Jaluino Bee, first draft

[Sebastien Lelong]

Hi guys,

As I mentioned some times ago, I'm trying to design a new Jaluino board, named Jaluino Bee because it needs a name. This idea is to provide a very small board, very cheap, thus using SMD components. It would include a Xbee socket, as a standard way to plug many different communication modules (real Xbee/ZigBee, RF, USB, ...). I'm trying to make it as modular as possible. Depending on usage, user would solder require  components or not. For instance:

  - use USB or not

  - crystal or internal clock

  - use 5V, 3V3, both or no voltage regulator (none could be used to directly power the board using batteries for instance). Based on adjustable vreg LM317.

  - or power the board through a serial module or USB

  - use I²C or not

  - Reset via RTS option

  - CTS/RTS option

  - connectors for pin header: plug on a breadboard (male) *or* used to plug potential shields (female)

  - ICSP connector

  - serial connector

Attached is a first schematic draft. No PCB design yet, I don't know if all of this will fit within 5x5cm or smaller. But I guess so.

Schematic is for PIC18F27J53, SOIC package, but I identified at least 2 other interesting chips:

  - PIC18F2550: quite common, USB inside

  - PIC18F25K22: for high speed application (up to 64MHz), lots of mem, no USB

More may also fit.

As for SMD design, I followed advices and used 1206 resistors and capacitors, as they are easier to solder. I also wanted to use SOIC package for MCU, easier to solder than SSOP for instance. There are a lot of jumpers, due to modularity. I'm hesitating: either using PTH jumpers, or solder jumpers. First are interesting when tinkering with the board, they can be always changed. But they are very tall. Solder jumpers cannot be easliy changed. I then figured out it may be possible to solder 0805 0ohm resistor over PTH jumper traces (0805 is 0.08" long, PTH space between pins is 0.1"). This way user can choose between a flexible, ready-to-tinker modules (PTH) and something more definitive (using 0 ohm resistors). What do you think ?

Every component I'm using here seem to be easily available. But because it's kind of painful to source components, I may provide most of them (except MCU) if it appeared to be manufactured.

Any advices, thoughts, feedback appreciated.

Cheers

Seb

--
Sébastien Lelong
http://www.sirloon.net
http://sirbot.org

[mattschinkel]

Great work seb!

Although "Bee" is a good name, there may be confusion with the jallib-
pack-bee

Matt

On Jan 22, 9:33 am, Sebastien Lelong <sebastien.lel...@gmail.com>
wrote:

>  jaluino_v01_bee_schematic.png
> 55KViewDownload

[funlw65(Vasi)]

It will be a nice challenge.

Vasi

On Jan 22, 4:33 pm, Sebastien Lelong <sebastien.lel...@gmail.com>
wrote:

[phalox]

It's a nice concept!

At GroupT (my college) we use the USB Whacker clone from sparkfun.
It's built around the 18F2553 (2bit extra ADC over 18F2550) :)
It's a nice microcontroller for experimenting stuff!

If you would keep it under 5cm², you could let it produce by
seeedstudio! They're really cheap... The only problem I had was that
there were some interconnections that shouldn't be there. But that
shouldn't happen anymore they told me :)

Good luck!!

[Sebastien Lelong]

Hi Toon,

2011/1/22 phalox <too...@gmail.com>

It's a nice concept!

At GroupT (my college) we use the USB Whacker clone from sparkfun.
It's built around the 18F2553 (2bit extra ADC over 18F2550) :)
It's a nice microcontroller for experimenting stuff!

If you want another one to have fun, have a look at 18F27J53 (though only support 3.3V device). You won't find so many features in one chip (including 12-bits ADC, USB without xtal,  2 USART, 2 MSSP, many remappable pins, RTC hardware, big & ram, ...

http://www.microchip.com/wwwproducts/Devices.aspx?dDocName=en548695

 

If you would keep it under 5cm², you could let it produce by
seeedstudio! They're really cheap... The only problem I had was that
there were some interconnections that shouldn't be there. But that
shouldn't happen anymore they told me :)

That's the idea, fit it within 5x5cm to manufacture it with Seeed. Last Jaluino v2.0 (and crumboard shields) were produced by seeed.

Cheers,

Seb

[phalox]

> If you want another one to have fun, have a look at 18F27J53 (though only
> support 3.3V device). You won't find so many features in one chip (including
> 12-bits ADC, USB without xtal,  2 USART, 2 MSSP, many remappable pins, RTC
> hardware, big & ram, ...
>
> http://www.microchip.com/wwwproducts/Devices.aspx?dDocName=en548695

That's a real nice one!
I had a look at the prices of both microcontrollers and it seems that
yours is even cheaper! I'm thinking of proposing this one for the next
batch of boards, only the 3.3v might give some issues...
For LEDs it's not really a problem... And for now we haven't used much
more than that.

Suprising how a more advanced device can be cheaper.

> That's the idea, fit it within 5x5cm to manufacture it with Seeed. Last
> Jaluino v2.0 (and crumboard shields) were produced by seeed.

$2 per PCB would be a real bargain! I'm still looking for a good way
to start with SMD. I'd need to make some own PCB's...

Toon

[Sebastien Lelong]

Hi,

2011/1/22 phalox <too...@gmail.com>

That's a real nice one!

I had a look at the prices of both microcontrollers and it seems that
yours is even cheaper! I'm thinking of proposing this one for the next
batch of boards, only the 3.3v might give some issues...
For LEDs it's not really a problem... And for now we haven't used much
more than that.

I succesfully used USB with 3.3V (and even 2.5V) used as power voltage for the PIC. Same with serial. Did not test I²C but I think Joep said it was supposed to work too. PIC18F27J53 (one problem with this PIC is writing its name) has some 5V tolerant inputs, which I think will greatly simplify some 5V/3V3 integration.

Cheers,

Seb

[phalox]

Maybe take this one into your design too?

It's pin compatible with the 2550, it only needs some capacitors, and
a different supply.
So one pcb would make 2 nice boards... one rated at 5V, the other at
3.3

Just an idea but I think it would be very nice!

ps: ever tried to write the names of those µC delivered with the TI
launchpad?
MSP430G2211IN14

[Sebastien Lelong]

There many PICs more or less pin compatible. I mean it needs at least to be compatible regarding power supply, clock, ICSP, and maybe also serial. So your PIC would also probably be usable with this PCB.

The problem is, for instance, where to put onboard LED. I put it in RA0 pin, which maybe is not a very good idea: RA0 also carries AN0, when using PIC with dependent ADC pins, this one will always be included in configuration, thus no more LED. So, where to put this onboard LED ? Meaning, which pin to sacrifice ? Or, maybe, just don't solder the LED... Or, maybe, I should develop a small app that would screen many ICs and report which could be used :)

Regarding 5V or 3V3, it's included in the design, though not sure yet if it's properly done. There are 2 regulators, both optional (bypass through solder jumper). So you can choose to power your board with 9V (regulated to 5V, then 3V3), 5V (5V reg bypassed, then regulated to 3V3), and 3V3 (all reg bypassed). Then you can choose (when appropriate) which between 5V and 3V3 to use to power your PIC (eg. PIC can have 5V, but Xbee requires 3V3, so you need both). It's only a matter of using the proper voltage regulator. LM317 can do many voltage output, that's why I chose it, but I still wonder if it'll be powerful enough. In doubt, its pin layout is compatible with other nice regultor (fixed output voltage), like LT1117.

PS: never tried TI chips

Cheers,

Seb

2011/1/23 phalox <too...@gmail.com>

--
You received this message because you are subscribed to the Google Groups "jallib" group.
To post to this group, send email to jal...@googlegroups.com.
To unsubscribe from this group, send email to jallib+un...@googlegroups.com.
For more options, visit this group at http://groups.google.com/group/jallib?hl=en.

[funlw65(Vasi)]

Hi Seb,

If you make the LED selectable, then no pin sacrifice at all and then
no matter which pin...well, the most used peripherals must be avoided.

Anyway, what about RC2? (Digital 13 LED on FreeJALduino) - it can be a
choice also for future Pinguinos... (why not to be us the ones which
will design also the future Pinguino board - even if is named Jaluino
"code_name_here").

Vasi

On Jan 23, 2:36 pm, Sebastien Lelong <sebastien.lel...@gmail.com>
wrote:

> > jallib+un...@googlegroups.com<jallib%2Bunsu...@googlegroups.com>
> > .

[funlw65(Vasi)]

On Jan 23, 2:36 pm, Sebastien Lelong <sebastien.lel...@gmail.com>
wrote:

> LM317
> can do many voltage output, that's why I chose it, but I still wonder if
> it'll be powerful enough. In doubt, its pin layout is compatible with other
> nice regultor (fixed output voltage), like LT1117.
>

Is powerful enough but the problem is the heat when you use LEDs, and
4x7segments digits or other hungry consumers - then the option to
bypass on board regulators is great. Would be better to be available
as normal jumpers...

Vasi

>
> 2011/1/23 phalox <too...@gmail.com>
>
>
>
> > Maybe take this one into your design too?
>
> > It's pin compatible with the 2550, it only needs some capacitors, and
> > a different supply.
> > So one pcb would make 2 nice boards... one rated at 5V, the other at
> > 3.3
>
> > Just an idea but I think it would be very nice!
>
> > ps: ever tried to write the names of those µC delivered with the TI
> > launchpad?
> > MSP430G2211IN14
>
> > --
> > You received this message because you are subscribed to the Google Groups
> > "jallib" group.
> > To post to this group, send email to jal...@googlegroups.com.
> > To unsubscribe from this group, send email to

> > jallib+un...@googlegroups.com<jallib%2Bunsu...@googlegroups.com>
> > .

[Sebastien Lelong]

Yeah, LM317 should be far enough, I must have mistaken with another one..

Cheers

Seb

2011/1/23 funlw65(Vasi) <fun...@gmail.com>

To unsubscribe from this group, send email to jallib+un...@googlegroups.com.

For more options, visit this group at http://groups.google.com/group/jallib?hl=en.

--

[Sebastien Lelong]

Indeed, RC2 seems a more reasonable option for onboard LED pin.

Regarding Pinguino, I know some users use Jaluino with Pinguino IDE.

Seb

2011/1/23 funlw65(Vasi) <fun...@gmail.com>

To unsubscribe from this group, send email to jallib+un...@googlegroups.com.

For more options, visit this group at http://groups.google.com/group/jallib?hl=en.

--

[vasile surducan]

LM317 need Vin=Vout+3V to work properly. 

http://www.national.com/ds/LM/LM117.pdf  page5

Your schematic is redundant, why do you need two LM317 since only one VDD level is used (+3V3 OR +5V)?

use the jumper on the R8, without jumper you'll have +5V, with jumper make R8 parallel with R8a so the equivalent resistor will be 390 and you'll have 3V3 at the output.

In that way you cut down three silly jumpers: SJ6, SJ7 and SJ8 and replace those with one.

