Trying to create a custom foot print for a solder jumper, but same issue applies to any custom pad, I do the following:
create two copper sections with “Draw a graphic polygon” icon in the drawing tool bar.
add pin to each ploygon
place a silk screen chevron between the polygon areas for inspection purposes
add a courtyard boundry
Once done the foot print show two pins in the middle of their respective areas but the polygons are not filled. Inspecting the properties for the polygons shows that they are both set to “filled”.
I save the footprint and then select and place it in the schematic. The view of the footprint when selected in the schematic tool shows the custom pads filled. When I update to the PCB, the footprint shows on the PCB tool as non-filled with the custom pad shape shown in outline.
When the Gerber files are plotted the custom pad shape is filled in.
So is there a way to see the custom pad shape in the PCB editor?
I can see that the solder jumpers in the library brought in from git all come into the PCB editor as filled.
I opened the footprint editor and I started with two SMD pads, edit your shape and size to your liking.
If you want a strange shape, use the graphic polygon or some other tool (with shading. ie. not line or arc) on the same layer as your pads.
Next, right click your pad inside the graphic shape. From “Select” menu, choose “edit pad as graphic shape” or (Crtl + E). This converts the pad to include the whole of the graphic polygon on the pad layer.
Click Ctrl + E again, to exit, and you have your new footprint.
Save this new footprint in a personal library and you are done.
For the Schematic, there are an assortment of Jumpers in the Kicad “Jumper” library. One of those should suit you.
Attach your new footprint to your chosen jumper symbol.
Except may be not correctly defined footprint (I don’t use custom shape and can’t check anything as have here only KiCad 5 (because of Windows 7)) I suppose your display settings (icons at the left toolbar) are set to display some things only as outline.
Yeah, I tried that @RaptorUK and @Piotr, but if it is a filled graphic polygon in a footprint, the zone controls do not work.
The only way I have found to make an outline only, in a graphic in a pad is to use the line or arc functions, whether the graphic is incorporated in the pad (Ctrl + E) or not.
The OP states he used the “filled” Graphic Polygon tool.
Sorry for the confusing regarding pin and pad. I should have known better.
So step 2 in add PAD to each polygon.
Forgot to mention, I am running Kicad in linux (LMint 20).
I wish I could see how to add pictures (screen shots).
I am sure it would make thing more clear.
Looks like I can upload files so I will try that.
In the PCB editor I have zones set to show fill, but it does not make any difference.
View in footprint editor:
Those screenshots clarify it.
It is called “Sketch mode” and you can find it in the menu at: PCB Editor / View / Drawing Mode.
There are also buttons for it in the toolbar on the left side of the PCB Editor:
This mode can be very useful to check if things are overlapping.
But also. use the Edit Pad as Graphic Shapes mode ( with [Ctrl + e]) as jmk mentioned in one of the first replies. This is quite important, because when your graphic shapes are not part of the pad itself, then you can not connect copper tracks to the pad, because the netlist does not recognize your graphics as a part of the net.
Interesting that it the view setting is passed on to the PCB editor.
Now the problem is that the DRC is indicating a conflict when I try to connect to either pad.
Not really. I saw you already posted your response while I was still editing mine to add that part.
The [Ctrl + e] Pad edit mode is a bit finicky to work with. It works quite good, but you need some practice. It can for example add or remove graphics from the pad by entering or exiting that mode. If the graphics has become part of the pad, then all of it will light up when you click the pad to select it. The pad number will then also be much bigger. Compare the sizes of the pad numbers in the first screenshot jmk posted.
If the pads are part of the netlist and you still can’t connect to it, then post a new screenshot. of the footprint, and preferably with a selected / highlighted pad.
