ATX breakout board v2 in KiCad

Hardware incubation. See also our in development projects wiki.

ATX breakout board v2 in KiCad

Postby ian » Wed Sep 12, 2012 8:19 am

ATX_PSU.v2-brd-KiCAD_front_20120911.png


Over the last week we re-visioned the ATX power supply breakout board in KiCAD, free of the confines of Eagle's 100mm by 80mm cell. We chose the ATX board because it's already at the limit, and it's fill of big connectors that can't be miniaturized.

This version builds on the already popular ATX Breakout Board v1.1, but adds new features and hackability. Stuff that simply wouldn't be possible without the unlimited routing area available from the open source alternative to our usual program.

Features of the ATX Breakout Board V2:

Adjustable positive and negative power rails
Fuse blown indicators on every rail, complementing the line good LEDs
Ground terminals on every line
1.25A polyfuses on all power lines, including the adjustable ones
2nd ATX jack for easier enclosure design
2x8 0.1'' header connected to all the power and control lines of the PSU, including the adjustable ones.
Open source, designed in KiCAD open source software

We'll post a complete update tomorrow on the blog. Love it? Hate it? Give me your wost :)

ATX_PSU.v2-sch-KiCAD_201209010a.png
Attachments
ATX_PSU.v2_KiCAD_gerber_20120911.zip
(357.76 KiB) Downloaded 459 times
ATX_PSU.v2_KiCAD_20120911.zip
(295.47 KiB) Downloaded 490 times
User avatar
ian
Crew
Crew
 
Posts: 10803
Joined: Mon Jul 06, 2009 6:14 am

Re: ATX breakout board v2 in KiCad

Postby Tarloth » Wed Sep 12, 2012 8:33 am

Ian:

THANKS! This is a useful board and it keep simple, THANKS
Tarloth
Full Member
Full Member
 
Posts: 118
Joined: Thu Oct 06, 2011 10:54 am

Re: ATX breakout board v2 in KiCad

Postby arhi » Wed Sep 12, 2012 9:05 am

Now this is a proper useful ATX PSU board!
Perfect :)
User avatar
arhi
Hero Member
Hero Member
 
Posts: 2160
Joined: Thu Jun 24, 2010 11:41 am
Location: Belgrade, Serbia

Re: ATX breakout board v2 in KiCad

Postby TitanMKD » Wed Sep 12, 2012 1:01 pm

Yes now this ATX Breakout board is really useful I was waiting adjustable power !!
If there's any spare PCB i'm ready to buy one (with a box ;)
Best Regards
Benjamin
TitanMKD
Full Member
Full Member
 
Posts: 118
Joined: Tue May 11, 2010 5:11 pm
Location: France

Re: ATX breakout board v2 in KiCad

Postby brian » Wed Sep 12, 2012 1:55 pm

I hope your KiCAD experience is going well, Ian. :-)
brian
Sr. Member
Sr. Member
 
Posts: 495
Joined: Sun Nov 14, 2010 12:27 am

Re: ATX breakout board v2 in KiCad

Postby bearmos » Wed Sep 12, 2012 2:30 pm

The new breakout board looks good!

Since it's getting larger, you might consider adding a few extra sets of stand-off holes in the middle to combat flex when banana plugs are pushed in (or pulled out).

You may also consider providing a generous copper pour on the tab of each regulator to help with heat dissipation - possibly include some thermal vias to the secondary layer and mirror the pour there as well. These regulators will get pretty toasty if they're providing a fair amount of current at a low voltage (not too much of a concern since they're thermally protected).

I'm also curious how your KiCAD experience was :) - I'll be sure to catch the recap on the blog.
bearmos
Hero Member
Hero Member
 
Posts: 748
Joined: Tue Nov 02, 2010 10:02 pm

Re: ATX breakout board v2 in KiCad

Postby beth » Wed Sep 12, 2012 3:32 pm

It looks really nice, a fantastic step forward for the ATX breakout board, different but nice.

I mean, I think that eagle has been in our life for a long long time, eight years in my case and I think that we are used to it, to its interface and with his weaknesses and strengths. Sometimes it's irritating, others is amazing, but for me the worst is its board size limitation if you want to stay with the free version (and not go for a pirate option with its associated problems).