Vasile 

--

[funlw65(Vasi)]

On Jan 23, 4:58 pm, vasile surducan <vsurdu...@gmail.com> wrote:
> LM317 need Vin=Vout+3V to work properly.http://www.national.com/ds/LM/LM117.pdf page5

>
> Your schematic is redundant, why do you need two LM317 since only one VDD
> level is used (+3V3 OR +5V)?
> use the jumper on the R8, without jumper you'll have +5V, with jumper make
> R8 parallel with R8a so the equivalent resistor will be 390 and you'll have
> 3V3 at the output.
>

He he, brilliant!

Vasi

> In that way you cut down three silly jumpers: SJ6, SJ7 and SJ8 and replace
> those with one.
>
> Vasile
>
> On Sat, Jan 22, 2011 at 6:33 AM, Sebastien Lelong <
>

> > jallib+un...@googlegroups.com<jallib%2Bunsu...@googlegroups.com>
> > .

[Sebastien Lelong]

Hi Vasile,

Thanks for your feedback.

2011/1/23 funlw65(Vasi) <fun...@gmail.com>

On Jan 23, 4:58 pm, vasile surducan <vsurdu...@gmail.com> wrote:

> LM317 need Vin=Vout+3V to work properly.http://www.national.com/ds/LM/LM117.pdf page5

 

>
> Your schematic is redundant, why do you need two LM317 since only one VDD
> level is used (+3V3 OR +5V)?
> use the jumper on the R8, without jumper you'll have +5V, with jumper make
> R8 parallel with R8a so the equivalent resistor will be 390 and you'll have
> 3V3 at the output.

OK, I see what you mean, but, in some cases, the two LM317 may not be redundant: power your PIC with 5V (Vdd=5V) but also power Xbee module with 3.3V.

 

Cheers,

Seb

2011/1/23 vasile surducan <vsur...@gmail.com>

LM317 need Vin=Vout+3V to work properly. 

http://www.national.com/ds/LM/LM117.pdf  page5

Ah.... I can remember having read drop voltage was 1.3V, I must have been confused again. Thanks for pointing this. Any hint for an adjutable voltage reg like this, for replacement ?

 

Your schematic is redundant, why do you need two LM317 since only one VDD level is used (+3V3 OR +5V)?

use the jumper on the R8, without jumper you'll have +5V, with jumper make R8 parallel with R8a so the equivalent resistor will be 390 and you'll have 3V3 at the output.

OK, I see what you mean and thought about that, but, in some cases, the two LM317 may not be redundant: power your PIC with 5V (Vdd=5V) but also power Xbee module with 3.3V. But you're right, it's kind of confusing. I'm still not sure about the power supply part, and don't want to make decision in the early stage.

Cheers

Seb

[Sebastien Lelong]

2011/1/23 Sebastien Lelong <sebastie...@gmail.com>

On Jan 23, 4:58 pm, vasile surducan <vsurdu...@gmail.com> wrote:

> LM317 need Vin=Vout+3V to work properly.http://www.national.com/ds/LM/LM117.pdf page5

Ah.... I can remember having read drop voltage was 1.3V, I must have been confused again. Thanks for pointing this. Any hint for an adjutable voltage reg like this, for replacement ? 

Maybe I should just use two different voltage regulator, one AMS1117/5V and AMS1117/3V3. Having only one component would have helped while sourcing them.

Also, what do you think about having standard 0.1" pitch jumpers, usable with pin headers (big but flexible), and potentially use 0805 0 ohm resistors instead (small, but more definitive). I hope you understand what I mean. Is it doable ? (I don't even want to ask if it's standard, but, maybe there's another better/standard option).

TIA

Seb

[Oliver Seitz]

>Also, what do you think about having standard 0.1" pitch jumpers, usable with pin headers (big but flexible), and potentially use 0805 0 ohm resistors instead (small, but more definitive). I hope you understand what I mean. Is it doable ? (I don't even want to ask if it's standard, but, maybe there's another better/standard option).

There are not-so-common 2.0mm jumpers that are somewhat smaller than the 0.1" types. But I for myself, I do have solder sucking wick, so solder jumpers would do for me. You can close and open them again, multiple times. I don't see it as a problem. If resistor pads were used, I'd solder a piece of wire there, no resistor. Wire is easier to remove than a real smd resistor.

For the voltage regulator, you could use an adjustable low-dropout type, like TS1117, but there are drawbacks like maximum input voltage=7V, minimum load current=10mA.

Greets,
Kiste

[Sebastien Lelong]

Hi guys,

So I'm about to change voltage regulators to dedicated ones (no more adjustable). I'd use AMS1117-5V and AMS1117-3.3V. These requires 22µF output filtering capacitors, tantalum ones. Just my curiosity: is tantalum really needed ? Or "standard" aluminium electrolytic ones enough ? (can be cheaper). I read tantalum's are smaller and more reliable. Do E-cap, C-cap, ... form factors (I think that's the name) often used in SMD design ? they really just look like PTH caps and seem very tall: http://rocky.digikey.com/weblib/Nichicon/Web%20photos/UD%20SERIES%204.0,5.8.jpg

I would have kept 100nF input capacitors, but datasheet doesn't mention it's required or recommended.

I've also replaced solder jumper with "standard" PTH jumper, this way, if prefered, soldering a wire is still possible.

Cheers,

Seb

2011/1/23 Oliver Seitz <karl...@yahoo.com>

--
You received this message because you are subscribed to the Google Groups "jallib" group.
To post to this group, send email to jal...@googlegroups.com.

To unsubscribe from this group, send email to jallib+un...@googlegroups.com.

For more options, visit this group at http://groups.google.com/group/jallib?hl=en.

[Oliver Seitz]

> Just my curiosity: is tantalum really needed ? Or "standard" aluminium electrolytic ones enough ? (can be cheaper). I read tantalum's are smaller and more reliable.

Tantalum combines high capacity (electrolytic) with very good high-frequency performance, almost like ceramic. Instead of a tantalum, you could usually use a standard electrolytic in parallel with a ceramic, but it's two parts then.

Greets,
Kiste

[funlw65(Vasi)]

How you will connect the board to shields and/or modules?

On Jan 24, 6:04 pm, Sebastien Lelong <sebastien.lel...@gmail.com>
wrote:

> Hi guys,
>
> So I'm about to change voltage regulators to dedicated ones (no more
> adjustable). I'd use AMS1117-5V and AMS1117-3.3V. These requires 22µF output
> filtering capacitors, tantalum ones. Just my curiosity: is tantalum really
> needed ? Or "standard" aluminium electrolytic ones enough ? (can be
> cheaper). I read tantalum's are smaller and more reliable. Do E-cap, C-cap,
> ... form factors (I think that's the name) often used in SMD design ? they

> really just look like PTH caps and seem very tall:http://rocky.digikey.com/weblib/Nichicon/Web%20photos/UD%20SERIES%204...

>
> I would have kept 100nF input capacitors, but datasheet doesn't mention it's
> required or recommended.
>
> I've also replaced solder jumper with "standard" PTH jumper, this way, if
> prefered, soldering a wire is still possible.
>
> Cheers,
> Seb
>

> 2011/1/23 Oliver Seitz <karlki...@yahoo.com>

>
>
>
> > >Also, what do you think about having standard 0.1" pitch jumpers, usable
> > with pin headers (big but flexible), and potentially use 0805 0 ohm
> > resistors instead (small, but more definitive). I hope you understand what I
> > mean. Is it doable ? (I don't even want to ask if it's standard, but, maybe
> > there's another better/standard option).
>
> > There are not-so-common 2.0mm jumpers that are somewhat smaller than the
> > 0.1" types. But I for myself, I do have solder sucking wick, so solder
> > jumpers would do for me. You can close and open them again, multiple times.
> > I don't see it as a problem. If resistor pads were used, I'd solder a piece
> > of wire there, no resistor. Wire is easier to remove than a real smd
> > resistor.
>
> > For the voltage regulator, you could use an adjustable low-dropout type,
> > like TS1117, but there are drawbacks like maximum input voltage=7V, minimum
> > load current=10mA.
>
> > Greets,
> > Kiste
>
> > --
> > You received this message because you are subscribed to the Google Groups
> > "jallib" group.
> > To post to this group, send email to jal...@googlegroups.com.
> > To unsubscribe from this group, send email to

> > jallib+un...@googlegroups.com<jallib%2Bunsu...@googlegroups.com>
> > .

> > For more options, visit this group at
> >http://groups.google.com/group/jallib?hl=en.
>
> --
> Sébastien Lelonghttp://www.sirloon.nethttp://sirbot.org
>

>  jaluino_v02_bee_schematic.png
> 60KViewDownload

[Sebastien Lelong]

With pin header I must add ! But you're right, better adding them right now before I forget (and I'm starting to...)

Cheers,

Seb 

2011/1/24 funlw65(Vasi) <fun...@gmail.com>

To unsubscribe from this group, send email to jallib+un...@googlegroups.com.

For more options, visit this group at http://groups.google.com/group/jallib?hl=en.

--

[mattschinkel]

> Maybe I should just use two different voltage regulator, one AMS1117/5V and
> AMS1117/3V3. Having only one component would have helped while sourcing
> them.

On one prototype board I bought, there is only a AMS1117/3V3. They
assume you want to input > 5v and get 3v output. If you want another
voltage you can put a jumper (just solder) to connect the input/output
of the regulator so your voltage is whatever the input is.

Matt.

[Sebastien Lelong]

Hi guys,

Here's my last version, including a 500mA fuse (not resettable, but I only have this one in my eagle lib), a rectifier diode for reverse polarity protection, onboard LED moved to RC2 (CCP1 pin). Some remaining "doubts":

  - which package would I need for the diode: DO-214AA, DO-214-AB or DO-214AC ?

  - I still have doubts about the power supply part. Initially, I wanted to have power through USB or a battery. The board should handle 3.3V and 5V, as an option. When using a battery, say 2 x 1.5V AAA cells, I'd need to bypass all regulation (maybe even a pump like this: http://www.sparkfun.com/products/9216). Using a rectifier diode will also drop the voltage down and may not be compatible. But I could also use a 9V battery, and thus need 5V and/or 3.3V regulators... and what if 3.3V is bypassed, but not the 5V regulator ? Xbee board will be powered with 5V, instead of 3.3V!!! You guessed it, I want many things and I'm not sure which is most important at this phase. Any input, advices ? I think when I'll start to create the PCB choices will be easier to make as I discard options to gain room :)

  - I added pin headers, 2 x 14 pins, I may add another one dedicated to power pins (like in Medium) if I get enough room (I doubt about it)

In order to save some precious room, I'm thinking of (high priority to low):

  - removing Reset-via-RTS option and make it always available (2-way jumper saved)

  - remove two I²C jumpers, always make the board acting as a master, and if not wanted, just don't solder the resistors

  - remove CTS jumper option (not used often ?)

  - remove power from serial module option, focusing on USB or battery

  - keep only one regulator, adding an optional resistor to match required 3.3V for Xbee when using 5V reg only.

  - move to 0603 smd components.....

Any feedback highly appreciated!

