How to make a library elelment of an antenna

[anthonyEX9NB]

I want to know how to create a library element of an antenna. This antenna is a PCB trace antenna that is printed on both sides of the PCB. It has copper areas that overlap with other copper areas. What happens is that I get a billion overlap and other errors when I run the DRC.

Can you tell me how to do this or give me some links to how to do this?

[ritste20]

Here is an older thread where we were talking about creating trace antennas and manipulating them in the schematic and board editor.

https://forums.autodesk.com/t5/fusion-360-electronics/connect-vias-to-pins-without-adding-an-extra-c... 

Are you familiar with the process of creating custom library elements?

Regards,

[anthonyEX9NB]

Yes, I have made many custom library elements.

I reviewed the solution you linked to, and it seems that eliminating the overlap errors means I have to name the elements in the library?

In the case of the antenna, I use "Lines" to make the antenna traces in the footprint. But you can't Name a line. I use PTH pads to connect the Line on one side of the board to the Line on the other side of the board. You can assign a Name to a PTH pad, but I can't assign the same Name to all the PTH pads in the antenna pattern.

Am I missing something?

[ritste20]

Correct, the pads must all have unique names. But once the symbol is placed in the schematic, you should be able to connect the nets to form the complete copper trace in the board editor. You would just create pins on your symbol for the start and end of the antenna loop and not include pins for any additional pads or PTHs you placed to create the actual footprint. Lines should be fine for the trace as long as they are on the copper layer.

Does that make sense? As I said it'd been a while since I've gone down this road and I'm not sure what has changed with recent updates.

Regards,

[jorge_garcia]

Hi @anthonyEX9NB,

I hope you're doing well. The key thing here is to create the antenna as an arbitrary pad shape and place an SMD pad or PTH pad to define connectivity to it. So you would draw the contour of the antenna using a POLYGON then within it's boundaries you would place a pad. That pad is what gives the antenna it's connectivity.

Let me know if there's anything else I can do for you.

Best Regards,

[anthonyEX9NB]

Good day, Gents! Just getting back to this now. See the attached PDF file for some more detail.

My antenna is  created in the Library Editor with a rectangular SMD, 19 vias, and Lines that overlap the SMD and the vias. Jorge says I should use polygons to draw the shape of the antennea but Steve Ritter says that Lines should be okay.

The problem is that the Lines don't seem to connect the SMD and vias so when I place the antenna on a PCB there are many Airwires which the DRC shows as errors.

The antenna needs to be as shown: thick traces with rounded ends. This is easy to create with Lines but it would be very cumbersome to create with polygons. But maybe polygons are the only way to connect the SMD and the vias so that I don't get a ton of DRC errors.

Also, with the way I have created the antenna and placed it in the design, the antenna pattern is created correctly on one side of the 3D model of the PCB but not on the other. What's up with that?

[jorge_garcia · Accepted solution]

Hello @anthonyEX9NB,

Thank you for the PDF, it clarifies everything. So first off, you've drawn everything correctly no problems. The reason you get the airwires is not because of the pads, it because of the device definition. In the second page of the PDF you show the connection in the device editor. Between the G.FEED pin and all the pads that are connected to that pin, you'll notice there is a little icon. If you hover over it, it will say All. Click it and it should change to Any, in this case what you want is ANY. All means that all of the pads must have traces to them in order to be considered connected, Any means that the netlist is satisfied as long as you connect to one of those pads. In your case you'll always just route to the feed point. Try it and I think you'll see the extra airwires go away.

For the issue in the 3rd page, the copper is likely correct but Fusion is expecting a 3D model (which in this case doesn't make sense). Since it hasn't been assigned a 3D model you get the default black rectangle. When you push from 2D to 3D you'll see in the dialog the option to specify that components don't need a 3D model in the components section just uncheck the box for the specific helical antenna component.

Hope this helps.

Best Regards,

[anthonyEX9NB]

Wow!! This is amazing! Changing the Any vs All is something I would have never found by myself! Not only did this concept fix the airwires for the antenna, but it fixed airwires for a few other parts that use the same concept.

Same goes for the telling Fusion 360 that a component doesn't need a 3D package. It fixed the antenna, which is now fully visible, as well as some fiducials and a plug-of-nails connector pattern that I use.

Thank you!!