ORCAD translation: Libraries, Off-Page, Power, and Ground symbols incomplete...

[ta...@listserver.pads.com]

When designing from scratch within my PADS suite I have learned to set up my component libraries in a complete fashion.
All component attributes are available on the LOGIC schematic and in the LAYOUT board design. They reference the same library and share the same attributes.
This allows BOM extraction from EITHER the schematic source file or the layout source file.

In addition, I have core group of OFF-Page, POWER, and GROUND symbols that have been acquired over the years of designing.
This makes new projects easier to get started.

I have a new project translating some ORCAD designs into PADS LOGIC.
I am not an ORCAD guy and know very little about it.
I have been provided with the original ORCAD desing files which include the .DSN, .OLB, .BOM, .DRC, .INC, ONL and .OPJ files.
Seemingly everything I need to redesign the boards.

PADS LOGIC will open the .DSN file as a translated schematic.
This translation provides me part symbols and subsequent component connections with net names.

In addition, PADS has library translators too. I can choose to translate the .OLB library file directly OR save all the parts from the translated schematic. Either way, I can end up with the same new library entries with part shapes but NO attributes... and invariably the part naming convention is very poor to say the least.

Question 1:
I am assuming the ORCAD library translators only work "correctly" if the original ORCAD Library/Design files HAVE attributes for all parts. The Original Engineer would have had to set ORCAD up right.
Otherwise, my library translation will be incomplete and I still have to edit each part for desired attributes ect.

How does the Translator handle the BOM translation process?
It seems I have to enter all BOM information into PADS which is time consuming and opens the door for errors in the final "translation"

Question 2:
The schematic/library translations has issues with the OFF PAGE, POWER, and GROUND symbols.
I end up with the incorrect symbols being used for OFF PAGE, POWER, and GROUND. This creates LOTS of extra work and the potential to make a bad net connection when attempting to sort through a multi-page schematic with multiple off-page connections and multiple power and ground connections.
How do I prevent these OFF-PAGE, POWER, and GROUND issues?

-Kevin DeFever

-END-
SupportNet: http://www.mentor.com/supportnet
To unsubscribe send a blank email to: leave-ta...@listserver.pads.com
For assistance please send mail to talkli...@mentor.com

[Cliff Harris]

You can look at the part attributes in OrCAD by hitting Ctrl-A to select all and then Ctrl-E to edit attributes. Select the Part tab at the bottom. You should then get a list of all the parts in the schematic and their attributes. In my experience, the only attribute that is set to something useful is "Value".

Since we do OrCAD to PADS here, I have to set the decal in the "PCB Footprint" attribute.

[Hawker <hawker@ashevillecommunity.org>]

OrCAD handles attributes very poorly and a bit weird.
Depending on what version of OrCAD you are using you are most likely
looking at OrCAD issues not PADS issues.
I am no OrCAD expert, but I have been forced to use it from time to time
when an engineer does the work in OrCAD.

To address you questions.
1) Most Engineers who use OrCAD have very little understanding of how to
make a schematic for actually manufacturing a PCB and Product. Most use
the generic symbols and they are not set for PCB and attributes. BOM
info tends to be generic etc. Very few actually use the attributes at
all. I can't tell you how many times i have told an engineer 74HCT377
or even worse 377 is not an acceptable part number.

2) OrCAD seems to have two levels of attributes. If you add them to the
part on the schematic (as most do) they do not translate to the actual
part, only that instance and do not seem to export library wise (other
the OrCAD to PADS net extractor that a user here wrote). The second
level is to actually put them in the library. That way allows them to
export better. Since this is conveluted I rarely see it done the second,
but proper way.

3) Earlier versions of OrCAD (9.2 and before) had serious net integrity
issues with off page symbols, especially ground. It was very possible to
have two net symbols look the same but be different nets or visa versa.
My guess is you have that going on and PADS does not know what to do
with it.

[Robert Kondner]

Hawker,

While I accept the fact most schematics area drawn in OrCAD (The reason
being 100 Million Flies Can't Be Wrong) can you just imagine the donkey-doo
that would result from the same flies swarming on ViewDraw? They would ask
100 Million questions and still get it wrong.

I don't think it is fair to criticize the tool because the user is a
newbie with little experience managing electronic part library. I have used
OrCAD 9.2 for years and never had a problem with net list extraction and
page symbols. Not to say other don't but at least it can work. I will say
the old 7.x version (As in Windows 3.1 days) had piles of issues.

Us old folk with experience from DOS days are a dying (or maybe downsized)
group so remember "The Newbies Shall Inherited the World". How do we make it
easier for them to "Get It Right"?

Bob Kondner

PS: The biggest problem I have seen with Newbies is they think their IPhone
is all they need to interface with the world. Getting them to pull out a pad
of graph paper and write/draw what they need is like pulling hens teeth.

-----Original Message-----
From: Hawker <haw...@ashevillecommunity.org>
[mailto:ta...@listserver.pads.com]
Sent: Tuesday, June 08, 2010 10:31 AM
To: Talk Mailing List
Subject: Re: ORCAD translation: Libraries, Off-Page, Power, and Ground
symbols incomplete...

[Hawker <hawker@ashevillecommunity.org>]

On 6/8/2010 11:04 AM, Robert Kondner wrote:
> Hawker,
>
> While I accept the fact most schematics area drawn in OrCAD (The reason
> being 100 Million Flies Can't Be Wrong) can you just imagine the donkey-doo
> that would result from the same flies swarming on ViewDraw? They would ask
> 100 Million questions and still get it wrong.
>
> I don't think it is fair to criticize the tool because the user is a
> newbie with little experience managing electronic part library. I have used
> OrCAD 9.2 for years and never had a problem with net list extraction and
> page symbols. Not to say other don't but at least it can work. I will say
> the old 7.x version (As in Windows 3.1 days) had piles of issues.
>
>

9.2 was almost there, but i have still spent time chasing nets that
displayed as one name but were actually two different names that did not
connect.
7.x was much worse, I agree. BTW I used 7.2 when I did work for
Tektronix circa 1995-1998. That was Windows NT 4.0 (or Windows 95 if you
were unlucky) so it was pre Windows 3.11. We used Viewdraw 7.x in the
3.11 days so that may be what you remember.

I agree it is not a tool issue in so much as the tool is too easy to do
things wrong in. Many people "learn" it early on and stick with it, even
though they don't understand what they are doing. I run into more OrCAD
users who are clueless to the big picture than Logic users who are
clueless.
That said OrCAD, being such a simple tool, is easier to make a mess in
than Logic.

[tcwaggoner]

Hawker,

Tell your Orcad users to EDIT>FIND>* (Nets).

It takes about a minute to look at the "Object ID" and "NetName" to find
split nets.

I just went through a customer design where they thought they had 5
different "grounds" (all using the same graphical symbol) but there were 6.

Things will stand out like

Object_ID Net_Name
GND GND
GND GND_N12345
GND GND_N67890

I do not use LOGIC, but the DxDesigner translation keeps these nets
split to match the original Orcad Capture schematic.

Terrence Waggoner

[Paul Brionez]

look for an offpage connected to a power net

tcwaggoner <ta...@listserver.pads.com> wrote:

-END-
SupportNet: http://www.mentor.com/supportnet
To unsubscribe send a blank email to: $subst('Email.UnSub')