Easy method for placing mounting holes

[Abhishek_bhatia]

Hello,

I am designing an carrier board for jetson-nano production SOM. It connected using this 260 pin connector.

Above is an reference image, like in the above I have placed the 260 pin connector and want to placed the mounting holes. I have 3d step model of SOM module. Is there any easy method for placing the mounting holes for standoff screws using the model. ?

Please suggest easiest way.

Regards
Abhishek

[paulvdh]

In KiCad mounting holes are regular footprints, so you treat them as such.
You start by placing mounting holes on the schematic. There are two versions. One version without a visible pin, and one with a visible pin.

For the footprints there are many more. There are footprints for different sized holes, footprints with and without circular copper pads, and even footprints in which the copper rings are connected with a bunch of via’s to make them stronger.

After assigning the footprints in the schematic, they show up on the PCB after [F8] and you can place them in the right location. You have to check the datasheet of tje jetson-nano for that.

After you’ve made one such module, you can make a template out of it, so you can re-use the PCB outline, connector & hole placement in other projects.

[Abhishek_bhatia]

Thanks for your response. I have idea about the placing mounting holes inside a schematic and then assigning them a footprint. But in PCB layout, the mounting holes should be placed at correct location, and for that I have to work on calculating the exact coordinates of mounting holes on SOM. But as I have proper 3d model of nano, is there any way I can utilize that model to place the holes at correct position?

Hope you got idea about what I want.

Thanks
Abhishek

[paulvdh]

KiCad has “magnetic points” that can snap 2D graphics to other 2D graphics, but not to 3D models.

I would start with modifying your 3D model in some CAD program, and export it as DXF. KiCad can import DXF and you can use such a drawing directly as a PCB outline for example, by placing the graphics on the Edge.Cuts layer.

You can then also link your 3D model to a KiCad footprint, and visually inspect if the mounting holes match. Mounting holes for screws usually have a quite wide tolerance. I believe a standard hole for an M3 screw is 3.5mm, and with KiCad it’s easy to get much more precise when you zoom in.

If you know the coordinates, you can also hover over a pad and then press e for edit and directly enter coordinates.

With: Pcbnew / File / Export / Step… you can also export your project as a 3D step file, and then load it in some mechanical CAD program. You can design a housing there, or just use it to check if things fit together.

[cflin]

I would start with modifying your 3D model in some CAD program, and export it as DXF. KiCad can import DXF and you can use such a drawing directly as a PCB outline for example, by placing the graphics on the Edge.Cuts layer.

Why not use @maui 's excellent StepUp script, which “marries” KiCAD to FreeCAD? FreeCAD is a very powerful open-source 3D mechanical CAD. @maui has posted detailed videos that show how to push-pull from/to KiCAD to/from FreeCAD. StepUP is a FreeCAD add-on script. What makes KiCAD and FreeCAD so powerful is their respective ecosystems, enabled by their open-source nature.

[SembazuruCDE]

What I would do is create a custom footprint for your module that includes the normal footprint for the connector as well as the mounting hole locations. That way if you need to nudge the connector (for example) 1mm to the right you don’t need to remember to also nudge both mounting holes 1mm to the right as well. Size the footprint courtyard to the connector to allow placing components under the module w/o DRC squawking at you. Obviously vertical clearance is up to you.

Hmmm… interesting thought, I haven’t experimented with this idea… Would KiCAD understand multiple enclosed shapes on the courtyard layer? I.e. using this as an example, if there was a rectangle around the connector and two circles around each footprint, would KiCAD understand and allow components inside the bounding box of the full footprint as long as there aren’t any violations with the 3 courtyard areas? Or would multiple enclosed areas in a single footprint’s courtyard layer confuse KiCAD? (I’m asking about 5.1.x here, but if the answer is different (or is planned to be different) in 5.99 please also advise.)