then. I never
>>>> believed it would come to fruition though, and it didn't.
>>> You gotta stop reading that crap.
>>>
>>> trade magazines ~= New York Times
>>>
>>> No intelligence there.
>>>
>> You don't ever read EETimes, EDN and stuff? I don't spend a lot of time
>> there but occasionally it nets me a hint to a product I might otherwise
>> have missed because it was geared towards a very different market.
>
> Nope, not for at least thirty years. They're a complete waste of time.
>

I don't read them often but glance over them. Many times I found gems,
cases where one of my clients had an almost perfect "wacky use" for some
IC. Their EEs missed it because they didn't keep an eye on these magazines.

In fact, sometimes they pay me for keeping that eye open :-)

[...]

>>> Hierarchy? I'd be happy to be able to print more than one page at a time. :-(
>>
>> Ugh. That sounds bad. That software goes on my "not to do" list :-)
>
> As I mentioned, I'm just learning the tool (a couple of weeks in on a hot
> design) so there may be things I'm missing but so far no one has been able to
> show me how to print multiple pages. They tell me that to print PDFs, they do
> one page at a time and then use Acrobat to stitch them together. Yeah, major
> ugh! It does look like the tool supports hierarchy, though. No one uses
> hierarchy or, I think, knows what to do with it, so I'll have to play with it.

That's because you aren't working in a heavily regulated industry, else
your colleagues would be familiar with it. I doubt anyone would dare to
submit a set of schematics for a very large system in med or aero
without a properly organized hierarchy. It would be like telling the tax
auditor "Here, it's all in this Hefty bag, somewhere".

[k...@att.bizzzzzzzzzzzz]

On Sun, 25 Dec 2011 12:11:58 -0800, Joerg <inv...@invalid.invalid> wrote:

>k...@att.bizzzzzzzzzzzz wrote:
>> On Sat, 24 Dec 2011 17:08:41 -0800, Joerg <inv...@invalid.invalid> wrote:
>>
>>> k...@att.bizzzzzzzzzzzz wrote:
>>>> On Sat, 24 Dec 2011 14:21:28 -0800, Joerg <inv...@invalid.invalid> wrote:
>>>>
>
>>> The whole sob story is summed up here and the word that, not
>>> surprisingly, darts out is "problem":
>>>
>>> http://en.wikipedia.org/wiki/EDIF
>>>
>>> Quote "The vendor companies did not always feel it important to allocate
>>> many resources to EDIF products, even if they sold a large number of
>>> them. There were several stories of active products with virtually
>>> no-one to maintain them for years. User complaints were merely gathered
>>> and prioritized. The harder it became to export customer data to EDIF,
>>> the more the vendors seemed to like it".
>>
>> You're talking about different "vendors" than I'm familiar with, at least at
>> that end of the business. Of course, EDIF isn't important for board level
>> tools.
>>
>
>So, then, which vendors are we talking about?

Chip manufacturers.

>Last time a move between a
>Mentor system to a Cadence system was contemplated the talk turned
>towards the effort of file conversion (schematic level, for a large IC).
>This effort was considered major. So far for EDIF ...

As I said above, EDIF's function is not to draw pretty pictures, rather take
the netlist generated by the schematic capture to the next level. I don't
recall even any reverse annotation.

>>>>>>>> ... Pretty pictures ain't it.
>>>>>>>>
>>>>>>> No, the intention was that CAD data becomes exchangeable between CAD
>>>>>>> system. That clearly did not materialize.
>>>>>> Maybe that was your wish. No one else had that fantasy, though. ;-)
>>>>>>
>>>>> That goal was all over the trade publications back then. I never
>>>>> believed it would come to fruition though, and it didn't.
>>>> You gotta stop reading that crap.
>>>>
>>>> trade magazines ~= New York Times
>>>>
>>>> No intelligence there.
>>>>
>>> You don't ever read EETimes, EDN and stuff? I don't spend a lot of time
>>> there but occasionally it nets me a hint to a product I might otherwise
>>> have missed because it was geared towards a very different market.
>>
>> Nope, not for at least thirty years. They're a complete waste of time.
>>
>
>I don't read them often but glance over them. Many times I found gems,
>cases where one of my clients had an almost perfect "wacky use" for some
>IC. Their EEs missed it because they didn't keep an eye on these magazines.
>
>In fact, sometimes they pay me for keeping that eye open :-)

A cow-orker used to send an article around once in a while with some comment
that we could use some technique or other. In every case it was something
incredibly obvious, that everyone in this group (less DimBulb and Slowman) has
been doing for decades, that the author was trying to claim as his own.