TIA

Cheers,

Seb

2011/1/25 mattschinkel <mattsc...@hotmail.com>

[funlw65(Vasi)]

I think you will need to design two boards. One supporting USB uCs and
second for serial uCs. Keep 1206 smd components, otherwise you must
provide the board assembled. And this is because of 5x5mm limit. Try
to see how many features you can put on a single type of board.

Vasi

On Jan 29, 6:03 am, Sebastien Lelong <sebastien.lel...@gmail.com>
wrote:

> 2011/1/25 mattschinkel <mattschin...@hotmail.com>

>
> > > Maybe I should just use two different voltage regulator, one AMS1117/5V
> > and
> > > AMS1117/3V3. Having only one component would have helped while sourcing
> > > them.
>
> > On one prototype board I bought, there is only a AMS1117/3V3. They
> > assume you want to input > 5v and get 3v output. If you want another
> > voltage you can put a jumper (just solder) to connect the input/output
> > of the regulator so your voltage is whatever the input is.
>
> > Matt.
>
> > --
> > You received this message because you are subscribed to the Google Groups
> > "jallib" group.
> > To post to this group, send email to jal...@googlegroups.com.
> > To unsubscribe from this group, send email to

> > jallib+un...@googlegroups.com<jallib%2Bunsu...@googlegroups.com>
> > .

> > For more options, visit this group at
> >http://groups.google.com/group/jallib?hl=en.
>
>
>

>  jaluino_v03_bee_schematic.png
> 62KViewDownload

[funlw65(Vasi)]

Hi Seb,


Thinking at your Jaluino Medium, I found this tread:
http://www.cnczone.com/forums/attachment.php?attachmentid=85952&d=1249734850

[vasile surducan]

On Sat, Jan 29, 2011 at 10:49 AM, funlw65(Vasi) <fun...@gmail.com> wrote:

I think you will need to design two boards. One supporting USB uCs and
second for serial uCs. Keep 1206 smd components, otherwise you must
provide the board assembled. And this is because of 5x5mm limit.

 

Try
to see how many features you can put on a single type of board.

all you need... 

Vasile

To unsubscribe from this group, send email to jallib+un...@googlegroups.com.

[Sebastien Lelong]

Hi guys,

So...I'm back, after several tries.

It was possible to keep most features, specifically providing 2 voltages, 5V and 3.3V. This was quite a mess though, mostly Xbee requires 3.3V, and possibly voltage shifter on inputs (datasheet says it's not 5V tolerant, but some report it is in reality). So I removed 5V regulation, and kept only 3.3V, making this board more 3.3V devices friendly. If Xbee isn't wanted, then one would just put an AMS1117-5V instead of 3.3V version.

I worked again on power supply inputs. There can be 4 sources: USB (5V regulated to 3.3V), external (5-9V regulated to 3.3V), serial (no regulation so must output 3.3V, quite rare), and battery (direct, no regulation). I put a fuse after the regulation part.

Since I had some room left, I added a microSD slot, though I still wonder how I'll solder it... :) It's on the bottom side. If replacing 3.3V regulator with a 5V one, again SD-card won't work.

I doubled shield/breadboard connectors to allow breadboard + shields at the same time. User could also solder some wires to plug the board to external daughter, using external connectors/holes. Shields can also be on top or bottom, both, etc...

I may also add another pin header which would include supplied voltage, making it available to shields/breadboard (voltage coming from USB, external, ...).

Anyway here's the result, see attached files: schematic, PCB, PCB top, PCB bottom (some comments are wrong, sorry).

Feedback appreciated. Highly !

Cheers,

Seb

2011/1/30 vasile surducan <vsur...@gmail.com>

[funlw65(Vasi)]

Very nice looking board, I like it. Still, hard to made. Some traces
can be manually repositioned to have a little more space between them.
If is about 8mills traces-space then better to have them in a less
number - a reduced number of fabrication errors ...
Anyway, I like it (good to have two rows of connectors - can be
combined with male-female ones).

Vasi

On Feb 4, 11:59 am, Sebastien Lelong <sebastien.lel...@gmail.com>
wrote:
> Hi guys,
>

> 2011/1/30 vasile surducan <vsurdu...@gmail.com>

> >> <jallib%2Bunsu...@googlegroups.com<jallib%252Buns...@googlegroups.com>

>
> >> > > .
> >> > > For more options, visit this group at
> >> > >http://groups.google.com/group/jallib?hl=en.
>
> >> >  jaluino_v03_bee_schematic.png
> >> > 62KViewDownload
>
> >> --
> >> You received this message because you are subscribed to the Google Groups
> >> "jallib" group.
> >> To post to this group, send email to jal...@googlegroups.com.
> >> To unsubscribe from this group, send email to
> >> jallib+un...@googlegroups.com<jallib%2Bunsu...@googlegroups.com>
> >> .
> >> For more options, visit this group at
> >>http://groups.google.com/group/jallib?hl=en.
>
> >  --
> > You received this message because you are subscribed to the Google Groups
> > "jallib" group.
> > To post to this group, send email to jal...@googlegroups.com.
> > To unsubscribe from this group, send email to
> > jallib+un...@googlegroups.com<jallib%2Bunsu...@googlegroups.com>
> > .
> > For more options, visit this group at
> >http://groups.google.com/group/jallib?hl=en.
>

> --
> Sébastien Lelonghttp://www.sirloon.nethttp://sirbot.org
>

>  jaluino_v04_bee_schematic.png
> 75KViewDownload
>
>  jaluino_v04_bee_pcb.png
> 43KViewDownload
>
>  jaluino_v04_bee_pcb_top.png
> 33KViewDownload
>
>  jaluino_v04_bee_pcb_bottom.png
> 24KViewDownload

[vasile surducan]

On Fri, Feb 4, 2011 at 8:59 AM, Sebastien Lelong <sebastie...@gmail.com> wrote:

Hi guys,

So...I'm back, after several tries.

It was possible to keep most features, specifically providing 2 voltages, 5V and 3.3V. This was quite a mess though, mostly Xbee requires 3.3V, and possibly voltage shifter on inputs (datasheet says it's not 5V tolerant, but some report it is in reality). So I removed 5V regulation, and kept only 3.3V, making this board more 3.3V devices friendly. If Xbee isn't wanted, then one would just put an AMS1117-5V instead of 3.3V version.

I worked again on power supply inputs. There can be 4 sources: USB (5V regulated to 3.3V), external (5-9V regulated to 3.3V), serial (no regulation so must output 3.3V, quite rare), and battery (direct, no regulation). I put a fuse after the regulation part.

Since I had some room left, I added a microSD slot, though I still wonder how I'll solder it... :) It's on the bottom side. If replacing 3.3V regulator with a 5V one, again SD-card won't work.

I doubled shield/breadboard connectors to allow breadboard + shields at the same time. User could also solder some wires to plug the board to external daughter, using external connectors/holes. Shields can also be on top or bottom, both, etc...

I may also add another pin header which would include supplied voltage, making it available to shields/breadboard (voltage coming from USB, external, ...).

Anyway here's the result, see attached files: schematic, PCB, PCB top, PCB bottom (some comments are wrong, sorry).

Feedback appreciated. Highly !

   Your designs looks better and better. However there is HUGE empty space on your board. Look for example the footbal field between the crystal and the micro. 

When using SMD one of the reason is miniaturization. But your board is still huge.

You cand do it with only 20% larger than the xbee itself?

Vasile

[Sebastien Lelong]

Hi Vasi,

Thanks for your feedback. Can you point me to these traces that could be repositioned ? I'm planning to manufacture it with Seeedstudio. Minimum requirements are 6mil space and 6mil width. I used 10mil for traces, sometimes 16mil for power traces.

Cheers,

Seb

2011/2/5 funlw65(Vasi) <fun...@gmail.com>

To unsubscribe from this group, send email to jallib+un...@googlegroups.com.

For more options, visit this group at http://groups.google.com/group/jallib?hl=en.

--

[Sebastien Lelong]

Hi Vasile,

Thanks for your feedback too !

Are you saying it's possible to make such a board only 20% greater than Xbee ? I could try to redesign it, but the bottleneck will pin header connectors. Also, on my first tries, there were many many vias, and I tried to have as few as possible. Going that small will mean more vias. Is this a problem ? For instance, PIC's datasheet says caps near xtal should on the same side. I tried to respect this.

What about the fuse ? Do you think it's properly positioned ? Since there are many power source options, I can't put a fuse for each...

Cheers,

Seb

2011/2/5 vasile surducan <vsur...@gmail.com>

[vasile surducan]

Hi Seb,

On Sat, Feb 5, 2011 at 1:48 AM, Sebastien Lelong <sebastie...@gmail.com> wrote:

Hi Vasile,

Thanks for your feedback too !

Are you saying it's possible to make such a board only 20% greater than Xbee ? I could try to redesign it, but the bottleneck will pin header connectors.

  true, you've chosen a header which is a compromise between size and space. 

 

Also, on my first tries, there were many many vias, and I tried to have as few as possible. Going that small will mean more vias. Is this a problem ? For instance, PIC's datasheet says caps near xtal should on the same side. I tried to respect this.

of course but you can use as well a SMD crystal on the micro side or on the opposite side as well

 

What about the fuse ? Do you think it's properly positioned ? Since there are many power source options, I can't put a fuse for each...

well, I dislike your style of powering board (JP3 and JP7 both ON by mistake could kill your USB) but that is, usually the fuse is protected by the micro or by the regulator, however one smd fuse (thermal or breackable) is enough, but I'm affraid yours will not protect something...

About jumpers, a good board has the smallest possible number of jumpers and variable resistors... even using 1-2 transistors instead of 3 jumpers is often better (mostly when the board is designed for beginners).

To unsubscribe from this group, send email to jallib+un...@googlegroups.com.

[Sebastien Lelong]

2011/2/5 vasile surducan <vsur...@gmail.com>

Also, on my first tries, there were many many vias, and I tried to have as few as possible. Going that small will mean more vias. Is this a problem ? For instance, PIC's datasheet says caps near xtal should on the same side. I tried to respect this.

of course but you can use as well a SMD crystal on the micro side or on the opposite side as well

Ye, I found smd crytal not so easy to find and quite expensive too. I found resonator too, but this may not be accurate enough in some cases.

 

 

What about the fuse ? Do you think it's properly positioned ? Since there are many power source options, I can't put a fuse for each...

well, I dislike your style of powering board (JP3 and JP7 both ON by mistake could kill your USB)

I'm not happy too with this. I thought about this a lot, without good results as you can see. I could remove external source, thus removing JP7.

 

but that is, usually the fuse is protected by the micro or by the regulator, however one smd fuse (thermal or breackable) is enough, but I'm afraid yours will not protect something...

So where do you suggest to put it ? BTW symbol is resettable but I'm planning to use "real" smd fuse.

