Searching \ for '[PIC]entering picsquirt into design contest' in subject line. ()
Make payments with PayPal - it's fast, free and secure! Help us get a faster server
FAQ page: www.piclist.com/techref/microchip/devices.htm?key=pic
Search entire site for: 'entering picsquirt into design contest'.

Exact match. Not showing close matches.
PICList Thread
'[PIC]entering picsquirt into design contest'
2006\09\08@160659 by peter green

flavicon
face
some time ago (a few weeks iirc, not sure exactly how long) i mentioned that
i would like to enter my picsquirt (
http://www.p10link.net/plugwash/picsquirt/ ) into the piclist design
contest.

i was in uni today sorting out other things (i can only work on the PCB
design on the departments computers and its the summer holidays atm) and
have tried to export a set of gerbers and a drill file. I have posted them
at http://www.p10link.net/plugwash/picsquirt/picsquirt_gerbers.zip  can
someone take a look at them and tell me if they seem suitable?


2006\09\08@174424 by James Newton, Host

face picon face
I've put it up at
http://www.piclist.com/images/boards/picsquirt/index.htm

The gerbers look ok at first glance, but I couldn't read the drill file.
What format is that? Maybe Olimex will have better luck, they certainly know
more about that stuff than I do. Please note, Olimex does not compensate for
plate through so your hole sizes need to be just a touch bigger than the
lead sizes.

Is there anywhere people can get a pre-programmed 18F2550 for it?

Any description of what all the stuff in the software archive does? Mouse?
TargetProg? TargetProgPortB?

Documentation for the use of the PC software?

Lots of questions, sorry, no good deed goes unpunished and this looks like a
good deed indeed.

Thanks!

---
James Newton: PICList webmaster/Admin
spam_OUTjamesnewtonTakeThisOuTspampiclist.com  1-619-652-0593 phone
http://www.piclist.com/member/JMN-EFP-786
PIC/PICList FAQ: http://www.piclist.com





> {Original Message removed}

2006\09\08@175904 by Brent Brown

picon face
On 8 Sep 2006 at 21:06, peter green wrote:
> some time ago (a few weeks iirc, not sure exactly how long) i
> mentioned that i would like to enter my picsquirt (
> http://www.p10link.net/plugwash/picsquirt/ ) into the piclist design
> contest.
>
> i was in uni today sorting out other things (i can only work on the
> PCB design on the departments computers and its the summer holidays
> atm) and have tried to export a set of gerbers and a drill file. I
> have posted them at
> http://www.p10link.net/plugwash/picsquirt/picsquirt_gerbers.zip  can
> someone take a look at them and tell me if they seem suitable?

Hi Peter,

Just a few comments on how you might make the PCB look nicer more than
anything else, hope you don't mind a little critiquing...
- Add a top overlay (if cost permits).
- Make all tracks straight or 45 degrees.
- Avoid internal angles of less than 90 degrees, eg. look at track junction near top
right corner on bottom layer. These places allow etchant to be trapped and you can
get over-etching (and it looks bad). Even 90 deg corners look nicer when a small
fillet of 45 deg is added.
- Try to make tracks exit pads from the end of the pad, looks nicer
- Pad sizes are well sized, but 0.010" tracks are a little on the fine side, looks like
you could handle 0.012" or 0.015" no problems. Only too fine if anyone is going to
make the boards at home.
- Hole sizes: You have 9 different sizes where 3 or 4 should be sufficient.
- In a few places you have tracks running past the end of the pad.
- "Necking down" from one track size to another looks bad when done on a corner,
try and do it on a straight section of track.
- I also couldn't read the drill file but I didn't persist with it.

Lot's of personal prefference in the above, so ignore where necessary! Nice project,
good work.

--
Brent Brown, Electronic Design Solutions
16 English Street, St Andrews,
Hamilton 3200, New Zealand
Ph: +64 7 849 0069
Fax: +64 7 849 0071
Cell: 027 433 4069
eMail:  .....brent.brownKILLspamspam@spam@clear.net.nz


2006\09\08@194900 by peter green

flavicon
face

> I've put it up at
> www.piclist.com/images/boards/picsquirt/index.htm
:) i see you have converted my gerbers to images too.

>
> The gerbers look ok at first glance, but I couldn't read the drill file.
> What format is that? Maybe Olimex will have better luck, they
> certainly know
> more about that stuff than I do. Please note, Olimex does not
> compensate for
> plate through so your hole sizes need to be just a touch bigger than the
> lead sizes.
I'll talk to the uni PCB facility where previous boards have been fabricated
to see what they do in this regard. as for the drill file format i just used
the default export options in altium.

>
> Is there anywhere people can get a pre-programmed 18F2550 for it?
are you asking for yourself or for making this design public? i could
possiblly supply one but i don't wan't to get into anything large scale.

>
> Any description of what all the stuff in the software archive does? Mouse?
> TargetProg? TargetProgPortB?
the dirs you need are firmware ,USB driver and PC, firmware is the firmware
for the programmer,PC is the PC side software, USB driver is the microchip
USB driver.

the targetprog and targetprogportB dirs are programs i wrote into target
chips to check i could program them.

mouse is an adaptation of the mouse in a circle demo to the picsquirts
hardware (and running without a bootloader) used for early testing.

>
> Documentation for the use of the PC software?
must get arround to writing that, but basically you just pass it a hex file
on the command line.

>
> Lots of questions, sorry, no good deed goes unpunished and this
> looks like a
> good deed indeed.
:)

2006\09\08@200026 by peter green

flavicon
face

> - Add a top overlay (if cost permits).
theres a top overlay in the design but its such a mess i thought the board
would look better without it (you can see it on the layout pdf on my site)
so i didn't bother putting it in that gerber set.

> - Make all tracks straight or 45 degrees.
yeah i got a bit lazy on this, maybe i'll change it if i can be bothered

> - Avoid internal angles of less than 90 degrees, eg. look at
> track junction near top
> right corner on bottom layer.
that looks just slightly less than 90 degrees, still noted

> These places allow etchant to be
> trapped and you can
> get over-etching (and it looks bad). Even 90 deg corners look
> nicer when a small
> fillet of 45 deg is added.
mmm can't say i've had any problems with any revs so far (the gerbers i've
sent are for a rev that hasn't been produced yet but the main changes are
increased pad sizes)

> - Try to make tracks exit pads from the end of the pad, looks nicer
noted

> - Pad sizes are well sized, but 0.010" tracks are a little on the
> fine side, looks like
> you could handle 0.012" or 0.015" no problems.
i just typed in the figure that the uni PCB guys gave me as min reccomended
and haven't got arround to increasing it.

>Only too fine if
> anyone is going to
> make the boards at home.
you'd be subjecting yourself to extreme pain if you tried to make this
without PTH anyway. A diy suitable layout would mean different priorities (i
wanted this pretty much as small as was feasible with through hole
components).

> - Hole sizes: You have 9 different sizes where 3 or 4 should be
> sufficient.
yeah, as my first PCB project i intially used standard lands from the
library and those i later replaced i based on ones from there. this could
probablly be changed if i can be bothered.

> - In a few places you have tracks running past the end of the pad.
yeah, mostly those tiny caps (which are actually a rules violation too but
they seem to fab ok on the uni process and worst case is you'd have to run a
knife down them) where i tried to keep the track as far away from the other
land as possible.

> - "Necking down" from one track size to another looks bad when
> done on a corner,
noted but not a big issue


More... (looser matching)
- Last day of these posts
- In 2006 , 2007 only
- Today
- New search...