I mostly do SMD. But I have a board design I am working on for some test equipment that they want DIP parts, so it will be easy to replace if something blows up.
My first try was to just do the DIP parts, and ignore the sockets. But the 3D view that they import into solid works does not look like what they build. Because it does not have the sockets.
Ideally I would like the 3D View to have both the sockets and the DIP Parts. But I am pretty sure that is not possible.
The next best would be to just have the sockets. The schematic uses the part symbols, but the footprint is the DIP socket. That is acceptable for the 3D Board drawing because that is what the board looks like when it comes out of soldering.
But now I have the BOM with the DIP Sockets.
How can I add the actual DIP parts? I was thinking of U1 for the socket, and U1X for the DIP part to go into the U1 Socket.
I know I can always add the parts to the BOM after I generate the BOM but that seems clunky. Is there a better way?
Is there a preferred or standard way to indicate DIP parts and DIP sockets, so they both show up on the BOM?
Right now the only way I see is to add the part and âExclude from boardâ. Is that how you do it?
I have started using two different footprints for DIP parts. For example, one 8-pin DIP footprint will show a STEP file with only the device placed for PCBs without sockets. A second 8-pin DIP footprint for the same part will use a STEP file showing a socket with the device installed in the socket so the skyline of the PCB is correct for those PCBs that require sockets. The footprint with the socket will have âW_SOCKETâ appended to its name.
However, I have to remember to manually add the sockets to the BOM. So far this process has been the best that I can come up with that is manageable across most projects.
Create a footprint for the socket with no actual pins. Maybe some silkscreen that says âinstall socketâ or some such. But importantly, no courtyard. Add appropriate 3D model.
Footprint for part is normal again, except that the 3D model has a Z offset to lift the model high enough off the board to allow the socket to fit underneath.
Both parts on schematic, both on the board, and both in the BOM.
Make sure that the origin for the footprints for the socket and part are in the same relative position for easy positioning on the board. They can âsnapâ to eachother.
Not long ago on the like this question someone said something that my reaction was: âA person learns all his lifeâ. He just said that you can add to one footprint more than one 3D model.
This of course not solves the problem of having both in BOM and I didnât tried his way.
I use one two-part element. It is shield made of frame and lid. I have two rectangles at schematic (one inside the second one, and one grounded) so I get two elements in BOM. My frame footprint has lot of pads (all with the same number) and lid footprint has 0 pads.
For the BOM it may be beneficial to put 2 footprints, socket and chip, on eachother. It is not pritty and will yield DRC errors.
The schematic would also need both elements. That would not be pritty either. Although you can âfixâ the schematic by making schematic sheets for each DIP IC. In the sheet you can simply put both IC and socket symbol. And your main sheet will still look okay.
I would however simply either make a new footprint with both 3D models (for re-using) or edit every footprint in the board to have both 3D models. And edit the BOM manually
If a librarian read this. Perhaps it is a good idea to add both 3D models to the same component. In the event that a user would need an IC socket, He can simply check the visible box for the socket, and manually raise the IC itself. Anyways just a brainfart.
I usually have a separate page in my schematic for all things non-electrical, like mountingholes, fiducials, company logo, etc.
Symbols for the required sockets could well go there, with the âExclude from boardâ attibute set. That way they donât clutter the schematic, but do end up in the BOM, and youâd have no DRC worries. Of course, the parts to be socketed would have to have a footprint that includes the 3D model for the socket, as descried above.
Following with interest since I face a very similar issue - an MCU (Teensy 4.1) which sits in a pair of SIL sockets. The space between the MCU and the main PCB is also used for some components and connectors. So it would be good to render a view with just the sockets, and also be able to render the view with MCU installed.
For a module with two sip sockets, I have been using freecad to import the single sip socket twice into a part, and export that out as a new step file for kicad.
I have now noticed that it does not need to be that complicated, since the kicad footprint editor 3d model tab lets you add more than one step file and adjust position/rotation of each individually. So making a two SIP part 3d model is actually pretty easy. Will still be a single line item on bom.
Adding the actual module as a separate part (I just have a little box on the schematic and footprint) works well to get the module on the bom and allow dragging it wherever you want on the pcb before a 3d render. Raise the module in Z to the plug-in height.
Thanks for that! But, like the Teensy 4.1 model and footprint I have, it is for the MCU soldered direct to the main PCB. So it gives an impression of the overall look in a socket, but not an accurate model.
