PCBWay Missing Copper Pad - Page 1
Forum section: electronics / general

author: aleperno
author_rank: Newbie
timestamp: June 05, 2020, 04:44:42 pm
content: Hi,I put an order in PCBWay and now I'm in a back an forth with 'support' due to them seeing an issue with the top copper layer that I'm not seeing; thus not able to continue the process.This is what they sent meBasically you can see a square "blank" with the trace ending there and the drilling hole, where it should be also showing a square copper area (the pad).I uploaded the same Gerber files to the PCBWay online gerber viewer and also used Linux Gerbv and in both I do see the copper padI used EasyEDA online editor in which the pads are under the "Multi-Layer Layer"Is there anything I might be doing wrong?Thanks in advance for any help

author: jmelson
author_rank: Super Contributor
timestamp: June 05, 2020, 05:06:40 pm
content: Quote from: aleperno on June 05, 2020, 04:44:42 pmClearly, this is an aperture problem. What format is the gerber file? RS-274X, or plain RS274 with a separate aperture file?What it looks like is their software for some reason sees that particular aperture as a small round one, while you intend a large square one. You might tryu to figure out which aperture # is the square one, and then tell them that aperture D22 or whatever is not being properly interpreted by their software.A rectangular pad definition will look like this in RS274X :%ADD22R,0.071X0.018*%That means that when drawing with aperture D22, it should be 0.071 in X dimension and 0.018 in Y dimension. (These are inch apertures, for mm the numbers will be a bit bigger.)Jon

author: aleperno
author_rank: Newbie
timestamp: June 05, 2020, 06:24:18 pm
content: Thanks Jon,AFAIK it is RS-274X (will attach the Gerber if anyone finds it helpful).The thing is in their screenshot the red dots are the drill holes, so I cant even distinguish if my apertures are being interpreted as small round ones, squared small ones...or not being taken into account at all.But it looks like there is an issue with the apertures... if you look at the 6 "holes" (for a switch) they also seem to be missing the pads.Could it be that their soft instead of interpreting as mm uses mil or something alike?I did inspect the top layer gerber and aperture definitions look OK

author: jmelson
author_rank: Super Contributor
timestamp: June 06, 2020, 07:12:29 pm
content: Quote from: aleperno on June 05, 2020, 06:24:18 pmPretty unlikey, the file will be either all metric OR all inch. it cannot be mixed, unless somebody there is doing manual processing of the files.The first two line of an RS274X file should look like :%FSLAX23Y23*%%MOIN*%for inch units, and :%FSLAX43Y43*%%MOMM*%for mm units. The first line defines the number of digits before and after the implied decimal point, the 2nd line specifies the units used.That applies to both the apertures and the linear measures of the traces and their positions. So, the traces all look right. Traces are drawnwith D01 (go to point) and D02 (draw in the current aperture to point). Apertures are flashed with D03.For such a simple file, you might be able to look at it as text (usually the apertures are flashed first, then the traces are drawn. The filled arewill be traces, and likely will be quite a lot of traces to fill up the plane area.)QuoteYes, something seems to have gone way wrong at PCBway on this job. You should be able to send them your picture and they should know what went wrong.On my boards, I create the Gerbers and then import them back in to a blank PCB, and go through them layer by layer. That way, the ONLY things I can see come from the Gerber data. If there is a discrepancy, it means the Gerbers did not get generated right. There are also some free gerber viewers (Gerbview, CAM360) that might be useful.Jon

author: aleperno
author_rank: Newbie
timestamp: June 07, 2020, 10:23:11 pm
content: I finally found out the issue and boy it was sillyI had an issue with my schematic where my PCB is ~100x75mm, there was a huge "shape" surrounding my PCB that I didn't notice because I was always zoomed in.It looks like the online gerber viewers focus in the board outline or something like that, because that "shape" was never visible, unless just opening the Top Layer.I decided to install Eagle and try to import my Gerber files and see if that caused any issues...and behold, it starts processing the file sequentially until it encounters one of the points of the "shape" and failsWe can see in the image the pads are not seen. So my guess is the software they're using fails due to the same reason (maybe without a warning) and stops processing the file and so it happens the pads definitions are after the failing "points".I deleted that "shape", re-sent the Gerber and was confirmed everything was OK.Thanks again Jon for the assistance

author: jmelson
author_rank: Super Contributor
timestamp: June 08, 2020, 03:43:06 am
content: 3.4 METERS ??!!?? Wow, lucky they didn't charge you for making that board! (If they could make one that big.)And, the shipping charge, too! I'm wondering if there was some foulup in the handling of the number of digitsleft and right of the implied decimal point? My software always shows the X and Y extent of the board, so Iwould quickly detect something very wrong.Jon