Footprints & Symbols for Microstrip Components

[spflanze]

I am designing a microstrip resonator (Omega Resonator) into a pcb. The copper pattern was such that it was easiest to design it in Inkscape. I then had Inkscape create a PNG of it, and I used KiCad’s Image Converter to convert that PNG into a footprint.

I created a schematic symbol for the foot print which has two pins. In the footprint editor I embedded inside the resonator’s microstrip trace an SMD pad for each of its schematic symbol pins at the location the input, and output, ports of this resonator are to be connected to with PCB traces.

In the PCB Editor I cannot connect to this footprint due to clearance rules. The PCB Editor does not recognize the copper from the PNG file as being a member of the SMD pad’s net, and so I cannot get the trace to connect to the pad. The trace will not enter the copper area defined by the PNG file.

This problem is complicated by the fact that the microstrip resonator has a DC electrical connection between the two SMD pads. I recognize that in the Schematic Editor the wires going to each of these pins will have to be assigned the same net. But how can a net be assigned to the copper area defined by the PNG file?

Is there a better way to do this?

[wildcatrealtime]

Hi @spflanze,

After importing the PNG to a copper layer, you can try the following:

1. Select the shape you imported
2. Right mouse click, a menu opens
3. Select [Create from Selection]
4. Select [Create Zone from Selection]
5. You can then assign a net name to the shape,then you can connect traces to it.

[maui]

you may consider these options:

RF Designing Tips

I think a FAQ on ‘RF designing tips’ could be a start… StepUp Stepup: the Sketcher for Footprint generation is working well with outlined shapes (i.e. Ti dxf files for RF antennas https://www.ti.com/tool/CC-ANTENNA-DK2 e2e.ti.com/support/wireless-connectivity RF discussion CC_2D00_Antenna_2D00_DK2.dxf source file RF tools are a featured Action Plugins/Scripts for RF Curved traces or RF Taper RF tools for KiCAD Qucs-RFlayout is a great tool to convert Qucs model directly to KiCAD Q…

[spflanze]

Thank you.
Once this is done in the footprint editor is there a way to make this zone a pad which can be assigned a pin number that can be associated with, and get a net name from, a schematic symbol’s pin?

[wildcatrealtime]

In the example above, you import the shape to the board, then convert it. After that, you can assign a net name to the shape. That will allow you to connect any wire that belongs to that net to your shape.

I think you cannot assign a net in the footprint editor, since the nets were not created yet. However, you may insert a pad that touches your shape and later assign a net to the pad.