Hey All -
I’ve got a board that I’m using a trace antenna. I’m curious as to why the GND feed is not interfacing with the top layer copper pour; that net is GND.
I’ve tried changing the pad connection to zone to solid. This image might be better than my description.
It looks like the trace that’s on the GND pad isn’t actually a GND trace for some reason and so the fill is keeping clear of it. There are tools on the left toolbar to make pads and traces outline only which can help in finding stray bits of track, and in the netlist import dialog is a button called “Rebuild board connectivity” which can sometimes reconnect bits of track that have lost their net for some reason. Try tweaking that trace a bit and see if you can get it to work.
For PCB trace antennas I’ve done in the past I defined a footprint with a tiny surface mount circle footprint with no paste/solder mask layers which I add as a CONN_1 to the end of my antenna trace in the schematic. Placing this footprint at the open end of the antenna means the trace is going from somewhere, to somewhere which helps enormously with loosing net names and keeping tracks tidy. KiCAD can easily get confused by traces that go nowhere it seems.
You definitely should try what Nathan suggested, but you might also want to check the properties of your copper plane. Make sure that where it says “Pad connection” you choose “solid”. Also, if that doesn’t work, you can try to manually place a track between your GND pad on your antenna and somewhere in the copper plane. If you place your track correctly then you won’t get copper anywhere you don’t want it. Run the DRC after to see if it fixes your layout. Good luck, hope that helps!
Another suggestion for you (and others): if you’re working on GitHub, we can clone and take a look at the project. Be sure to mention what rev of KiCad you’re using if/when you do that.
Nathan -
Thanks for the feedback.
I tried the “Rebuild board connectivity” but it still yielded the same result as seen in the attached image in my initial post.
I appreciate the comments about the not having not having paste/solder mask layers. The antenna pads did have the paste and solder mask layers included. I’ve since fixed that. I had hoped that my fix the issue, but it did not.
I tried moving the a very small circular pad in the antenna trace. I noticed that I was getting essentially the same result. See the image.
I started wondering if the issue has to do with the GND feed overlapping the pad. I created a temporary footprint to test this hypothesis. Here is the result. It seems to prove the hypothesis.
I’ve essentially cheated to get the desired gerbers.
I created a temporary footprint that removes the feed overlapping the pad and run the DRC. imgur.com/IWunVFe
Then I read in the original footprint with the overlap on the pad and do not run the DRC. imgur.com/lqm71Cv
Then I get the desired gerber files. It doesn’t sit well with me to not run the DRC, so if anyone has a different procedure I’d be interested to hear it.
Sorry for the bad links, it wouldn’t let use a hyperlink, upload or paste the link.
Ok, the problem is that you’re trying to connect two nets together. You have the antenna net and the GND net connecting with no component between them. The DRC will always associate the track with one or the other, in this case it seems the ground feed trace is getting assigned to the antenna net and so the fill is not joining up, you should also get a DRC error where the track hits the ground pad.
Two things to try would be:
Just make the antenna net ground, this doesn’t make sense electrically but in a naive approach of assuming all connected copper is at the same potential would satisfy the DRC.
Make a special coupler footprint and add that as a component between the two nets. I’m not sure how well this approach might work, but you can set the “Net pad clearance” on the second tab of the edit pad dialogue to negative which should allow you to overlap two pads without causing a DRC violation. This way you could then make a footprint with two pads on different nets that actually overlap so create a single area of copper.
Hey Luke, sorry, the system auto tags someone who posts too many links early (as that is the indicator of spamming). I figured out how to approve the links, you should be able to post links again. If you move up in “trust level”, you’ll also be able to drop pictures directly over top of the input text box (one of my favorite features) and it auto uploads to our S3 container.
Another “hack” solution is to use 0 ohm resistors to electrically join separate nets and avoid DRC complaints.
Hi All -
I was able to get back to this issue. I was eventually able generate something I was comfortable with that didn’t require me having use the little DRC trick I had used to just generate the desired gerbers.
I’ve outline what I did below.