I was reluctant with KiCad, however seeing your schematic, the result and option of converting libraries from eagle to KiCad maybe it deserves a try, so I think that it worths.

All the best, beth.
beth
Newbie
Newbie
 
Posts: 18
Joined: Wed Feb 03, 2010 2:21 pm

Re: ATX breakout board v2 in KiCad

Postby LongHairedHacker » Wed Sep 12, 2012 3:54 pm

Moin

First of all nice work with the board and it's also cool to finally see you trying kicad.

TitanMKD has just discovered a minor 'bug' in the Kicad Part library from http://dangerous-prototypes-open-hardwa ... rt_Library .

When loading the eeschema lib in stable we both got a bunch of errors starting with :
Code: Select all
<undefined DRAW command #> occured at line 9368


When I tried with testing I got :
Code: Select all
Library <dp_devices> component load error error <field 1 does not have the correct number of parameters> occurred at line 131


After some cross debugging via IRC using the stable (BZR rev. 3256) and the latest unstable (BZR rev. 3718) versions of kicad I could narrow the problems down to 2 things :

First Problem:
Some versions of kicad don't like #-line comments between then DRAW and the ENDDRAW command.
For example this snippet (line 9348 to 9425) in the original dp_devices.lib :
Code: Select all
#
# Dev Name: RESISTOR_ARRAY_8
# Package Name: CAT16-F8/CAT16-J8
# Dev Tech: ''
# Dev Prefix: RN
# Gate count = 8
#
DEF RESISTOR_ARRAY_8 RN 0 40 N N 8 L N
# Gate Name: A
# Symbol Name: RESISTOR
F0 "RN" -150 59 50 H V L B
F1 "RESISTOR_ARRAY_8" -150 -130 50 H V L B
F2 "dp_devices-CAT16-F8/CAT16-J8" 0 150 50 H I C C
DRAW
P 2 1 0 0 -100 -35 100 -35
P 2 1 0 0 100 35 -100 35
P 2 1 0 0 100 -35 100 35
P 2 1 0 0 -100 -35 -100 35
X 1 1 -200 0 100 R 40 40 1 1 P
X 2 16 200 0 100 L 40 40 1 1 P
# Gate Name: B
# Symbol Name: RESISTOR
P 2 2 0 0 -100 -35 100 -35
P 2 2 0 0 100 35 -100 35
P 2 2 0 0 100 -35 100 35
P 2 2 0 0 -100 -35 -100 35
X 1 2 -200 0 100 R 40 40 2 1 P
X 2 15 200 0 100 L 40 40 2 1 P
# Gate Name: C
# Symbol Name: RESISTOR
P 2 3 0 0 -100 -35 100 -35
P 2 3 0 0 100 35 -100 35
P 2 3 0 0 100 -35 100 35
P 2 3 0 0 -100 -35 -100 35
X 1 3 -200 0 100 R 40 40 3 1 P
X 2 14 200 0 100 L 40 40 3 1 P
# Gate Name: D
# Symbol Name: RESISTOR
P 2 4 0 0 -100 -35 100 -35
P 2 4 0 0 100 35 -100 35
P 2 4 0 0 100 -35 100 35
P 2 4 0 0 -100 -35 -100 35
X 1 4 -200 0 100 R 40 40 4 1 P
X 2 13 200 0 100 L 40 40 4 1 P
# Gate Name: E
# Symbol Name: RESISTOR
P 2 5 0 0 -100 -35 100 -35
P 2 5 0 0 100 35 -100 35
P 2 5 0 0 100 -35 100 35
P 2 5 0 0 -100 -35 -100 35
X 1 5 -200 0 100 R 40 40 5 1 P
X 2 12 200 0 100 L 40 40 5 1 P
# Gate Name: F
# Symbol Name: RESISTOR
P 2 6 0 0 -100 -35 100 -35
P 2 6 0 0 100 35 -100 35
P 2 6 0 0 100 -35 100 35
P 2 6 0 0 -100 -35 -100 35
X 1 6 -200 0 100 R 40 40 6 1 P
X 2 11 200 0 100 L 40 40 6 1 P
# Gate Name: G
# Symbol Name: RESISTOR
P 2 7 0 0 -100 -35 100 -35
P 2 7 0 0 100 35 -100 35
P 2 7 0 0 100 -35 100 35
P 2 7 0 0 -100 -35 -100 35
X 1 7 -200 0 100 R 40 40 7 1 P
X 2 10 200 0 100 L 40 40 7 1 P
# Gate Name: H
# Symbol Name: RESISTOR
P 2 8 0 0 -100 -35 100 -35
P 2 8 0 0 100 35 -100 35
P 2 8 0 0 100 -35 100 35
P 2 8 0 0 -100 -35 -100 35
X 1 8 -200 0 100 R 40 40 8 1 P
X 2 9 200 0 100 L 40 40 8 1 P
ENDDRAW
ENDDEF