[vasile surducan]

On Sat, Feb 5, 2011 at 2:46 AM, Sebastien Lelong <sebastie...@gmail.com> wrote:

2011/2/5 vasile surducan <vsur...@gmail.com>

Also, on my first tries, there were many many vias, and I tried to have as few as possible. Going that small will mean more vias. Is this a problem ? For instance, PIC's datasheet says caps near xtal should on the same side. I tried to respect this.

of course but you can use as well a SMD crystal on the micro side or on the opposite side as well

Ye, I found smd crytal not so easy to find and quite expensive too. I found resonator too, but this may not be accurate enough in some cases.

 

 

What about the fuse ? Do you think it's properly positioned ? Since there are many power source options, I can't put a fuse for each...

well, I dislike your style of powering board (JP3 and JP7 both ON by mistake could kill your USB)

I'm not happy too with this. I thought about this a lot, without good results as you can see. I could remove external source, thus removing JP7.

one compromise: use a three pole jumper, either JP3 or JP7 by one move...

 

 

but that is, usually the fuse is protected by the micro or by the regulator, however one smd fuse (thermal or breackable) is enough, but I'm afraid yours will not protect something...

So where do you suggest to put it ? BTW symbol is resettable but I'm planning to use "real" smd fuse.

There are two unprotected power supplies: the battery which is most aggressive since a short circuit current can go higher than 500mA and the external power supply. Both USB and U1 have short circuit protected outputs.  since you choose to protect only 3V3, then the logic place is in series with external battery. However, there is no reverse voltage protection neither for batter nor external power supply which is bad...

[Sebastien Lelong]

2011/2/5 vasile surducan <vsur...@gmail.com>

I'm not happy too with this. I thought about this a lot, without good results as you can see. I could remove external source, thus removing JP7.

one compromise: use a three pole jumper, either JP3 or JP7 by one move...

I'll try !

 

 

 

but that is, usually the fuse is protected by the micro or by the regulator, however one smd fuse (thermal or breackable) is enough, but I'm afraid yours will not protect something...

So where do you suggest to put it ? BTW symbol is resettable but I'm planning to use "real" smd fuse.

There are two unprotected power supplies: the battery which is most aggressive since a short circuit current can go higher than 500mA and the external power supply. Both USB and U1 have short circuit protected outputs.  since you choose to protect only 3V3, then the logic place is in series with external battery. However, there is no reverse voltage protection neither for batter nor external power supply which is bad...

The trouble with polarity protection (this is what we're talking about isn't ?) is the drop voltage involved with diode. For external power supply, it'd be ok, but for battery, for which I plan to use 2 x AAA cells, I just can't afford it...

The difference between battery and external is just external goes to the 3.3V regulator. I could remove external and put a jumper to select whether to go to the vreg or not. thi would give something like this:

Obviously, the problem is now when you put more than 3.3V (or more) and select no regulation... Maybe I could combine both 2-way jumpers and physically avoid some combination (cut wire, something like that), so when you select USB, at least you have to choose regulation.

Would fuse be properly set in this case ?

Cheers,

Seb

[Oliver Seitz]

>> Both USB and U1 have short circuit protected outputs.  

You mean, power rails on USB connectors at a computer are short-circuit protected? This is true, but the protection is often a non-resettable SMD fuse somewhere in the middle of a very big PCB called mainboard... I'd prefer not to blow that one.

>The trouble with polarity protection (this is what we're talking about isn't ?) is the drop voltage involved with diode.

Only if you're using a diode in series. You could also use the fuse and a reasonably strong schottky diode from ground. So, reverse polarity will not go beyond 0.5V, and the fuse will blow when strong reverse power is applied.

Greets,
Kiste

[Sebastien Lelong]

Hi Kiste,

2011/2/5 Oliver Seitz <karl...@yahoo.com>

>> Both USB and U1 have short circuit protected outputs.  

You mean, power rails on USB connectors at a computer are short-circuit protected? This is true, but the protection is often a non-resettable SMD fuse somewhere in the middle of a very big PCB called mainboard... I'd prefer not to blow that one.

:)

OK, so I can put another SMD fuse for USB.

>The trouble with polarity protection (this is what we're talking about isn't ?) is the drop voltage involved with diode.

Only if you're using a diode in series. You could also use the fuse and a reasonably strong schottky diode from ground. So, reverse polarity will not go beyond 0.5V, and the fuse will blow when strong reverse power is applied.

Thanks for the tip. Could you point to some direction about this diode ?

I was also thinking about using a schottky diode to regulate max 3.3V. I mean, according to my last power supply schematic, if user select USB but no regulation, xbee could be damaged for instance. Could a 3.3V schottky diode be used for thi purpose ? (make sure it won't be more than 3.3V ?)

 

Cheers,

Seb

[Sebastien Lelong]

Or, should I keep another fuse at its first place, after regulation ? I first thought that put this fue here would protect USB (but not the regulation part) and the whole circuit.

Please enlighten me !

Seb 

2011/2/5 Sebastien Lelong <sebastie...@gmail.com>

[Oliver Seitz]

Err, I must admit that I wrote more in general... I haven't had a look at none of the schematics or drawings...

First, to clear a bit confusion:

Schottky: A diode that is usually significantly faster than silicon diodes, and has a lover voltage drop (~ 0.3V). Reverse polarity is however limited, 30V is common. There exist types that can withstand higher voltage, but the speed decreases due to the capacitance.

Zener: A silicon diode that conducts on straight polarity and insulates on reverse. But from a certain ("breakdown") voltage upward, zener diodes start conducting even in reverse polarity. This voltage is not very accurate, and there is a quite soft bend in the curve, no corner, when it starts conducting. It can be used to limit voltages, but in regulation it's usually not the best choice.

>>>The trouble with polarity protection (this is what we're talking about isn't ?) is the drop voltage involved with diode.

>>Only if you're using a diode in series. You could also use the fuse and a reasonably strong schottky diode from ground. So, reverse polarity will not go beyond 0.5V, and the fuse will blow when strong reverse power is applied.

>Thanks for the tip. Could you point to some direction about this diode ?
I was also thinking about using a schottky diode to regulate max 3.3V. I mean, according to my last power supply schematic, if user select USB but no regulation, xbee could be damaged for instance. Could a 3.3V schottky diode be used for thi purpose ? (make sure it won't be more than 3.3V ?)

A resistor+zener diode for regulation eats a lot of power. If you need 100mA at min. 3V while supply is 3.3V, the resistor can be at most 0.3V/0.1A=3 Ohm. If supply is 5.5V then while the zener diode limits to 3.3V, the resistor conducts (5.5-3.3)V/3 Ohm=733mA. That is 1.6 Watt for the resistor, and 2.5 Watt for the zener diode. Quiescent power 4 Watt. Usable as heating, but no micro electronic.

Reverse protection using fuse and "crowbar" diode: I've not seen SMD fuses below 500mA to easily come by. So I feel like protecting the computer-onboard fuse can or can not work. Even a super fast acting fuse can hold double it's rating for up to five seconds. It's pure chance which of two fuses in series will blow. To make sure which fuse blows, you would have to use one rated at most 300mA. But, reverse polarity should not be the main concern on USB, but on other inputs. A 500mA super fast fuse will blow within 5s at 1A and within 1ms at 5A. This is what the crowbar diode must cope with, only occasionally, though. SS12L could be a candidate. It is only rated 1A, but a surge current of 30A for 8ms is specified in the datasheet. It is in DO-219-AB(SMF) package, 2x3mm in size.

Whoops... Looked in a PIC datasheet. Only -0.3V are rated for PICs as absolute maximum. The SS12L will allow about 0.7V while conducting 3A. This might kill the PIC. I do know that PICs die on reverse polarity. But does anyone know if they die within milliseconds when applying only 1V in reverse?

Greets,
Kiste

[vasile surducan]

Seb, it's yours design so you have to enlighten us.

 You want three power supplies: one battery, one external supply, one USB.

The load is one nanowatt PIC and one XBEE which draw max 270mA on TX  and the user unknown load.

 In your opinion the 500mA fuse should protect the load for the extra drawn current, the power supplies or all of them?

Vasile

--

[Sebastien Lelong]

Sure, I understand what you mean. So here's some self-enligthenment :)

I want the board to be safe: it should never damage USB host for instance (this is the most important point). It must also be fool proof: a short circuit should just blow a fuse. Ideally reverse polarity shouldn't be a problem.

I know this is still fuzzy, from what your say, Kiste, blow speed is also important. I just don't have enough knowledge to pick the better solution, the better compromise.

In my opinion, 500mA should protect the load for extra current (user load) *and* board itself (PIC, etc...) *and* the power supplies.

Cheers,

Seb  

2011/2/5 vasile surducan <vsur...@gmail.com>

Seb, it's yours design so you have to enlighten us.

[Sebastien Lelong]

2011/2/5 Oliver Seitz <karl...@yahoo.com>

Err, I must admit that I wrote more in general... I haven't had a look at none of the schematics or drawings...

First, to clear a bit confusion:

Schottky: A diode that is usually significantly faster than silicon diodes, and has a lover voltage drop (~ 0.3V). Reverse polarity is however limited, 30V is common. There exist types that can withstand higher voltage, but the speed decreases due to the capacitance.

Zener: A silicon diode that conducts on straight polarity and insulates on reverse. But from a certain ("breakdown") voltage upward, zener diodes start conducting even in reverse polarity. This voltage is not very accurate, and there is a quite soft bend in the curve, no corner, when it starts conducting. It can be used to limit voltages, but in regulation it's usually not the best choice.

Yeah sorry, I meant Zener. Thanks for the clarifications. Ideally what I would to do, when add Vdd level (output of regulator or direct output, near "Vdd" arrow ), is:

if voltage <= 3.3V then

    Vdd = voltage

else

    Vdd = 3.3V

end if

 

:)

Cheers

Seb

[Sebastien Lelong]

Typically I wanted to use this kind of fuse: http://cgi.ebay.com/10pcs-Little-fuse-notebook-repair-LF-Fuse-SMD-1206-0-5A-/220725125732?pt=LH_DefaultDomain_0&hash=item33643e2264#ht_1113wt_754

[vasile surducan]

take a look to the attach, maybe will be useful if understand.

vasile

[Sebastien Lelong]

OK, this one should protect both battery and USB (not considering blow speed):

If it sounds ok to you, I'll keep this one.

cheers,

seb

2011/2/5 Sebastien Lelong <sebastie...@gmail.com>

[Sebastien Lelong]

Thanks !

Why using a coil (L1 ?) with USB ? And how it's 1A protected while using 0.8A fuse ?

So, I understand you're using 2 zener diodes 20V/1A for polarity protection, is that right ? 

Cheers

[vasile surducan]

On Sat, Feb 5, 2011 at 10:30 AM, Sebastien Lelong <sebastie...@gmail.com> wrote:

Thanks !

Why using a coil (L1 ?) with USB ?

L1 + C2 is a filter, for the noise coming from the computer. Also the USB connector ground can be AC or DC coupled to avoid noises, read the USB2.0 specifications...

