Error with Footprint Designer and OrCAD PCB
Printed From: PCB Libraries Forum
Category: PCB Footprint Expert
Forum Name: Questions & Answers
Forum Description: issues and technical support
URL: https://www.PCBLibraries.com/forum/forum_posts.asp?TID=956
Printed Date: 07 Nov 2024 at 10:11pm
Topic: Error with Footprint Designer and OrCAD PCB
Posted By: Lekselius
Subject: Error with Footprint Designer and OrCAD PCB
Date Posted: 04 Jun 2013 at 6:58am
|
When generating an Ethernet connector for OrCAD PCB V16.6 using "FP Designer" (FD) the pads are wrong. They look OK in "Footprint Designer" but there is an error when running the .bat file and the resuling footprint are without holes. I have tried this both with OrCAD V16.3 and OrCAD V16.6 with the same result.
The error message from the padstack editor is: --- PADSTACK
ERRORS and WARNINGS:
DEFAULT
INTERNAL: No pads are defined. When loaded into a design, no internal pads
will be added for unmatched padstack layers or when
additional internal connection layers are added to the design. Drill hole
size is equal or larger than smallest pad size. --- The large mechanical hole are incorrect in the resulting footprint and all holes are missing drill information etc. Attached are screenshot of the error message, FP designer window with the footprint, and the resulting footprint in Orcad PCB designer 16.3. Attached are also the exported footprint to be run with orcad 16.6.    uploads/3458/RB1_125BAG1AN.zip" rel="nofollow - uploads/3458/RB1_125BAG1AN.zip
|
Replies:
Posted By: chrisa_pcb
Date Posted: 05 Jun 2013 at 3:08pm
|
Hi, What version of our tool are you currently using?
|
Posted By: Lekselius
Date Posted: 06 Jun 2013 at 11:23pm
| I'm running PCB Library Expert version 2013.02 |
Posted By: Tom H
Date Posted: 07 Jun 2013 at 7:03am
|
Did you watch this Footprint Designer training video? http://www.pcblibraries.com/products/fpx/userguide/default.asp?ch=104" rel="nofollow - http://www.pcblibraries.com/forum/pcb-library-construction-guidelines_forum30.html" rel="nofollow - http://www.pcblibraries.com/forum/pcb-library-construction-guidelines_forum30.html |
Posted By: Lekselius
Date Posted: 11 Jun 2013 at 10:57pm
|
I have watched the video and followed the exact same step as in the tutorial, creating an identical footprint but I get the same error when importing the footprint as I got previously. This is the footprint in package designer:  Error when running the batch file:  Resulting footprint in Orcad:  And the files to create the Orcad footprint created by FP designer: uploads/3458/Tutorial_1234N.zip" rel="nofollow - Tutorial_1234N.zip |
Posted By: BennsPCB
Date Posted: 15 Jun 2013 at 7:27am
|
Have you turned on "Setup/Design Parameters.../Display non-plated holes". Otherwise you only see the pad, which will be drilled away. Just my 2 cents, ... |
Posted By: d_nilsson
Date Posted: 25 Jul 2013 at 4:55pm
|
Hi, Was this issue ever resolved? I'm running into the same problem, using FP Designer in version 2013.08. If I open up the sample part AMPH_10-507143-85E in Sample Data - FP Designer.fpx and try to just build it (no changes) for Orcad PCB 16.6 the padstack definition for the NPTHs (keying holes using padstack c100hn295k395_395) is invalid. Cadence padstack editor will spit out during processing of the batch file: PADSTACK ERRORS and WARNINGS: Drill hole size is equal or larger than smallest pad size. Pad will be drilled away. I think this is since what FP Designer is telling Cadence to do is to add 1mm pads on all layers without thermal relief or anti-pad and then drill with a 2.95mm drill, Cadence doesn't like that definition of a NPTH. Is this a known bug? Any workarounds? According to padstack designer in FP Designer there should be a 3.95mm antipad, but that antipad seems to be set to "null" in Cadence when instead it maybe should have been the regular pad that should have been set to "null". Thanks Daniel |
Posted By: Tom H
Date Posted: 25 Jul 2013 at 5:41pm
|
The CAD interface programmer (Chris) is on vacation and will be back next week. ------------- Stay connected - follow us! https://twitter.com/PCBLibraries" rel="nofollow - X - http://www.linkedin.com/company/pcb-libraries-inc-/" rel="nofollow - LinkedIn |
Posted By: d_nilsson
Date Posted: 26 Jul 2013 at 4:12am
|
Ok, I will manually modify the padstack definition in Orcad PCB Designer then until Chris is back. |
Posted By: chrisa_pcb
Date Posted: 10 Aug 2013 at 12:44pm
| I'll be looking at fixing this issue shortly, but it probably won't make it into the tool until the next update in a couple of weeks. |
Posted By: afyon
Date Posted: 11 Mar 2014 at 10:48am
|
@Lekselius, I’m having the
same issue so I wanted to thank you for starting the thread. I worked around
the issue by making custom pads. Just for future reference, has this issue been
fixed now and if so, which revision number includes this update. I don’t have
an internet connection the PC I work on so I just wanted to know if the latest
patch would update this for me. I’m kind of hoping I can find a small update
patch instead of updating the complete OrCAD. http://www.7pcb.ca/PCB-Assembly-services/" rel="nofollow - pcb assembly
|
Posted By: chrisa_pcb
Date Posted: 11 Mar 2014 at 12:25pm
|
Can you post your FPX along and the details with the exact issue you may have? I'm pretty positive the initial issue was handled but would like to see how its the same or differs from the original issue. Also. make sure to get past a padstack error that you close the error, do file -> save in pad_designer, you should get the error again(close it), it'll ask you to save padstack with warnings.. put yes, and then close it. If you don't manually save a non-plated padstack with warnings, it will not generate the .pad and use the first .pad it can find in the directory rather than the one you wanted it to generate. This will cause a regular non-plated hole to tend to be generated improperly. Its a OrCAD PCB issue that if you simply close out the padstack designer, it doesn't save the actual .pad with warnings, if it had warnings. |