Should actually look like this :
Code: Select all
#
# Dev Name: RESISTOR_ARRAY_8
# Package Name: CAT16-F8/CAT16-J8
# Dev Tech: ''
# Dev Prefix: RN
# Gate count = 8
#
DEF RESISTOR_ARRAY_8 RN 0 40 N N 8 L N
# Gate Name: A
# Symbol Name: RESISTOR
F0 "RN" -150 59 50 H V L B
F1 "RESISTOR_ARRAY_8" -150 -130 50 H V L B
F2 "dp_devices-CAT16-F8/CAT16-J8" 0 150 50 H I C C
DRAW
P 2 1 0 0 -100 -35 100 -35
P 2 1 0 0 100 35 -100 35
P 2 1 0 0 100 -35 100 35
P 2 1 0 0 -100 -35 -100 35
X 1 1 -200 0 100 R 40 40 1 1 P
X 2 16 200 0 100 L 40 40 1 1 P
P 2 2 0 0 -100 -35 100 -35
P 2 2 0 0 100 35 -100 35
P 2 2 0 0 100 -35 100 35
P 2 2 0 0 -100 -35 -100 35
X 1 2 -200 0 100 R 40 40 2 1 P
X 2 15 200 0 100 L 40 40 2 1 P
P 2 3 0 0 -100 -35 100 -35
P 2 3 0 0 100 35 -100 35
P 2 3 0 0 100 -35 100 35
P 2 3 0 0 -100 -35 -100 35
X 1 3 -200 0 100 R 40 40 3 1 P
X 2 14 200 0 100 L 40 40 3 1 P
P 2 4 0 0 -100 -35 100 -35
P 2 4 0 0 100 35 -100 35
P 2 4 0 0 100 -35 100 35
P 2 4 0 0 -100 -35 -100 35
X 1 4 -200 0 100 R 40 40 4 1 P
X 2 13 200 0 100 L 40 40 4 1 P
P 2 5 0 0 -100 -35 100 -35
P 2 5 0 0 100 35 -100 35
P 2 5 0 0 100 -35 100 35
P 2 5 0 0 -100 -35 -100 35
X 1 5 -200 0 100 R 40 40 5 1 P
X 2 12 200 0 100 L 40 40 5 1 P
P 2 6 0 0 -100 -35 100 -35
P 2 6 0 0 100 35 -100 35
P 2 6 0 0 100 -35 100 35
P 2 6 0 0 -100 -35 -100 35
X 1 6 -200 0 100 R 40 40 6 1 P
X 2 11 200 0 100 L 40 40 6 1 P
P 2 7 0 0 -100 -35 100 -35
P 2 7 0 0 100 35 -100 35
P 2 7 0 0 100 -35 100 35
P 2 7 0 0 -100 -35 -100 35
X 1 7 -200 0 100 R 40 40 7 1 P
X 2 10 200 0 100 L 40 40 7 1 P
P 2 8 0 0 -100 -35 100 -35
P 2 8 0 0 100 35 -100 35
P 2 8 0 0 100 -35 100 35
P 2 8 0 0 -100 -35 -100 35
X 1 8 -200 0 100 R 40 40 8 1 P
X 2 9 200 0 100 L 40 40 8 1 P
ENDDRAW
ENDDEF


After a quick sed -i '/^#/d' dp_devices.lib it worked fine in the stable version (3625), but had other errors in testing.