 

And how it's 1A protected while using 0.8A fuse ?

because a 0.8A regular fuse will never blow at 0.8 A, but you need 20 years of work and 1000 fuses to know that (or a good fuse datasheet to read before starting your design)

So, I understand you're using 2 zener diodes 20V/1A for polarity protection, is that right ? 

you still don't know (after Oliver's message) which is difference between a zener symbol and a schottky simbol and still trying to design board for selling, capitalist economy it's amazing ...fortunately the buyers will don't know either those un-interesting things...

A schottky is protecting the silly user only for reversing the polarity of the power supply, by blowing the fuse if it's reversed. A zener needs a series resistor to limit the current after the voltage is increased above the zenner thresold limit.

Vasile

[Sebastien Lelong]

2011/2/6 vasile surducan <vsur...@gmail.com>

 

And how it's 1A protected while using 0.8A fuse ?

because a 0.8A regular fuse will never blow at 0.8 A, but you need 20 years of work and 1000 fuses to know that (or a good fuse datasheet to read before starting your design)

So I'd need 300mA to protect 500mA ?... Or I could 500mA knowing it'll blow at 800mA

 

So, I understand you're using 2 zener diodes 20V/1A for polarity protection, is that right ? 

you still don't know (after Oliver's message) which is difference between a zener symbol and a schottky simbol

Yes I do. Yours didn't look like Zener ones, but the "DZ" (ooops, D2) and the symbol trace fading way confused me (I had to use the same magnifier as the one I used to smd solder :))

 

and still trying to design board for selling, capitalist economy it's amazing ...

Impressive, I was wondering how many more posts you'd need before talking about capitalist economy :) Oh, should I repeat there's no profit around this project ? That makes it less capitalist, maybe...

If you had read "The Cathedral and the Bazaar", you'd know how open source project communities work, the same applied to open hardware projects. Many human societies are based on owning things: the bigger and most, the better. There are different types of levels. In this book they also talk about another society (can't remember the name), this time based on gifts: the bigger the gift, the more valuable, the better, you, the giver, will be recognized as an important person in this society. Open source projects are le that (not every os projects though), so are open hardware projects. But for the latter, there's often some money around, as it's material. You can't download a PCB, unfortunately. S

Well, you already know all of that, and I know you're joking. What you still don't know is I'm not trying to design boards for selling.

And what could I say now ? Well, thanks Vasile for your highly valuable gift :)

fortunately the buyers will don't know either those un-interesting things...

maybe, maybe not. I never expect anything from people who would be interested (call them "buyers").

 

A schottky is protecting the silly user only for reversing the polarity of the power supply, by blowing the fuse if it's reversed. A zener needs a series resistor to limit the current after the voltage is increased above the zenner thresold limit.

OK, thanks also for the gift wrap :) 

So, reading Kiste's post, Shottky diodes have a lower drop voltage than other diodes, typically 0.3V. This means I'll have 3V - 0.3V = 2.7V when using battery, is that right ?

If I add a schottky diode to my last power supply proposal, I can save one fuse and one diode.

[Oliver Seitz]

>So I'd need 300mA to protect 500mA ?... Or I could 500mA knowing it'll blow at 800mA 

It takes it's time to blow a fuse. For a super fast acting SMD fuse I already gave some numbers, here a bit more detail, example is a 500mA fuse:

It will *not* blow within 1 hour at 625mA,
it will blow in less than 5 sec. at 1000mA,
it will blow in less than 1 msec. at 5A.

Some numbers for a time-lag fuse:

It will *not* blow within 4 hours at 500mA,
it will blow in less than 5 sec. at 1000mA,
at 5 A it will blow in less than 100ms, but not before 10ms.

So, if you put those two in series, only the super fast fuse will blow at very high currents, while at modest overload any of the two can blow. If you want to protect a 500mA fuse in your computer, you would have to use an external fuse rated not higher than 300mA.

There are books about connecting fuses in series :-)

Greets,
Kiste

[Sebastien Lelong]

Hi Kiste,

Thanks for the figures. I hope not to forget them :)

I had a look at last Arduino design (Uno). They use a 500mA polyfuse, resettable, claiming it'll add a proctection layer, in addition to the one included in USB host. From Jaluino Medium discussion, I understood polyfuse doesn't act fast enough, that's why it uses a "standard" one. This would make two reasons Arduino wouldn't be suitable to USB regarding fuse protection. Unfortunately, polyfuses remain the most interesting option: easy to find, small, reusable...

Cheers,

Seb

2011/2/6 Oliver Seitz <karl...@yahoo.com>

--
You received this message because you are subscribed to the Google Groups "jallib" group.
To post to this group, send email to jal...@googlegroups.com.
To unsubscribe from this group, send email to jallib+un...@googlegroups.com.
For more options, visit this group at http://groups.google.com/group/jallib?hl=en.

[funlw65(Vasi)]

Hi Seb,

The board will be less general with the two 4k7 resistors on RB1-2...
BTW, is here a chance to have a Software SPI library?

Vasi

On Feb 6, 1:48 pm, Sebastien Lelong <sebastien.lel...@gmail.com>
wrote:

> Hi Kiste,
>
> Thanks for the figures. I hope not to forget them :)
>
> I had a look at last Arduino design (Uno). They use a 500mA polyfuse,
> resettable, claiming it'll add a proctection layer, in addition to the one
> included in USB host. From Jaluino Medium discussion, I understood polyfuse
> doesn't act fast enough, that's why it uses a "standard" one. This would
> make two reasons Arduino wouldn't be suitable to USB regarding fuse
> protection. Unfortunately, polyfuses remain the most interesting option:
> easy to find, small, reusable...
>
> Cheers,
> Seb
>

> 2011/2/6 Oliver Seitz <karlki...@yahoo.com>

[Sebastien Lelong]

Hi Vasi,

2011/2/6 funlw65(Vasi) <fun...@gmail.com>

The board will be less general with the two 4k7  resistors on RB1-2...

Arf... These were supposed to be I²C pull-up resistors, but they aren't connected to the correct pins ! Nice catch, thanks, I'll fix this asap ! If you don't want this feature, just don't solder resistors, that's the idea.

BTW I tried to move traces and add more spaces as you suggested. I'll post the result soon.

cheers,

Seb 

[Sebastien Lelong]

18F27J53 has two MSSP modules. MSSP1 can be used for both I²C and SPI, while MSSP2 can only be used for SPI. Since I want i²C, and SPI for embedded sd-card, I²C must use RB4 and RB5 pins (pullups for SDA1 and SCL1).

I thus need to use different pins for SPI. MSSP2 has remappable pins (RPn pins on datasheets, see screenshot). Interesting feature, I'm supposed to select whatever remappable pins needed for SPI... Need more thoughts, but I think I'll remap them on RP2, RP11, RP12 and RP13.

Datasheet reading.........

Cheers,

Seb

2011/2/6 Sebastien Lelong <sebastie...@gmail.com>

[funlw65(Vasi)]

Start thinking what features will have a Jaluino board with
18F47J53... (I would like to be able tu use RTC,, useful for a SD Card
logger). Then start cutting for a smaller board as Jaluino BEE (Pinout
is very important - where is possible). So, better to start with a
10x10cm board ? ;)

Vasi

On Feb 6, 6:02 pm, Sebastien Lelong <sebastien.lel...@gmail.com>
wrote:

> 18F27J53 has two MSSP modules. MSSP1 can be used for both I²C and SPI, while
> MSSP2 can only be used for SPI. Since I want i²C, and SPI for embedded
> sd-card, I²C must use RB4 and RB5 pins (pullups for SDA1 and SCL1).
>
> I thus need to use different pins for SPI. MSSP2 has remappable pins (RPn
> pins on datasheets, see screenshot). Interesting feature, I'm supposed to
> select whatever remappable pins needed for SPI... Need more thoughts, but I
> think I'll remap them on RP2, RP11, RP12 and RP13.
>
> Datasheet reading.........
>
> [image: 18f27j53.png]
>
> Cheers,
> Seb
>

> 2011/2/6 Sebastien Lelong <sebastien.lel...@gmail.com>
>
>
>
> > Hi Vasi,
>
> > 2011/2/6 funlw65(Vasi) <funl...@gmail.com>

>
> >> The board will be less general with the two 4k7  resistors on RB1-2...
>
> > Arf... These were supposed to be I²C pull-up resistors, but they aren't
> > connected to the correct pins ! Nice catch, thanks, I'll fix this asap ! If
> > you don't want this feature, just don't solder resistors, that's the idea.
>
> > BTW I tried to move traces and add more spaces as you suggested. I'll post
> > the result soon.
>
> > cheers,
> > Seb
>
> --
> Sébastien Lelonghttp://www.sirloon.nethttp://sirbot.org
>

>  18f27j53.png
> 56KViewDownload

[Sebastien Lelong]

2011/2/6 funlw65(Vasi) <fun...@gmail.com>

Start thinking what features will have a Jaluino board with
18F47J53... (I would like to be able tu use RTC,, useful for a SD Card
logger).

18F27J53 has built-in RTC, this is one reason why I chose it (indeed for data logger, that's also why I wanted to put sd card if possible (microsd).

 

Then start cutting for a smaller board as Jaluino BEE (Pinout
is very important - where is possible). So, better to start with a
10x10cm board ? ;)

OK I see what you mean, but I'm driven by costs. 10x10cm PCBs aren't that expensive, still twice the price as 5x5cm. Or, reading it on the other side, 5x5cm PCBs are very, very cheap. I hope to build a board for less than $10/$12, components + PCB all included.

PS: btw note 18f47j53 is only available on QFN package. Much harder to solder, would require specific equipment.

Cheers

Seb

--

You received this message because you are subscribed to the Google Groups "jallib" group.
To post to this group, send email to jal...@googlegroups.com.
To unsubscribe from this group, send email to jallib+un...@googlegroups.com.
For more options, visit this group at http://groups.google.com/group/jallib?hl=en.

[funlw65(Vasi)]

> OK I see what you mean, but I'm driven by costs. 10x10cm PCBs aren't that
> expensive, still twice the price as 5x5cm. Or, reading it on the other side,
> 5x5cm PCBs are very, very cheap. I hope to build a board for less than
> $10/$12, components + PCB all included.

I think it will fit in 5x5cm with SD card but no XBEE:
http://www.adelaida.ro/product_info.php?products_id=11928&osCsid=037c0dd113d36e13790d335451ccfb12

but...

>
> PS: btw note 18f47j53 is only available on QFN package. Much harder to
> solder, would require specific equipment.

only with 18F46J50 then :(

[Sebastien Lelong]

2011/2/6 funlw65(Vasi) <fun...@gmail.com>

I think it will fit in 5x5cm with SD card but no XBEE:
http://www.adelaida.ro/product_info.php?products_id=11928&osCsid=037c0dd113d36e13790d335451ccfb12

The one I use is closed to this one. I have it both with Xbee. (sd card socket is on the bottom side)

Cheers,

Seb

[Sebastien Lelong]

Hi Vasile, guys,

2011/2/6 vasile surducan <vsur...@gmail.com>

A schottky is protecting the silly user only for reversing the polarity of the power supply, by blowing the fuse if it's reversed.