As I said, a total waste of time.

>>>> Hierarchy? I'd be happy to be able to print more than one page at a time. :-(
>>>
>>> Ugh. That sounds bad. That software goes on my "not to do" list :-)
>>
>> As I mentioned, I'm just learning the tool (a couple of weeks in on a hot
>> design) so there may be things I'm missing but so far no one has been able to
>> show me how to print multiple pages. They tell me that to print PDFs, they do
>> one page at a time and then use Acrobat to stitch them together. Yeah, major
>> ugh! It does look like the tool supports hierarchy, though. No one uses
>> hierarchy or, I think, knows what to do with it, so I'll have to play with it.
>
>
>That's because you aren't working in a heavily regulated industry, else
>your colleagues would be familiar with it. I doubt anyone would dare to
>submit a set of schematics for a very large system in med or aero
>without a properly organized hierarchy. It would be like telling the tax
>auditor "Here, it's all in this Hefty bag, somewhere".

Could easily be. I rather like hierarchical designs. If for no other reason,
it makes schematics far easier to read. Recently someone (here?) was arguing
that there was no need. I asked if he wrote flat VHDL, too.

[Joerg]

k...@att.bizzzzzzzzzzzz wrote:
> On Sun, 25 Dec 2011 12:11:58 -0800, Joerg <inv...@invalid.invalid> wrote:
>
>> k...@att.bizzzzzzzzzzzz wrote:
>>> On Sat, 24 Dec 2011 17:08:41 -0800, Joerg <inv...@invalid.invalid> wrote:
>>>
>>>> k...@att.bizzzzzzzzzzzz wrote:
>>>>> On Sat, 24 Dec 2011 14:21:28 -0800, Joerg <inv...@invalid.invalid> wrote:
>>>>>
>>>> The whole sob story is summed up here and the word that, not
>>>> surprisingly, darts out is "problem":
>>>>
>>>> http://en.wikipedia.org/wiki/EDIF
>>>>
>>>> Quote "The vendor companies did not always feel it important to allocate
>>>> many resources to EDIF products, even if they sold a large number of
>>>> them. There were several stories of active products with virtually
>>>> no-one to maintain them for years. User complaints were merely gathered
>>>> and prioritized. The harder it became to export customer data to EDIF,
>>>> the more the vendors seemed to like it".
>>> You're talking about different "vendors" than I'm familiar with, at least at
>>> that end of the business. Of course, EDIF isn't important for board level
>>> tools.
>>>
>> So, then, which vendors are we talking about?
>
> Chip manufacturers.
>

They just get the GDS-II files and make our wafers. Or did you mean TI,
AD, ON Semi and so on? Can't imagine that they dont' use the major CAD
suites. The schematic file formats between those suites of different
vendors are incompatible from what I've been told many times.

>> Last time a move between a
>> Mentor system to a Cadence system was contemplated the talk turned
>> towards the effort of file conversion (schematic level, for a large IC).
>> This effort was considered major. So far for EDIF ...
>
> As I said above, EDIF's function is not to draw pretty pictures, rather take
> the netlist generated by the schematic capture to the next level. I don't
> recall even any reverse annotation.
>

That is a far cry from what EDIF was touted to be. In German they have a
saying which loosely translates into "The mountain has reached full
term, and it gave birth to a mouse" :-)

>>>>>>>>> ... Pretty pictures ain't it.
>>>>>>>>>
>>>>>>>> No, the intention was that CAD data becomes exchangeable between CAD
>>>>>>>> system. That clearly did not materialize.
>>>>>>> Maybe that was your wish. No one else had that fantasy, though. ;-)
>>>>>>>
>>>>>> That goal was all over the trade publications back then. I never
>>>>>> believed it would come to fruition though, and it didn't.
>>>>> You gotta stop reading that crap.
>>>>>
>>>>> trade magazines ~= New York Times
>>>>>
>>>>> No intelligence there.
>>>>>
>>>> You don't ever read EETimes, EDN and stuff? I don't spend a lot of time
>>>> there but occasionally it nets me a hint to a product I might otherwise
>>>> have missed because it was geared towards a very different market.
>>> Nope, not for at least thirty years. They're a complete waste of time.
>>>
>> I don't read them often but glance over them. Many times I found gems,
>> cases where one of my clients had an almost perfect "wacky use" for some
>> IC. Their EEs missed it because they didn't keep an eye on these magazines.
>>
>> In fact, sometimes they pay me for keeping that eye open :-)
>
> A cow-orker used to send an article around once in a while with some comment
> that we could use some technique or other. In every case it was something
> incredibly obvious, that everyone in this group (less DimBulb and Slowman) has
> been doing for decades, that the author was trying to claim as his own.
>
> As I said, a total waste of time.
>

Not all all to me. Has about the same value as some select (very few)
manufacturer email updates. Takes 1-2 min to read through diagonally. If
this nets 1-2 wacky uses for an off-market chip per year, and it usually
does, then the ROI is huge. I've had cases where the cost of a module
dropped by a couple hundred bucks because a consumer chip could replace
a super expensive boutique set of parts.

