How do I create mounting hole with vias

Question

I'm looking for a way to create mounting hole with 6 vias (as a library component) for M3 screw. I was able to create such a package but when I use it on a board and run DRC, I get "Overlap" errors. The vias are defined as small pads since vias are not available in library designer. Is there a way to get rid of the errors? I remember that I was able to define such a component in KiCAD and I' surprised that in Eagle it is that difficult.

Here: pcb design - Mounting hole on a PCB - Electrical Engineering Stack Exchange is an example of such a mounting hole (the right most on the photo).

Mark

autodeskguest · Accepted Answer

As you can see, in both cases "vias" as reported as "Overlap" by DRC. How can I get rid of this last error? I believe your issue is : The mounting hole giving the overlap errors has a schematic symbol with a pin that is not connected to any net. Perform an ERC and you will see the unconnected pin listed. Simply apply a stub net to that pin and the overlap errors go away. HTH Warren

autodeskguest · Answer

On 4/06/2016 6:50 p.m., markusbass wrote: I have some progress. The problems that I had with polygon were a result of the way I tested the package. There were no other tracks on the board and no other components inside the polygon. After correcting this the solution almost works. It looks like this: The "Overlap" error is not reported now. But the pad is not connected to the ground despite the fact that the polygon is "GND" , the mounting holes are connected to GND on the schematic and the package has "Thermals" option checked. How can I correct this problem? Also two vias are connected with track but this will be removed during drilling of the board. Why this track is displayed? The current solution uses "append" feature (as suggested) and "@x" in the names of the small pads (but I'm not sure whether this is important). Mark -- To view any images and attachments in this post, visit: https://www.element14.com/community/message/198809 The track between two vias is likely to be a polygon orphan. Review the attached library. It gives a PTH mounting hole and 6 stitching vias. When you set DRC to appropriate values there are no DRC errors. Ignore the sizes in this example and create sizes that suit you. If you don't get the attachment at E14. Get it from the news,cadsoft.de newsgroup or the EagleCentral.ca mirror. HTH Warren

autodeskguest · Answer

On 04/06/16 07:50, markusbass wrote: I have some progress. The problems that I had with polygon were a result of the way I tested the package. There were no other tracks on the board and no other components inside the polygon. After correcting this the solution almost works. It looks like this: The "Overlap" error is not reported now. But the pad is not connected to the ground despite the fact that the polygon is "GND" , the mounting holes are connected to GND on the schematic and the package has "Thermals" option checked. How can I correct this problem? Also two vias are connected with track but this will be removed during drilling of the board. Why this track is displayed? The current solution uses "append" feature (as suggested) and "@x" in the names of the small pads (but I'm not sure whether this is important). The presence of those stray tracks suggests the hole isn't really a hole (or isn't present on all the layers a hole should be on) since tracks that pass through holes should throw DRC errors. Can they be ripped up? The airwires remaining after a ratsnest suggests that your pads are not connected to the same net as the polygon. This could be because they're unconnected - if your library symbol names them GND that is not enough to make them GND pins. Either the schematic must connect them to GND or the pins on the library part must be "power" pins called GND (and possibly hidden on an uninvoked symbol, not sure on that). Personally, I'd name the pins/pads in the library as something generic, then explicitly connect to GND on the schematic. It makes for more clarity and flexibility.