After some more readings (like http://qsysociety.org/qsywp/2010/12/diy-how-to-use-a-diode-to-provide-reverse-polarity-protection/ or http://highfields-arc.6te.net/constructors/other/revpolepro.htm or http://jeelabs.org/2011/01/09/easy-electrons-%E2%80%93-diodes/), there doesn't seem to be voltage drop when using fuse + diode like you suggested. Diode should be overrated compared to the fuse, so it won't blow before the fuse. In this case, a resettable fuse clearly is a good choice :)

Since there's no voltage drop, why using Schottky diodes (since they're also less resistant) ? What not just "usual" diodes like 1N4001 (or 1N4007) ? 

TIA

Seb

[Sebastien Lelong]

2011/2/6 vasile surducan <vsur...@gmail.com>

On Sat, Feb 5, 2011 at 10:30 AM, Sebastien Lelong <sebastie...@gmail.com> wrote:

So, I understand you're using 2 zener diodes 20V/1A for polarity protection, is that right ? 

you still don't know (after Oliver's message) which is difference between a zener symbol and a schottky simbol and still trying to design board for selling, capitalist economy it's amazing ...fortunately the buyers will don't know either those un-interesting things...

Not that I like nitpicking but...

Shottky diode symbol:

Zener diode symbol, more than one available. Currently used (I guess to avoid confusion with Schottky's):

Previously (still widely) used (but looks like Shottky's, right ?).

To my defense, this *could* explain why I got confused (but there are other reasons, I'm sure), your diodes really look like "Schottner" ones ! :)

Cheers,

Seb

[Oliver Seitz]

>there doesn't seem to be voltage drop when using fuse + diode like you suggested.

That's true, as long as you don't remember that a fuse has a resistance ;-) But it's usually a small drop.

>Diode should be overrated compared to the fuse, so it won't blow before the fuse.

The rating can be in the same magnitude. The schottky I was talking about is rated at 1A, but it has a surge rating of 30A for 8ms. The fuse blows within 1ms at 5A, so no danger at all for the diode.

>In this case, a resettable fuse clearly is a good choice :)

might be, but do remember to have a look at the cold resistances of polyswitch or the like, it can be several ohms.

>Since there's no voltage drop, why using Schottky diodes (since they're also less resistant) ? What not just "usual" diodes like 1N4001 (or 1N4007) ? 

If you're running a strong current through a silicon diode, the voltage drop can reach 1V or a bit more. This voltage reaches the PIC as reverse supply voltage. PICs are only guaranteed to survive 0.3V reverse supply, that's why I was suggesting schottky.

Greets,
Kiste

[funlw65(Vasi)]

Hi Seb,

If you use only 4 pins from the XXBEE, then is good to edit the
footprint and keep only those pins, alog with other 2-3 as board
support (you still have the female socket on the board but with other
pins cut) and remove the others,, making room for traces and maybe
1206 size SMDs.

Vasi

On Feb 7, 2:47 pm, Sebastien Lelong <sebastien.lel...@gmail.com>
wrote:
> 2011/2/6 vasile surducan <vsurdu...@gmail.com>

>  vermeil_IEC_Zener_Diode_Symbol.png
> 2KViewDownload
>
>  250px-Schottky_diode_symbol.svg.png
> 2KViewDownload
>
>  140px-Zener_diode_symbol.svg.png
> < 1KViewDownload

[Sebastien Lelong]

Hi Vasi,

I think I prefer keeping all socket pins, it'll be more solid, and will require less work to adapt. I don't think traces between Xbee scoket holes should be a problem, manufacturer should handle this (eagle checks and reports everything is fine, running seeed rules).

Another point that come to me: the board is 5cm width, and is supposed to be breadboardable. But isn't 5cm width a little too... big for a breadboard ?? 

Cheers,

Seb

2011/2/7 funlw65(Vasi) <fun...@gmail.com>

[funlw65(Vasi)]

Hi Seb,

On Feb 7, 5:26 pm, Sebastien Lelong <sebastien.lel...@gmail.com>
wrote:

> Hi Vasi,
>
> I think I prefer keeping all socket pins, it'll be more solid, and will
> require less work to adapt. I don't think traces between Xbee scoket holes
> should be a problem, manufacturer should handle this (eagle checks and
> reports everything is fine, running seeed rules).

I thought at 44pin TQFP package (I'm playing with that now).

>
> Another point that come to me: the board is 5cm width, and is supposed to be
> breadboardable. But isn't 5cm width a little too... big for a breadboard ??
>

Yes, if you limit yourself at one, long piece of breadboard - I'm
thinking at two independent boards :) (at least).
Also, perfboards with female connectors can be used as testing boards
for your final projects.

> Cheers,
> Seb
>
> 2011/2/7 funlw65(Vasi) <funl...@gmail.com>

[funlw65(Vasi)]

Can be:

1. One of these:
http://www.adelaida.ro/product_info.php?products_id=8870&osCsid=7b37cf93ec215b66779dbdb93d702265
2. Two of these:
http://www.adelaida.ro/product_info.php?products_id=11585&osCsid=7b37cf93ec215b66779dbdb93d702265
3. Two of these:
http://www.adelaida.ro/product_info.php?products_id=8868&osCsid=7b37cf93ec215b66779dbdb93d702265

and so on...
Not to speaking that you can use perfboards/veroboards/stripboards of
any size....

[Sebastien Lelong]

OK, thanks. 

I adjusted pin header so they match 0.1" space for perfboard usage. BTW how do you use such boards, I mean, there's no trace, only holes withpads. So how do you connect components together ? What are the best practices ?

Cheers,

Seb

2011/2/7 funlw65(Vasi) <fun...@gmail.com>

Can be:

1. One of these:
http://www.adelaida.ro/product_info.php?products_id=8870I adjusted pin header so they match 0.1" space. &osCsid=7b37cf93ec215b66779dbdb93d702265
2. Two of these:
http://www.adelaida.ro/product_info.php?products_id=11I adjusted pin header so they match 0.1" space. 585&osCsid=7b37cf93ec215b66779dbdb93d702265

[funlw65(Vasi)]

I think you speak about perfboards.
Connections are made with isolated wires, non-isolated wires along
holes, or simply with a lot of solder... Often you use the terminals
from resistors, capacitors, ... all components you use - speaking
about a final montage.

But guys around here which greater experience can tell you more.
Personally, I prefer stripboards/veroboards.

On Feb 7, 6:55 pm, Sebastien Lelong <sebastien.lel...@gmail.com>
wrote:

> OK, thanks.
>
> I adjusted pin header so they match 0.1" space for perfboard usage. BTW how
> do you use such boards, I mean, there's no trace, only holes withpads. So
> how do you connect components together ? What are the best practices ?
>
> Cheers,
> Seb
>

> 2011/2/7 funlw65(Vasi) <funl...@gmail.com>

>
>
>
> > Can be:
>
> > 1. One of these:

> >http://www.adelaida.ro/product_info.php?products_id=8870Iadjusted pin
> > header so they match 0.1" space. &osCsid=7b37cf93ec215b66779dbdb93d702265<http://www.adelaida.ro/product_info.php?products_id=8870&osCsid=7b37c...>
> > 2. Two of these:
> >http://www.adelaida.ro/product_info.php?products_id=11Iadjusted pin header
> > so they match 0.1" space. 585&osCsid=7b37cf93ec215b66779dbdb93d702265<http://www.adelaida.ro/product_info.php?products_id=11585&osCsid=7b37...>
> > 3. Two of these:
>
> >http://www.adelaida.ro/product_info.php?products_id=8868&osCsid=7b37c...

[funlw65(Vasi)]

Let's say you want a FreeJALduino board to learn microcontrollers but
in your area you have only stripboards/veroboards.
This is how to use them for a custom FreeJALduino board:

http://sites.google.com/site/funlw65/electronics/jaluino-pinguino-28-pins-starting-bo/freejalduino-on-veroboard

Or, even better, if you received a Jaluino as present, you can shield
it
with perboards/stripboards/veroboards in a very short time:

http://sites.google.com/site/funlw65/electronics/jaluino-pinguino-28-pins-starting-bo/freejalduino-stripboard-shields/pin-integrity-test-shield

On Feb 7, 7:03 pm, "funlw65(Vasi)" <funl...@gmail.com> wrote:
> I think you speak about perfboards.
> Connections are made with isolated wires, non-isolated wires along
> holes, or simply with a lot of solder... Often you use the terminals
> from resistors, capacitors, ... all components you use - speaking
> about a final montage.
>
> But guys around here which greater experience can tell you more.
> Personally, I prefer stripboards/veroboards.
>
> On Feb 7, 6:55 pm, Sebastien Lelong <sebastien.lel...@gmail.com>
> wrote:
>
> > OK, thanks.
>
> > I adjusted pin header so they match 0.1" space for perfboard usage. BTW how
> > do you use such boards, I mean, there's no trace, only holes withpads. So
> > how do you connect components together ? What are the best practices ?
>
> > Cheers,
> > Seb
>
> > 2011/2/7 funlw65(Vasi) <funl...@gmail.com>
>
> > > Can be:
>
> > > 1. One of these:
> > >http://www.adelaida.ro/product_info.php?products_id=8870Iadjustedpin
> > > header so they match 0.1" space. &osCsid=7b37cf93ec215b66779dbdb93d702265<http://www.adelaida.ro/product_info.php?products_id=8870&osCsid=7b37c...>
> > > 2. Two of these:

> > >http://www.adelaida.ro/product_info.php?products_id=11Iadjustedpin header

[funlw65(Vasi)]

See this tutorial page for veroboards:
http://www.zen22142.zen.co.uk/Prac/vero_circ/vero.htm

On Feb 7, 7:11 pm, "funlw65(Vasi)" <funl...@gmail.com> wrote:
> Let's say you want a FreeJALduino board to learn microcontrollers but
> in your area you have only stripboards/veroboards.
> This is how to use them for a custom FreeJALduino board:
>

> http://sites.google.com/site/funlw65/electronics/jaluino-pinguino-28-...

>
> Or, even better, if you received a Jaluino as present, you can shield
> it
> with perboards/stripboards/veroboards in a very short time:
>

> http://sites.google.com/site/funlw65/electronics/jaluino-pinguino-28-...

[funlw65(Vasi)]

Ok, last one.

Here is a very nice blog with veroboard projects (mainly Atmel):
http://txapuzas.blogspot.com/

[vasile surducan]

Oh boy, you own me a french wine and a french cheese next time I'll be at Paris (and seems will be soon).

Until the fuse is blowing there is a voltage drop. And that voltage drop may kill everything on your board. That's why you need fast diode turn on and low voltage drop on that diode (which only schottky has) until the fuse blow ( meaning fast fuse blow, which a resettable fuse does not always assure...)

Vasile

TIA

Seb

[funlw65(Vasi)]

Hmmm, Microchip are designing devices thinking with their legs and not
the brains...