Depends on the field you are working in though. For RF there ain't too
much use in this. For ultrasound, laser stuff, fast machine control,
very different story.

>>>>> Hierarchy? I'd be happy to be able to print more than one page at a time. :-(
>>>> Ugh. That sounds bad. That software goes on my "not to do" list :-)
>>> As I mentioned, I'm just learning the tool (a couple of weeks in on a hot
>>> design) so there may be things I'm missing but so far no one has been able to
>>> show me how to print multiple pages. They tell me that to print PDFs, they do
>>> one page at a time and then use Acrobat to stitch them together. Yeah, major
>>> ugh! It does look like the tool supports hierarchy, though. No one uses
>>> hierarchy or, I think, knows what to do with it, so I'll have to play with it.
>>
>> That's because you aren't working in a heavily regulated industry, else
>> your colleagues would be familiar with it. I doubt anyone would dare to
>> submit a set of schematics for a very large system in med or aero
>> without a properly organized hierarchy. It would be like telling the tax
>> auditor "Here, it's all in this Hefty bag, somewhere".
>
> Could easily be. I rather like hierarchical designs. If for no other reason,
> it makes schematics far easier to read. Recently someone (here?) was arguing
> that there was no need. I asked if he wrote flat VHDL, too.

Take a look at his tool cabinets. They are probably a royal mess :-)

[k...@att.bizzzzzzzzzzzz]

I mean TSMC, IBM, and such. Again, schematics output netlists, which like
Humpty, can't be put back together into pretty picture schematics.

>>> Last time a move between a
>>> Mentor system to a Cadence system was contemplated the talk turned
>>> towards the effort of file conversion (schematic level, for a large IC).
>>> This effort was considered major. So far for EDIF ...
>>
>> As I said above, EDIF's function is not to draw pretty pictures, rather take
>> the netlist generated by the schematic capture to the next level. I don't
>> recall even any reverse annotation.
>>
>
>That is a far cry from what EDIF was touted to be. In German they have a
>saying which loosely translates into "The mountain has reached full
>term, and it gave birth to a mouse" :-)

Touted by your "industry newsletters"? That's what it *is*.

I read very few of the manufacturer's emails. When I need something I search
their web sites.

>Depends on the field you are working in though. For RF there ain't too
>much use in this. For ultrasound, laser stuff, fast machine control,
>very different story.
>
>
>>>>>> Hierarchy? I'd be happy to be able to print more than one page at a time. :-(
>>>>> Ugh. That sounds bad. That software goes on my "not to do" list :-)
>>>> As I mentioned, I'm just learning the tool (a couple of weeks in on a hot
>>>> design) so there may be things I'm missing but so far no one has been able to
>>>> show me how to print multiple pages. They tell me that to print PDFs, they do
>>>> one page at a time and then use Acrobat to stitch them together. Yeah, major
>>>> ugh! It does look like the tool supports hierarchy, though. No one uses
>>>> hierarchy or, I think, knows what to do with it, so I'll have to play with it.
>>>
>>> That's because you aren't working in a heavily regulated industry, else
>>> your colleagues would be familiar with it. I doubt anyone would dare to
>>> submit a set of schematics for a very large system in med or aero
>>> without a properly organized hierarchy. It would be like telling the tax
>>> auditor "Here, it's all in this Hefty bag, somewhere".
>>
>> Could easily be. I rather like hierarchical designs. If for no other reason,
>> it makes schematics far easier to read. Recently someone (here?) was arguing
>> that there was no need. I asked if he wrote flat VHDL, too.
>
>
>Take a look at his tool cabinets. They are probably a royal mess :-)

Ulp! I resemble that. ;-)

[Joerg]

So are they not using Mentor and Cadence?

