Hey, I’ve put a CONN_01X04 into my schematic, basically to have some endpoints for an external usb cable. ofc they are all connected differently on my pcb, one of which to ground. I used the following footprint:
Wire_Pads:SolderWirePad_4xInline_1-2mmDrill
It shows up correctly in pcbnew, but with all pads, not just 1, connected to ground. I assume this is an error? Of course i could break out every line seperately with x1 wire pads, but maybe someone knows a better solution?
Did you by any chance get an error (or at least a warning) when importing the netlist?
If i remember correctly the footprint you chose has all it’s pads with the same pad number.
The pin/pad numbers are what kicad uses to connect between symbol and footprint pins. If a footprint has multiple pads with the same number they are connected to the same net.
1 Like
Indeed, but forgot to attach it:
Error: Component ‘P1’ pad ‘4’ not found in footprint ‘Wire_Pads:SolderWirePad_4xInline_1-2mmDrill’
Error: Component ‘P1’ pad ‘3’ not found in footprint ‘Wire_Pads:SolderWirePad_4xInline_1-2mmDrill’
Error: Component ‘P1’ pad ‘2’ not found in footprint ‘Wire_Pads:SolderWirePad_4xInline_1-2mmDrill’
Your first guess seems to be perfectly right. However I’m no expert, would you know and tell me what I can do about it?
Choose a different footprint. (Maybe make your own)
Or use 4 single pin connectors with the single pad SolderWirePad footprint.
Never ignore errors on netlist import. They mean something went horribly wrong!
1 Like
Don’t use that 
For generic off-board connections, normally you would use something like “PinHeader_1x04_P2.54mm_Vertical” or the equivalent (these have been renamed a few times).
1 Like
Also if I do not really want to use pin headers? I only need a contact drill hole to hand solder some wire to, no breakout pin. I guess I have to specify if I send this to a company for mounting that they actually should not mount the pin headers?
Depends on your assembly company. I suppose there might be some that take a KiCad project and build the whole thing without asking what you want. Normally you will specify the BOM to the assembler, and also specify what component goes in what footprint. It is very common to mark components as “no fit”, they will be used to dealing with it.
1 Like
ok then I will do just that, thanks for your help.
In addition to the option explained by @bobc there is also a way to tell kicad what to include in the pos file used by the assembly house.
Every footprint has a property called ‘Attributes’
This can be either Normal (=THT part), Normal + insert (= SMD part) or virtual.
When exporting the pos file you can specify what you want to be included. The tool-tip says this is limited to components with only SMD pads. (I am not sure if it is really implemented that way.)
1 Like
This topic was automatically closed 30 days after the last reply. New replies are no longer allowed.