Drill holes on printouts - Page 1
Forum section: electronics / general

author: MadModder
author_rank: Regular Contributor
timestamp: January 16, 2016, 03:42:45 pm
content: When I print a layout it is possible to either have the holes on every pad, or not have any holes (solid pads).But it is very difficult to drill in the center of the pads with any of those two options.What I want is to have a tiny hole, maybe 10-15mil, on every through hole pad, regardless of what the drill sizes are set to on the pads.As a center punch. That way it is way easier to drill the holes manually.Is this possible?I could do that in Orcad PCB, I think it was called drilling aid or something similar. But I don't use Orcad anymore.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: January 16, 2016, 03:44:40 pm
content: There's a setting in there for "leave pads empty". Possibly not on the PDF outputs, but yes on the gerbers.Tim

author: MadModder
author_rank: Regular Contributor
timestamp: January 16, 2016, 04:20:13 pm
content: In fabrication outputs, gerber files, I have no option for empty pads. I can place drill position cross hairs, and drill size symbols.I'm using AD16.Ofcourse one solution is to make all drill holes tiny on all footprints. But then I can't use those footprints if I want to use some PCB manufacturer in the future. And I get a very incorrect drill table.

author: pmcouto
author_rank: Unknown
timestamp: January 16, 2016, 04:53:38 pm
content: MadModder,AFAIK Altium cannot do it.However, you can use this little trick:1-Make a copy of your PCB file2-Open the copy of your original PCB and use Altium’s “Find Similar Objects” feature to select all multilayer pads on the PCB3-Change the hole size to the value you want4-If you have vias, repeat step #2 to select all vias and edit hole sizeHope this helps

author: T3sl4co1l
author_rank: Super Contributor
timestamp: January 16, 2016, 05:15:07 pm
content: Ohh, I'm thinking of "include unconnected mid layer pads", nevermind.You could do it in a roundabout way by plotting the layer to PDF, including holes. Set a black background, copper color white, and plot drill holes (they'll end up black by default, and I don't think can be changed..?). Then print negative, somehow at some stage (possibly requiring postprocessing).Or open the gerbers in CAMTastic, and there might be a way to cut out copper under the holes. I'm not sure. CAMTastic is astonishingly opaque to try to do anything with.Tim

author: MadModder
author_rank: Regular Contributor
timestamp: January 16, 2016, 05:24:07 pm
content: Well, yes. I was thinking about combining the bottom layer and a negative drill layer, but was unsure whether the holes would be actual size or dots... Have to test.@pmcoutoI have tried that. All pads are selected, but when I right click, select properties and change hole size, only the pad I clicked on is affected. And if I click somewhere else than on a pad, I can not change properties at all.No, the plotted drill holes have the exact same sizes as the holes on the layer output. So no dice...

author: T3sl4co1l
author_rank: Super Contributor
timestamp: January 16, 2016, 05:28:09 pm
content: Quote from: MadModder on January 16, 2016, 05:24:07 pmYou must use the PCB Inspector Pane to edit selections. Or look at the PCB List and Edit them spreadsheet style.Tim

author: MadModder
author_rank: Regular Contributor
timestamp: January 16, 2016, 05:50:52 pm
content: I can't edit the hole parameter in the PCB inspector when multiple pads are selected.It just says <...> and when I click on that it reports the size on the first hole, but the value is uneditable.The list works, but changing one pad at a time is quite tedious. I could however set up an automatic keyboard script in Autoit...Do I really have to finish my CNC router and have that drill my holes?

author: pmcouto
author_rank: Unknown
timestamp: January 16, 2016, 07:18:55 pm
content: MadModder,Try this:-Right-click on any pad-Select “Find Similar Objects…” menu option-“Find Similar Objects…” screen pops-up-Under “Kind” section, make sure “Object Kind” is “Pad” and last column shows “Same”-Under “Object Specific” section, make sure “Layer” is “Multilayer” and change last column from “any” to “Same”-Click “Apply” and check all pads are selected (highlighted)-Click “OK”-“PCB Inspector” screen pops-up and all pads remain selected-Under “Object Specific” section, find “Hole Size” parameter-Click on the value on the second column (it shows “<…> if you have multiple hole sizes) and enter the desired hole size-After entering the new hole size value, press “Enter” and close “PCB Inspector” screenAll pads now have the new hole size!Repeat procedure for Vias, if you have any and wish to also change hole size.Now, you need to setup the printout:-Under “File” menu, select “Page Setup”-“Composite Properties“ screen pops-up-Adjust parameters as needed (if you’re using toner transfer method to do your PCB, make sure you set the scale to 1.00 and select “Mono” under “Color Set”)-Click on “Advanced”-“PCB Printout Properties” screen pops-up-On the first column “Printouts & Layers”, under “Multilayer Composite Print”, delete all but the layer(s) you want to print. You probably want to keep the copper layer (Top or Bottom), Multi-Layer and the layer containing your board outline (possibly Keep-Out Layer).-On the second column “Include Components” leave both options selected-On the third column “Printout Options” tick “Holes” checkbox (you can also tick “Mirror”, if you want to mirror the printout”)-Click on “OK” to close “PCB Printout Properties” screen-Under “File” menu, select “Print Preview”-Check that what is shown is what you want to print and click on “Print”. If you need to make any adjustments, just close this screen and go to “Page Setup” again.You have now on your printer a printout with the all pads showing a hole with the size you entered!

author: MadModder
author_rank: Regular Contributor
timestamp: January 16, 2016, 08:15:18 pm
content: The problem is, I can't change the <...> value for holes when multiple pads are selected. When I click on it, it shows 42mil highlighted blue. When I click again, a cursor comes up, but I cant type in anything. I can't delete it either. Windows says *DING* everytime I press a key. I can change all kinds of things around it. I can change every pad to the same net name even. Those values I can't change, have a grey background. The rest has white background.

author: MadModder
author_rank: Regular Contributor
timestamp: January 16, 2016, 08:39:42 pm
content: Hey! I found the problem!Some of the footprints have an invisible extra pad only on the mechanical 15-layer with pin number zero, with no pin connected. I wonder why.I recall I have read somthing about a pin zero used to connect some data to in the footprint library somehow...Anyway, I selected one of those, and found similar objects that were pads, but NOT on that layer. Voila! Drill holes changed in a jiffy now.Thanks for the inspector tip.The printing stuff I already got the hang of.