I’m designing my first little board which is supposed to give some “UI” to my dev boards. As you can see it contains four LEDs, a Buzzer, and a Switch (which all will be then connected to GPIOs) connected to a header that is supposed to be compatible with a breadboard. The ERC seems to be fine.
Now I placed this in the PCB editor using footprints from the builtin library and before actually routing anything, I’m greeted with a lot of clearance violations at the components:
Nearby: I also don’t understand the error with regards to the header. The header is supposed to extend beneath the board to support plugging it into the breadboard, so why is it complaining that it’s not 100% within the edge cuts?
I did not change anything, so they were left at the default values. I changed them now to match your settings, but I still have the same error. Taking another footprint for the components didn’t change anything either. I still don’t know what the problem is. Are footprints or the component placing (where do the offending 0.18mm come from) or some settings to blame? Is it possible that the default net class properties (clearance 0.2mm) are incompatible with the footprints?
I still don’t know what the problem is. Are footprints or the component placing or some settings to blame?
footprints placement: no
footprint selection combined with netclass/board constrain: yes
where do the offending 0.18mm come from?
look into the exact drc-error-description: clearance violation between “pad1 of D2 and pad2 of D2” → so the gap between the pads is not big enough for the netclass/board constraint
Is it possible that the default net class properties (clearance 0.2mm) are incompatible with the footprints?
Thats very well possible. The default board setup constraints and the default netclass values are only default values. Especially for small footprint with small pads and small pitch (pitch==gap between pads) the default constraint values are to coarse.
So you as the designer have to set the netclass/board values, depending on the used footprints and depending on the used pcb-manufacturer.
I believe that your are using 0402 components, the space between the pads are 0.48mm, your minimum clearance should be smaller than your defined 0.25mm, 0.20mm should be sufficient.
I think the OP is using a 0201-sized footprint. At least C0201 has exactly 0.18mm space between the pads, this is exactly the value from the DRC-error-report.
And for 0201-footprints the default board/netclass constraints (with clearance==0.2mm) is to coarse.
@DrMickeyLauer : Additionally for a beginner I would strongly discourage to use such small footprints. As a beginner you should use devices with 1206-footprint (these parts are 3.2x1.6mm) , and later you could advance to 0805 or 0603 devices.
Meh, I find 0603 to be easy to hand-solder with good tweezers and a small soldering iron, no special tools needed otherwise. And I don’t have great motor skills. Hot air would make it even easier.
But yes, I would never use 0201 unless I’m designing some very dense board with very tight size constraints, like the board of a smartphone or watch.
Thank you, this is it! I must confess that I need to do more research on where the gazillions of footprints for one component (like a resistor, or a diode) differentiate themselves and which ones I should use (in order to prepare for sending the board to a manufacturer).
