"undefined aperture used" and missing pads in old Gerber Files - Page 1
Forum section: electronics / general

author: Echo88
author_rank: Frequent Contributor
timestamp: December 30, 2019, 04:05:38 pm
content: Hi,i want to manufacture a few pcbs at jlcpcb/other manufacturer based on the design-files of an Evaluation board from Linear:https://www.analog.com/en/design-center/evaluation-hardware-and-software/evaluation-boards-kits/dc230a-a.html#eb-overviewhttps://www.analog.com/media/en/reference-design-documentation/design-integration-files/230A-ABCD.zipZip contains the Gerbershttps://www.digikey.de/product-detail/de/linear-technology/DC230A-D/DC230A-D-ND/4963668#imagesPicture of the pcbSadly the gerbers arent displayed properly in a lot of Gerber Viewers i tried, likewww.gerber-viewer.com,https://www.gerblook.orgor gerbv. the program gerbv specifies the error:"Undefined aperture number called out in D code. Found undefined D code D10 in file..."In ViewMate the Layers are displayed, but missing component-pads and the trace-width isnt correct.In the attachment its visible how the traces are too thin and the pads are missing.Also the drill-file shows holes, but they arent correctly differing in size.The file "DC230A-2.asc" indicates that the gerbers were done with PADS: "!PADS-POWERPCB-V3.5-MILS! DESIGN DATABASE ASCII FILE 1.0" and the file "230A2REA.doc" shows the file-naming.Is it possible that someone here uses PADS and can use the .DSN/.pcb-file to generate gerbers, which are useful to the manufacturer and can be viewed with normal gerber viewers? Or maybe theres another way to go, to make it work?Thanks.

author: SiliconWizard
author_rank: Super Contributor
timestamp: December 30, 2019, 05:36:28 pm
content: Yeah, this is pretty old Gerber, RS274-D format, with separate aperture files. Most viewers won't take this, and most PCB manufacturers won't care either. You could re-create the aperture definitions for each file (associated .rep) and add them in the corresponding Gerber files to make them compliant (RS274-X), but that would be some work (and you need to know about Gerber...)Sorry I don't have PADS...

author: nigelwright7557
author_rank: Frequent Contributor
timestamp: December 30, 2019, 05:55:14 pm
content: As said previously its probably old gerber format with separate aperture files.You can merge the two files by hand if your careful but having said that you can verify its right by using a decent gerber viewer.I write PCBCAD software and needed a decent gerber viewer for verification of gerber/excellon output.I use GCPrevue and that works very well. Sadly its paid for version only now unless you can find an old free copy online.I found some of the online viewers were simply incorrect.

author: nctnico
author_rank: Super Contributor
timestamp: December 30, 2019, 07:59:33 pm
content: DSN is Orcad format. If you have access to pads (probably downloadable from somewhere) then you can re-create the Gerbers. OTOH a PCB manufacturer shouldn't have a problem with missing apertures. Try to upload the design to Eurocircuits and see if they can use it.

author: Echo88
author_rank: Frequent Contributor
timestamp: December 31, 2019, 02:47:42 pm
content: Thanks for the clarification that its the RS-274-D-format.I found that GerbView is capable of displaying the traces and layouts correctly after a playing around with it a bit.GerbView couldnt understand the aperture-table for the drill-file, so i changed the drillcommands to include the drill-size: T1F197S55 becomes T1C.02F197S55 for example.But i still see an XY-offset with the drillfile and am unsure how the the manufacturer knows which holes are vias and which not, since theres no mention of plating/nonplating in any file.I might get PADS as a trial-software in two weeks, when i inquire from my work-e-mail-address.

author: Mattylad
author_rank: Regular Contributor
timestamp: December 31, 2019, 04:19:14 pm
content: The information you need is all within the zip file you linked to.As standard for RS274-D, with each file there is also a .rep file.This is a text file that contains the aperture information.All dimensions are in thou/mil.Either select these files for auto import if your gerber viewer allows this or modify the aperture table within the viewer to match the apertures in the files.Check every .rep file as they may not all contain the same numbers.If your getting a drill offset this is likely because the plot has been centered on the bed before output and the NCdrill bed is not the same size as the photoplot bedso the centers are not in the same place.GC-Prevue had an offset feature that allowed you to move a layer based on 2 selection points.To identify the plated/non plated holes read drl01.rep the 20th and 94th holes are plated, the 70th ones are not.DDo124.pho is a drill drawing, import this and set the apetures from its report file and this should give you enough info to go off.

author: chrisl
author_rank: Regular Contributor
timestamp: December 31, 2019, 08:20:25 pm
content: If you goal is to just manufacture a few PCBs the zip file contains everything a fab house needs to fabricate the PCB; just to send the zip file over to a fab house of your choice.BTW the schematic is done in ORCAD and the layout is done in PADS which is a very standard CAD combo in the Valley back in the 90s.

author: emsnickw
author_rank: Contributor
timestamp: March 09, 2020, 01:35:22 am
content: It looks likes gerblook was recently overhauled. no more hanging up while processing.