Second Problem:
Since testing was still complaining about line 131 (which became now line 75 due to deleting comments), I took a closer look at the parameters.
The F1 call is supposed to have 8 parameters as far I can tell from editing kicadlibs in vim.
Code: Select all
F1 "CAPACITOR_NPOL-PTH_0.1"" 100 100 50 H V L B

It has 8 parameters here as well, but there is a double "" at the end of the string, leading the parser to think that there were only 2 strings given.
Modifying the line to :
Code: Select all
F1 "CAPACITOR_NPOL-PTH_0.1" 100 100 50 H V L B

Did solve this.
I'm not sure whether it is possible to escape " characters there, so the best is possibly to use a double ' instead.

I've uploaded the version with both problems fixed here : http://www.sebastians-site.de/homepage/ ... evices.lib

It's a nice library and I'm looking forward to use it (especially the SOB pcb outlines).

Sebastian
DIY-electronics ... eating all my money and free time since 1998
User avatar
LongHairedHacker
Newbie
Newbie
 
Posts: 49
Joined: Fri Jun 24, 2011 7:19 am

Re: ATX breakout board v2 in KiCad

Postby touch » Tue Sep 18, 2012 8:02 pm

Looks great, any idea when it will be available?
touch
Newbie
Newbie
 
Posts: 31
Joined: Wed Feb 15, 2012 10:50 pm

Re: ATX breakout board v2 in KiCad

Postby ian » Fri Sep 21, 2012 10:01 am

THanks Sebastian, we're looking into it.
User avatar
ian
Crew
Crew
 
Posts: 10803
Joined: Mon Jul 06, 2009 6:14 am

Re: ATX breakout board v2 in KiCad

Postby vimark » Fri Sep 21, 2012 10:25 am

@LongHairedHacker

Kindly update your kicad libraries to rev 2005, these were created using eagle2kicad-0.9d.ulp and those errors were fixed. The first commit was made using 0.9b ULP

Digging on 1st error:

I've investigated the first error that involve a '#' comment in between DRAW and ENDDRAW, these error occurs on converted devices containing multiple symbols in one device. e.g. those chips having separate supply pins (In eagle, you use 'invoke' command to get the supply pins). Another one, those array resistors containing 4 or 8 resistors in one device, in which you use invoke to use the other elements. same for those 4 in 1 and 2 in 1 package op-amps. The ULP seems having difficulty converting these devices and repeatedly creating script on the same element composing that device.
vimark
Crew
Crew
 
Posts: 1297
Joined: Fri Feb 12, 2010 3:23 am
Location: Davao City, Philippines

Re: ATX breakout board v2 in KiCad

Postby kenyee » Wed Jan 02, 2013 9:50 am

Looks like you still have lots of space (can't see the back) to add these two suggestions:
viewtopic.php?f=50&t=4963
and from http://dangerousprototypes.com/2012/06/ ... ments-wrap arhi's comment:
"ATX supply is extremely dirty with incredibly high ripple. If you already made a PCB to get the 3,+-5,-+5 and +-12V (wait, where’s -5 ?!) out why didn’t you add some capacitance on each rail? some combo of 2x10nF + 100nF + 1uF ceramic + 10uF ceramic on each rail would improve things significantly, and adding a LC filter to 5V and 3V3 rails would be additional bonus. On top of this, at least 2 more output should exist, one 9V 1A (simple 7809 would suffice) + one VAR voltage 1-2A (317 or something similar) With regards to 5V load, I found that using a resistor is really too much of a waste of energy so I power a light from 5V. It provides proper load + can be used as backlight for a PSU case. A regular car headlight lamp can be used. It will not be as bright and hot as when it’s running at 12V (nor you want it that bright/hot), it will be cooler then the 10W resistor and will be a super useful add-on."

For the rest of the layout, I'd suggest moving the VAdj+- connectors up and into the middle of the board to cut the width of it down...looks like there might be enough space to do this too.
But definitely *LOTS* better than the ATX V1.x layouts. Get a nice SoB case for this and it'll be a best seller :-)
kenyee
Newbie
Newbie
 
Posts: 48
Joined: Tue May 22, 2012 9:26 am

voltage adjustment range?

Postby kenyee » Fri Feb 01, 2013 2:50 pm

Any idea how far the voltage can be adjusted?

It'd be useful if it went to 15V to simulate a 12V battery being charged by a solar panel...
kenyee
Newbie
Newbie
 
Posts: 48
Joined: Tue May 22, 2012 9:26 am


Return to Project development, ideas, and suggestions