It seems to me that you can't use I2C, SPI and RTC same time :
( (thinking at pins used to remap the second SPI)

Here are three workarounds (target: logger applications):
1. using an external RTCC - waste.
2. using HW SPI with a SD card and I2C software - RTC on chip
3. using HW I2C and software SPI with SD card - RTC on chip.

Only the first one it appears to be reliable to me.

I don't know an ATmega with RTC but ATmega644P have 2 USART, 1 SPI, 1
I2C (TWI).. All are separated - have their own pins.

On Feb 6, 6:02 pm, Sebastien Lelong <sebastien.lel...@gmail.com>
wrote:

> 18F27J53 has two MSSP modules. MSSP1 can be used for both I²C and SPI, while
> MSSP2 can only be used for SPI. Since I want i²C, and SPI for embedded
> sd-card, I²C must use RB4 and RB5 pins (pullups for SDA1 and SCL1).
>
> I thus need to use different pins for SPI. MSSP2 has remappable pins (RPn
> pins on datasheets, see screenshot). Interesting feature, I'm supposed to
> select whatever remappable pins needed for SPI... Need more thoughts, but I
> think I'll remap them on RP2, RP11, RP12 and RP13.
>
> Datasheet reading.........
>
> [image: 18f27j53.png]
>
> Cheers,
> Seb
>

> 2011/2/6 Sebastien Lelong <sebastien.lel...@gmail.com>
>
>
>
> > Hi Vasi,
>
> > 2011/2/6 funlw65(Vasi) <funl...@gmail.com>
>

> >> The board will be less general with the two 4k7  resistors on RB1-2...
>
> > Arf... These were supposed to be I²C pull-up resistors, but they aren't
> > connected to the correct pins ! Nice catch, thanks, I'll fix this asap ! If
> > you don't want this feature, just don't solder resistors, that's the idea.
>
> > BTW I tried to move traces and add more spaces as you suggested. I'll post
> > the result soon.
>
> > cheers,
> > Seb
>
> --

[Sebastien Lelong]

2011/2/8 funlw65(Vasi) <fun...@gmail.com>

Hmmm, Microchip are designing devices thinking with their legs and not
the brains...

It seems to me that you can't use I2C, SPI and RTC same time :
( (thinking at pins used to remap the second SPI)

Assuming PIC18F27J53. Why wouldn't it be possible ? I2C on RB4/RB5, SPI remapped on RA5/RC0/RC1/RC2, RTCC on RB1, and still serial on RC6/RC7 (though I have absolutely no idea how RTCC works, nor if SPI can be remapped this way).

Seb

[funlw65(Vasi)]

Hi Seb,

On Feb 8, 8:45 am, Sebastien Lelong <sebastien.lel...@gmail.com>
wrote:
> 2011/2/8 funlw65(Vasi) <funl...@gmail.com>

>
> > Hmmm, Microchip are designing devices thinking with their legs and not
> > the brains...
>
> > It seems to me that you can't use I2C, SPI and RTC same time :
> > ( (thinking at pins used to remap the second SPI)
>

> . ...

> (though I have absolutely no idea how RTCC works, nor if SPI can be remapped
> this way).

The same here. Yes, assuming 18F26J50, 18F27J53. But, RTC needs a
crystal with two capacitors and for this, pins RC0 and RC1 are
occupied (so, I can keep Boot LED on RC2). On 18F46J50 is ok, more
pins so you can have also a HW SPI remapped, but not on 28pin variants
(assuming you want also de internal RTC).

>
> Seb

[vasi vasi]

Hi Seb,

This is how it looks until now using 18F46J50 on 5x5cm board, with all major features. SD Card not yet all pins connected, board is only USB powered (I need to squeeze more space for a jumper), it use a modified footprint of XBEE PRO and I think is already at the limit, using 10 mill traces, 10 mill spaces between.

Entire schematic is just for size test (needs a pro review).

Traces are auto routed, of course...

--
Vasi

[Sebastien Lelong]

According to datasheet, RTC module can also be clocked by the INTRC oscillator.

Again, no practice around this...

2011/2/8 funlw65(Vasi) <fun...@gmail.com>

--
You received this message because you are subscribed to the Google Groups "jallib" group.
To post to this group, send email to jal...@googlegroups.com.
To unsubscribe from this group, send email to jallib+un...@googlegroups.com.
For more options, visit this group at http://groups.google.com/group/jallib?hl=en.

[Sebastien Lelong]

Another Jaluino clone ? *That* is capitalism :)

I thought you wanted to stay from SSOP (or TQFP) package, regarding how hard it is to solder them. I'm not sure to understand the purpose of this design.

Cheers,

Seb

2011/2/8 vasi vasi <fun...@gmail.com>

[funlw65(Vasi)]

I'm not seeing myself doing that board... But, if it must be a logger
(the cheapest one) then let it have all features possible :-) The
mother of all loggers :-)) - Made in China :-D . The 3.3V devices
power! Long live the Mother Russia!

Just kidding (well, in a technical way)

Vasi

On Feb 8, 10:45 am, Sebastien Lelong <sebastien.lel...@gmail.com>
wrote:

> Another Jaluino clone ? *That* is capitalism :)
>
> I thought you wanted to stay from SSOP (or TQFP) package, regarding how hard
> it is to solder them. I'm not sure to understand the purpose of this design.
>
> Cheers,
> Seb
>

> 2011/2/8 vasi vasi <funl...@gmail.com>

[Oliver Seitz]

>According to datasheet, RTC module can also be clocked by the INTRC oscillator.Again, no practice around this...

INTOSC has a typical accuracy of +/- 0.15%, which is about 13 hours per year, while INTRC ranges from 20.3-42,2kHz, this is 31,25 +/- 35%, or more than 8 hours per day. With this inaccuracy, I'd prefer to read the time from a random number generator :-D

32.768kHz watch crystals are small and cheap. If you want to use the RTC, don't economize in the wrong place.

Greets,
Kiste

[funlw65(Vasi)]

So, if we want to use the main features, a 44pin package is a must .. :
(
What said the (guppy) fish? "Damn you, Aquascan!"

[Oliver Seitz]

>Assuming PIC18F27J53. Why wouldn't it be possible ?

I think it will.

32.768kHz crystal on pins 11,12
I2C (MSSP1) on pins 25,26
USART1 on pins 17,18

SPI (MSSP2) and USART2 are freely remappable to the remaining 10 RPx pins.

RTCC is an (optional) output that can give the RTC input frequency, 1 pulse per second or an alarm signal.

Greets,
Kiste

[Sunish Issac]

Microchip may want to sell their dedicated RTCs ;-)

Sunish

[Oliver Seitz]

> It seems to me that you can't use I2C, SPI and RTC same
> time :
> ( (thinking at pins used to remap the second SPI)

Can you explain a bit? Where's the collision?

Greets,
Kiste

[funlw65(Vasi)]

He he, I think the collision is only in my head.
Well, Sebastien wanted to remap the SPI2 pins on pins used by the RTC
clock.and Boot LED...

I considered these:

- RP17, RP18 are occupied by RX1, TX1
- RP4 is RTC out
- RP7, RP8 is I2C1
- RP9, RP10 are part of ICSP connector
- RP11, RP12 are RTC clock
- RP13 is Boot LED (RC2) <-- other boards compatibility.

I also was conditioned by the some rules from my board (and Arduino
pinout "rules"):
- it is nice to have contiguous pins on extension connector for at
least half of a Port. (not shared with I2C, SPI, Serial) - good to use
it on LCD's by example,
- on old 19Fs you have to have some kind of order on ADC pins, because
are dependent of each other (well, not applicable here where ADC pins
are independent)

Also I had/have some unclear things:
- you said RTC Out pulse pin is optional. That mean I can disable it
without loosing RTC feature?
- when you remap pins for SPI2, it needs to be in order (RP1, RP2,
RP3, etc.), or can be selected random?

What ever is selected here on 28pin device, it propagates on the 44pin
one.

Vasi

P.S. Well, pinout compatibility was until now only FreeJALduino and
Pinguino boards care. But it will be nice also for Jaluino family.

[Sebastien Lelong]

So I'll try to include another Xtal, thanks for your input. 10 remappable pins - 4 (SPI2) - 1 (RTCC) - 1 (onboard LED) = 4 remaining pins, 2 of which could be used for RX2/TX2. This would give the following features:

  - 1 serial (RX1/TX1)

  - 1 I²C (SDA1/SCL1), to deal with sensors or the like

  - 1 SPI (remapped, say on 21(RB0), 23(RB2), 27(RB6) and 28(RB7), with microSD slot

  - 1 USB (mini)

  - 1 timer1 clock on 11(RC0) and 12(RC1)

  - 1 onboard LED on 24(RB3)

  - optional Xtal on 9(RA7) and 10(RA6) (intosc can be used to save pins)

  - some remaining pins for ADC, including Vref pins

  - optional serial RX2/TX2, remapped as needed on remaining pins: 2(RA0), 3(RA1), 7(RA5)

I could also remap SPI2 on the same pins as 18F25K22's MSSP2 module (MSSP1 has collision with USB pins) so both could be used (you never know...): RB0/RB1/RB2/RB3. But this kicks out 22(RB1) carrying RTCC output pin... Too bad. Still, RX2/TX2 can be mapped RB/RB7 to match 25K22.I'll think some more about this, it could be interesting, 18F25K22 can run faster and be powered at 5V. There could be a solder jumper selecting either RB1 (for 18F25K22) or RA5 (18F27J53, so RTCC is available), pins are closed from each other, to specify SCK2 pin.

Remappable pins are getting me crazy :)

BTW, does anyone has any experience regarding remappable pins ?...

Cheers,

Seb

2011/2/8 Oliver Seitz <karl...@yahoo.com>

Greets,
Kiste

[Sebastien Lelong]

2011/2/8 funlw65(Vasi) <fun...@gmail.com>

He he, I think the collision is only in my head.
Well, Sebastien wanted to remap the SPI2 pins on pins used by the RTC
clock.and Boot LED...

I considered these:

 - RP17, RP18 are occupied by RX1, TX1
-  RP4 is RTC out
- RP7, RP8 is I2C1
- RP9, RP10 are part of ICSP connector

these pins can still be used for other purpose when not in ICSP, right ?

 

- RP11, RP12 are RTC clock
- RP13 is Boot LED (RC2) <-- other boards compatibility.

There's no compatibility issue here, just use an alias...

 

Also I had/have some unclear things:
- you said RTC Out pulse pin is optional. That mean I can disable it
without loosing RTC feature?

this is what I understand, Kiste may confirm

 

- when you remap pins for SPI2, it needs to be in order (RP1, RP2,
RP3, etc.), or can be selected random?

from what I understand, it can be whatever order you want. There are actually 2 registers per remappable pins, one for input, another four output. You then select what function to associate.

Cheers,

Seb

[funlw65(Vasi)]

I would like to rely on K22 uC series for a VERY nice family of boards
but is not yet widely available. Which can be separate from USB family
boards.
Unfortunately, regarding to USB, Microchip is not consistent (I'm
missing very hard K50 equivalent of 2550/4550).
So, this mix of different uC's are not good for a family of boards
which try to offer some future/backward compatibility :-( (not to say
that a very bad mix is 5V - 3.3V boards - and I'm reffering at
interfacing)

>Remappable pins are getting me crazy :)

I said that to you long time ago :P - a first Cookoo song.

