Cadence PSD Layout Plus (OrCAD) and Drill Files

I have always used OrCAD (now known as Cadence) to design my boards and I’m pretty used to it, so I’d like to use it with Sparkfun, but I’ve been browsing some of the DRD files users post here and mine look a lot different. I select Extended Gerber and 2.3 format in Layout Plus:

http://img221.echo.cx/img221/5484/g239uo.gif

http://img40.echo.cx/img40/5403/gext7va.gifç

And my .drd file looks like:

*
G04 Mass Parameters ***
*
G04 Image ***
*
%INC:\DOCUMENTS AND SETTINGS\DORAGASU\ESCRITORIO\ANALOG\PCB\ANALOG.DRD*%
%ICAS*%
%MOIN*%
%IPPOS*%
%ASAXBY*%
G74*%FSLAN2X23Y23*%
*
G04 Aperture Definitions ***
*
%AMTHERMAL210*
1,1,0.0689,0,0,*
1,0,0.0530,0,0,*
21,0,0.0690,0.0100,0,0,135.0*
21,0,0.0690,0.0100,0,0,225.0*%
%AMTHERMAL217*
1,1,0.0739,0,0,*
1,0,0.0580,0,0,*
21,0,0.0740,0.0100,0,0,225.0*
21,0,0.0740,0.0100,0,0,315.0*%
%AMTHERMAL221*
1,1,0.0529,0,0,*
1,0,0.0370,0,0,*
21,0,0.0530,0.0100,0,0,225.0*
21,0,0.0530,0.0100,0,0,315.0*%
%AMTHERMAL227*
1,1,0.0679,0,0,*
1,0,0.0520,0,0,*
21,0,0.0680,0.0100,0,0,45.0*
21,0,0.0680,0.0100,0,0,135.0*%
%AMTHERMAL235*
1,1,0.0399,0,0,*
1,0,0.0240,0,0,*
21,0,0.0400,0.0100,0,0,45.1*
21,0,0.0400,0.0100,0,0,135.1*%
......

Is this format correct? and if not, any suggestion to get the right format? I hope I have not to learn how to use Eagle or any other CAD package…

Interesting - I don’t think I’ve seen a drill file like that. Ben probably has…

Try the RS-274D format. That’s not quite right either, but I think it’s closer than the extended output. You can email your order to Ben and he’ll attemp an import. CAMTastic may be able to handle it…

-Nathan

This file is from a 4 layer-6 mil board I have made at work. I haven’t started yet the design I’m planning to send you because I want to know if you can handle this kind of DRD files. If you confirm you can’t, I’ll have start learning Eagle (and I’ll have to make my libraries again :().

If it doesn’t matter that this board has 4 layers, I can send you the gerber files to confirm whether you can or not import them.

BTW, I have tested with RS-274D format and this is the result:

G54D92*
G01X01837Y00300D02*
Y04235D01*
X03935D01*
Y00300D01*
X01837D01*
G54D140*
G01X02471Y-01883D02*
X02437D01*
X02454D02*
Y-01783D01*
X02437Y-01800D01*
X02334Y-01833D02*
X02384D01*
X02392Y-01850D01*
Y-01867D01*
X02384Y-01883D01*
X02334D01*
X02326Y-01867D01*
Y-01850D01*
X02359Y-01783D01*
X02297Y-01883D02*
X02231D01*
X02297Y-01817D01*

Thanks a lot for the support, I really appreciate it.

OK, I’ve been researching, and I have finally downloaded Camtastic DXP (I don’t really know if this is the version you use at Sparkfun). I have renamed the output files as you say in the tutorial (.cmp, .sol, etc) and finally I have imported it with Camtastic DXP. It have worked with the default import options:

http://img277.imageshack.us/img277/6346/import5su.gif

Note it’s 3.4 leading format, but I have also changed it to 2.3 trailing and worked both times, I suppose the auto-detection option overrides these settings.

Now I have some more questions… My .DRD file outputs the drill locations and also a table containing the drill tools sizes, as shown in this image:

http://img278.imageshack.us/img278/5091/drd2en.gif

Is this correct?

Also, the border of the board is in two layers: the .drd and also in a file specifically created for the border (a .fab file). Is this OK? If you don’t need the .fab file or if you want me to put the border in other layer, please let me know.

Thanks in advance.

You are not alone on using Orcad for layout. It is an excellent piece of software and I use it for all of my designs. There is the issue of drill files thought. Someone on the forum wrote a program that converts the thruhole.tap → thruhole.drl. I have it at home (not here at work), just private message me if you are interested.

PM sent!

Thanks a lot for help.

I started the Eagle tutorial, but I decided not to use it when I saw how crappy the autorouter is. With Cadence you have the Specctra autorouter, that is by far the best autorouter I have ever seen. I have routed with it really dense 6-layer boards with great results, I had to do only a few changes to the auto-routed board.

Has anybody info about what layer in the gerber files is the border of the design supposed to be?

doragasu,

I have ordered several boards from Spark Fun, all designed with Orcad 9.22. I’ve had nothing but excellent results. Hopefully I can answer your questions.

That .drd file is merely a gerber of the drill layer you see in Layout. So, it’s just those graphics of the drill data. I have not found it to be all that useful.

The “real” drill file is the thruhole.tap that the post-processor creates in Layout. It looks like a regular drill file:

%

T1C0.0200F200S100

X009300Y011000

X010100Y009100

I use the extended gerber setting, and the 2.3 output format. The board outline in my design is usually on the global layer (layer 0) in Layout. After creating the gerber files, this board outline is in the top assembly layer. It’s the “.ast” file.

So when I send my files off to Spark Fun, I include a .zip of the following:

.ast contains the board outline (I like to delete all the text in Layout)

.top top copper

.bot bottom copper

.smt soldermask top

.smb soldermask bottom

.sst top silkscreen

.ssb bottom silkscreen

.dts drill size chart

.tap the drill file

No .drd file is needed. Hopefully it’s an easy matter for Spark Fun to process these files, but I have not heard them raise any issues.

I think it’s just a matter of other programs using a different naming converntion for our thruhole.tap file.

  • Mike

So it was that easy after all!

Thanks a lot mike!, I’ll start my design as soon as I get some spare time…