<scratching head>

>>>> Last time a move between a
>>>> Mentor system to a Cadence system was contemplated the talk turned
>>>> towards the effort of file conversion (schematic level, for a large IC).
>>>> This effort was considered major. So far for EDIF ...
>>> As I said above, EDIF's function is not to draw pretty pictures, rather take
>>> the netlist generated by the schematic capture to the next level. I don't
>>> recall even any reverse annotation.
>>>
>> That is a far cry from what EDIF was touted to be. In German they have a
>> saying which loosely translates into "The mountain has reached full
>> term, and it gave birth to a mouse" :-)
>
> Touted by your "industry newsletters"? That's what it *is*.
>

No, touted by all sorts of bigshot EDA companies.

That is exactly why I am sometimes the first to come up with a "wacky
use" idea for a part. Because of the "when I need something" effect. By
then engineers are typically already under schedule pressure and, guess
what, they immediately scoot over to Analog Devices or LTC. There they
find the $3.50 part that does the job. It's good stuff, support is great
and they know it'll work.

Then comes yours truly, proposing to use this automotive IC instead
because it's only 31 cents a piece, and some jaws drop. Usually the only
reason I come up with ideas like that is because I've read about it a
few months ago, can't quite remember where, but remember enough bits and
pieces about it that a few minutes on the web will find it back. Without
reading industry newsletters this would usually not happen.

All this probably means little to you because your company doesn't
design real mass products, stuff where 5k units/mo roll off a conveyor
belt in Guangdong. Then such a price difference matters, big time.

>> Depends on the field you are working in though. For RF there ain't too
>> much use in this. For ultrasound, laser stuff, fast machine control,
>> very different story.
>>
>>
>>>>>>> Hierarchy? I'd be happy to be able to print more than one page at a time. :-(
>>>>>> Ugh. That sounds bad. That software goes on my "not to do" list :-)
>>>>> As I mentioned, I'm just learning the tool (a couple of weeks in on a hot
>>>>> design) so there may be things I'm missing but so far no one has been able to
>>>>> show me how to print multiple pages. They tell me that to print PDFs, they do
>>>>> one page at a time and then use Acrobat to stitch them together. Yeah, major
>>>>> ugh! It does look like the tool supports hierarchy, though. No one uses
>>>>> hierarchy or, I think, knows what to do with it, so I'll have to play with it.
>>>> That's because you aren't working in a heavily regulated industry, else
>>>> your colleagues would be familiar with it. I doubt anyone would dare to
>>>> submit a set of schematics for a very large system in med or aero
>>>> without a properly organized hierarchy. It would be like telling the tax
>>>> auditor "Here, it's all in this Hefty bag, somewhere".
>>> Could easily be. I rather like hierarchical designs. If for no other reason,
>>> it makes schematics far easier to read. Recently someone (here?) was arguing
>>> that there was no need. I asked if he wrote flat VHDL, too.
>>
>> Take a look at his tool cabinets. They are probably a royal mess :-)
>
> Ulp! I resemble that. ;-)

My wife sez me too :-(

Fixing her sewing machine right now.

[Joerg]

Joerg wrote:
> k...@att.bizzzzzzzzzzzz wrote:
>> On Sun, 25 Dec 2011 13:02:49 -0800, Joerg <inv...@invalid.invalid> wrote:
>>
>>> k...@att.bizzzzzzzzzzzz wrote:
>>>> On Sun, 25 Dec 2011 12:11:58 -0800, Joerg <inv...@invalid.invalid> wrote:
>>>>

[...]

>
>>>>> Last time a move between a
>>>>> Mentor system to a Cadence system was contemplated the talk turned
>>>>> towards the effort of file conversion (schematic level, for a large IC).
>>>>> This effort was considered major. So far for EDIF ...
>>>> As I said above, EDIF's function is not to draw pretty pictures, rather take
>>>> the netlist generated by the schematic capture to the next level. I don't
>>>> recall even any reverse annotation.
>>>>
>>> That is a far cry from what EDIF was touted to be. In German they have a
>>> saying which loosely translates into "The mountain has reached full
>>> term, and it gave birth to a mouse" :-)
>> Touted by your "industry newsletters"? That's what it *is*.
>>
>
> No, touted by all sorts of bigshot EDA companies.
>

Sorry, meant EDA distributors.

[...]

[Phil Hobbs]

It diffused northward when Rome fell. ;)
That's a quotation from one of Horace's odes: "Parturient montes,
nascetur ridiculus mus". See e.g. http://en.wikiquote.org/wiki/Horace

Cheers

Phil Hobbs


--
Dr Philip C D Hobbs
Principal Consultant
ElectroOptical Innovations LLC
Optics, Electro-optics, Photonics, Analog Electronics

160 North State Road #203
Briarcliff Manor NY 10510
845-480-2058

hobbs at electrooptical dot net
http://electrooptical.net