On Feb 8, 6:53 pm, Sebastien Lelong <sebastien.lel...@gmail.com>
wrote:
> 2011/2/8 funlw65(Vasi) <funl...@gmail.com>

>
> > He he, I think the collision is only in my head.
> > Well, Sebastien wanted to remap the SPI2 pins on pins used by the RTC
> > clock.and Boot LED...
>
> > I considered these:
>
> >  - RP17, RP18 are occupied by RX1, TX1
> > -  RP4 is RTC out
> > - RP7, RP8 is I2C1
> > - RP9, RP10 are part of ICSP connector
>
> these pins can still be used for other purpose when not in ICSP, right ?

Yes but with some care. On a final project where destination is not
changed, yes.

>
> > - RP11, RP12 are RTC clock
> > - RP13 is Boot LED (RC2) <-- other boards compatibility.
>
> There's no compatibility issue here, just use an alias...
>

Yes, a virtual layer is always a solution but I wanted also to be HW
compatibility (at least, this is the first thing I'm trying to solve,
where is possible).

[Oliver Seitz]

>- RP9, RP10 are part of ICSP connector
>these pins can still be used for other purpose when not in ICSP, right ? 

You can use them for ICSP *and* for something else, you just have to make sure no electrical collision can occur. You can e.g. use them as general purpose I/O on a shield board. You just have to take off that board when reprogramming via ICSP.

>- you said RTC Out pulse pin is optional. That mean I can disable it without loosing RTC feature?

Yes. I really can hardly see any use of that function at all. You can make the ":" on a clock display blink. Great.

 
>>- when you remap pins for SPI2, it needs to be in order (RP1, RP2, RP3, etc.), or can be selected random?

>from what I understand, it can be whatever order you want. There are actually 2 registers per remappable pins, one for input, another four output. You then select what function to associate.

Right. Almost right. It's a bit more complicated, but in a sensible way.

For pins used as outputs, you set the *pin* to the *peripheral*.
For pins used as inputs, you set the *peripheral* to the *pin*.

This makes it possible for a peripheral to drive several output pins simultaneously. And it makes it possible for a pin to serve as input to several peripherals. It even makes it possible to connect one peripheral's output to another one's (or even its own) input with only using one pin.

Greets,
Kiste

[funlw65(Vasi)]

BTW, where to put the final configuration? In USB bootloader? In a
layer library?

[vasi vasi]

Corrected an error, better (aesthetic) arrangement of components, SD Card socket only partially connected (VCC + GND) - waiting for jury. Also, the VCC pin from ICSP socket not yet connected.

All I/O pins are connected to extension socket (exceptions are: VDDCORE, VUSB, and the main oscillator pins).

Board is powered externally only via USB, yet (it needs just a connector for other external sources).... Internal 3.3VCC is available also on extension connector.

Anyway, as is now, it is a good start for everyone to start adding/removing components and features.

--
Vasi

[vasile surducan]

Vasi,

still too big PCB, distance between crystal and micro also too big, I can't see any filtering cap near xbee (which is must, else the RF spectrum will stinks),I was lazy to see how much copper did you allowed for LDO heatsink...

However I like your design, maybe you are interested in a secondary job in pcb design?

Vasile

--

[Sebastien Lelong]

2011/2/8 funlw65(Vasi) <fun...@gmail.com>

>Remappable pins are getting me crazy :)

I said that to you long time ago :P - a first Cookoo song.

Sure, but I'm not talking about pin mapping (which was quite usable in the end with cuckoo), but about remappable pins, which brings pin mapping next level (thus, crazy next-level too :))

Cheers,

Seb

[funlw65(Vasi)]

Hi,

On Feb 9, 7:14 am, vasile surducan <vsurdu...@gmail.com> wrote:
> Vasi,
>
> still too big PCB, distance between crystal and micro also too big, I can't
> see any filtering cap near xbee (which is must, else the RF spectrum will
> stinks),I was lazy to see how much copper did you allowed for LDO
> heatsink...
>

I will make a decision regarding to SPI2 pins and solve the other
issues.

> However I like your design, maybe you are interested in a secondary job in
> pcb design?
>

Thank you, but you know, I started on Sebastien's base design! I don't
know who will want to work with someone which designed only few
boards, it has poor knowledge and lack of experience...
I don't know if I am good for this job, but I like to design. Anyway,
I'm very slow ....

Vasi

> Vasile

[vasile surducan]

On Wed, Feb 9, 2011 at 11:26 PM, funlw65(Vasi) <fun...@gmail.com> wrote:

Hi,

On Feb 9, 7:14 am, vasile surducan <vsurdu...@gmail.com> wrote:
> Vasi,
>
> still too big PCB, distance between crystal and micro also too big, I can't
> see any filtering cap near xbee (which is must, else the RF spectrum will
> stinks),I was lazy to see how much copper did you allowed for LDO
> heatsink...
>

I will make a decision regarding to SPI2 pins and solve the other
issues.

> However I like your design, maybe you are interested in a secondary job in
> pcb design?
>

Thank you, but you know, I started on Sebastien's base design! I don't
know who will want to work with someone which designed only few
boards, it has poor knowledge and lack of experience...

Ok, then. I'm not interested in such things of toys, but is a good starting point for learning.

Mostly this one, which has a small part of RF, which btw was treated so far as DC.

Even the 20MHz part of this design is understand by most people from this list as DC, so when I'm saying there is huge distance between the crystal to the PIC I'm not talking just to free off some used air from my mouth.

A 20MHz square wave generated by the crystal oscillator has powerful odd harmonics up to the 13'th, meaning from 20MHz above 2GHz.

The zigbee PLL synteziser has a local oscillator which may interfere with the micro clock and it's harmonics. As higher the harmonics as bad. The result can be a PLL unlock from time to time, which is translated (for people which doesn't have a spectrum analyzer) in data lost in unexpected way. 

Vasile

[Oliver Seitz]

May I apply for the job? ;-)

But I should warn you: I do not use those automatic via generators that some people call autorouters.

> which btw was treated so far as DC.

I do know what "short traces" means, and I usually think of DC when it's below 1MHz...

>A 20MHz square wave

Well, it's a crystal, not an oscillator, right? So it is not supposed to be square. And even if it was an oscillator, many people would be surprised when connecting a scope, how "round" a "square" can be...

Greets,
Kiste

[vasi vasi]

Last variant - it may be worse.


--
Vasi

[vasile surducan]

On Thu, Feb 10, 2011 at 9:59 AM, Oliver Seitz <karl...@yahoo.com> wrote:

May I apply for the job? ;-)

  No, because I can't pay you at your standards. 

 

But I should warn you: I do not use those automatic via generators that some people call autorouters.

> which btw was treated so far as DC.

I do know what "short traces" means, and I usually think of DC when it's below 1MHz...

I didn't read your post, sorry, here seems to be a new email. 

>A 20MHz square wave

Well, it's a crystal, not an oscillator, right? So it is not supposed to be square. And even if it was an oscillator, many people would be surprised when connecting a scope, how "round" a "square" can be...

Yes, is round, but the oscillator output (inside the micro) is square, and the spectrum is exactly in my story...

Vasile

 

Greets,
Kiste

[vasile surducan]

On Thu, Feb 10, 2011 at 12:04 PM, vasile surducan <vsur...@gmail.com> wrote:

On Thu, Feb 10, 2011 at 9:59 AM, Oliver Seitz <karl...@yahoo.com> wrote:

May I apply for the job? ;-)

  No, because I can't pay you at your standards. 

 

But I should warn you: I do not use those automatic via generators that some people call autorouters.

One more  idea: you can't afford to not use the autorouter when you deal with 12 layers or so and have more than 5000 joints...

[Oliver Seitz]

>>May I apply for the job? ;-)
>No, because I can't pay you at your standards.  

I would give you a discount ;-)

>One more idea: you can't afford to not use the autorouter when you deal with 12 layers or so and have more than 5000 joints...

Ok, that's right, but I haven't had such boards yet. But sometimes I did single-layer boards when people thought double-layer would be the minimum.

>I didn't read your post, sorry, here seems to be a new email. 

I haven't wrote anything about RF yet, I just wanted to emphasize your point that anything above 1MHz is (at least can be) something to take special care of.

>>>A 20MHz square wave
>>Well, it's a crystal, not an oscillator, right? So it is not supposed to be square. And even if it was an oscillator, many people would be surprised when connecting a scope, how "round" a "square" can be...

>Yes, is round, but the oscillator output (inside the micro) is square, and the spectrum is exactly in my story...

Inside the micro there's even a 64MHz clock, no? But if supply is properly bypassed, I think we can just care about external signals. For example, the USB D+ and D- lines, that can carry 12MHz at more than 3V amplitude shouldn't be automatically routed. In Vasi's design, those lines contain forks, and are not routet in parallel next to each other. That's something I would mark for review. I would also try to avoid mapping those lines to a USB socket *and* a pin header.

Greets,
Kiste

[vasile surducan]

On Thu, Feb 10, 2011 at 12:49 PM, Oliver Seitz <karl...@yahoo.com> wrote:

>>May I apply for the job? ;-)
>No, because I can't pay you at your standards.  

I would give you a discount ;-)

>One more  idea: you can't afford to not use the autorouter when you deal with 12 layers or so and have more than 5000 joints...

Ok, that's right, but I haven't had such boards yet. But sometimes I did single-layer boards when people thought double-layer would be the minimum.

>I didn't read your post, sorry, here seems to be a new email. 

I haven't wrote anything about RF yet, I just wanted to emphasize your point that anything above 1MHz is (at least can be) something to take special care of.

>>>A 20MHz square wave
>>Well, it's a crystal, not an oscillator, right? So it is not supposed to be square. And even if it was an oscillator, many people would be surprised when connecting a scope, how "round" a "square" can be...

>Yes, is round, but the oscillator output (inside the micro) is square, and the spectrum is exactly in my story...

Inside the micro there's even a 64MHz clock, no? But if supply is properly bypassed, I think we can just care about external signals. For example, the USB D+ and D- lines, that can carry 12MHz at more than 3V amplitude shouldn't be automatically routed.

Agree. However that depends on CAD. Eagle can't, but other can. For example what if you have to route 30 pairs carrying 3Gbps?

I've did it manually once...

 

In Vasi's design, those lines contain forks, and are not routet in parallel next to each other. That's something I would mark for review. I would also try to avoid mapping those lines to a USB socket *and* a pin header.

  That's other problem, USB should have around 120 ohm impedance and must be routed as a pair, I'm telling that at all designs which appear here... I would never route crystals and fast communication buses through pin headers, jumpers, and all the rest.

But you know, I know that you know so why wasting words?

BTW one women is using between 5000 to 18000 words per day. How many words have waste all mens talking on this subject? More than 5 standard womens?