I have recently transitioned from using OrCAD to KiCAD, and am currently on version V7.0.9. I am in the process of designing a Footprint for a Mounting Hole. To help you understand the specific Mounting Hole I am trying to create, I have attached a picture with this message.
In KiCAD’s “Footprint Editor,” when creating a PAD, it seems that I can only set the shape or size of the Drill Hole, and the shape or size of the copper/Solder Mask PAD. However, I would like to design the shape/size/inner diameter/outer diameter of the copper/Solder Mask individually and differently. Is there a way to achieve this? If so, could you please provide a detailed explanation on how I can implement this?
designing solder mask (also for solder paste) individually:
turn off the automatic “solder mask” creation in the pad properties dialog
activate the F.Mask/B.Mask layer
use the graphic drawing tools (line, arc, circle, polygone) to draw any shape you want. Remember that solder mask is a negative layer - every shape you draw will remove the solder mask from the board
if you want to draw a really complicated shape:
the builtin drawing tools are good for basic usage, not really designed for artistic work
you could use a external drawing tool (inkscape, qcad, librecad, autocad, …), save as dxf/svg and import this graphic into the footprint editor (import into the f.mask/b.mask layer)
as the import doesn’t supports all existing dxf/svg features make sure to simplify your drawing before saving
I understood your explanation. But I have a question here. If you look at the photo I attached, there is a gap between the Drill Hole and F.Cu. This area is an area without any layers.
Therefore, there are two problems when drawing as a .dxf drawing and then “loading” it into the Kicad library editor.
I want to fill the F.Cu area (green). After filling the outer diameter of the F.Cu area, I tried to process the inner diameter of the F.Cu area with Anti-Copper, but I don’t know how to set Anti-Copper in the Footprint editor.
When creating a PAD, an error will occur if you set only the size of the drill hole, then uncheck Solder Mask and set the PAD size to 0. The error states that the PAD size must be larger than the drill hole. If you directly handle a PAD of a special shape with a .dxf file, only the Drill Hole must be created when creating the PAD, but this is not possible due to this error.
I use this style of mounting hole myself. I’ve attached a footprint that I just threw together (hopefully close to what you are looking for). A quick overview of how I did it is below, I’m happy to go into more detail if it is useful. (Note that I’m using the nightly v8.0.0-rc2, but I don’t think this process has changed since v7)
I started with a non plated through hole in the center with a hole diameter larger than the pad diameter to remove any copper from that area. This is the actual mechanical screw hole.
Add a graphical circle on the front copper (F.Cu) layer around the hole with a radius in the “middle” of where the eventual pad should be. Set the line width of that circle to some larger value to create a “donut” shape. This step may require some calculation if you have strict rules about how close the mechanical hole can get to the copper pad.
Add a new pad on the front copper (F.Cu) layer, this time a smaller SMD circle pad, that fits within the filled “donut” area of the graphical circle. Move it to a location where it won’t otherwise show on top of the graphical circle.
Select the new pad and press CMD/CTRL + E (depending on OS) or right click on the new pad and select “Edit Pad as graphical shapes”. Select the graphical circle and press CMD/CTRL+E again to exit the pad editing mode. Now the graphical circle should have been combined with the little pad.
Copy and paste the custom “donut” shaped pad and edit the copy to be on the back copper (B.Cu).
Add vias if desired, just a series of normal through hole pads with the same pad number as the existing pad.
Draw a graphical circle on the front soldermask (F.Mask) layer with the Filled checkbox checked to cover the entire footprint. Do the same on the back soldermask (B.Mask) layer.
After opening the FOOTPRINT file you attached, I understood everything you explained. Thank you so much for your active help. Now you can design mounting holes of these complex shapes on your own.
Here, I would like to ask one more question. To draw F.Cu and B.Cu into circular strips, you drew a circle with a radius of 2.54mm from the center and a line width of 1.8mm. Is there a way, other than this method, to draw F.Cu and B.Cu as a circle with a diameter of ø7mm, and then add an area inside the circle with a diameter of ø3mm to prevent the copper foil from being placed?
If I’m understanding you correctly, the answer is no. There is no concept in KiCad of “anti-pads” as they are sometime described in PADS Layout (an alternative commercial eCAD software). You also cannot make fillable zones in KiCad’s footprint editor, so you can’t make a circular copper pour with a circular keepout zone in the middle to do the same thing.
A small tip: numerical fields such as these radius and line width ones support taking simple equations instead of plain numbers.
So in your case you would enter ((7 - 3) / 2 + 3) / 2 in radius, and (7 - 3) / 2 in line width.
The caveat is that it does not remember the equation. So, if you re-edit the circle, you will only see the calculated value. But at least it saves many back and forth between a calculator and kicad .
.