Make a previous project into a "daughterboard"

[Moriambar]

I hereby certify that I am not simply asking someone else to design a footprint for me.

Hi, I recently printed a pcb created with kicad. This has basically one connector (2 pin header) and a mounting hole. Let’s call this “mymodule”.
In a future project I will possibly need to include this functional block, basically reserving the space for the header and mounting hole (stacking mymodule on top on the latter project pcb). Is there any way to kind of “import” the mymodule position for headers and mounting hole (as if it were a footprint) whithout doing manual measuring on the mymodule pcb project?

Cheers

[johanh]

I’m not aware of a direct “import” like that (correct me if I’m wrong). But you can copy parts or complete schematics/boards from one schematic to another and from one PCB editor project to another by selecting and then just copy/paste. Be sure to not have conflicting component numbering in the schematic. Then it’s a little hit and miss when making sure that components stay in place when doing the Update PCB from Schematic. You can adjust options in the update dialog before doing this. Take a copy of the project first and remember to save. Maybe there is a better way of doing it, but this is what I have done for some small things.

[RobK]

This is just a (possibly stupid) idea, but I think exporting your ‘mymodule’ to dxf, then importing it in the Footprint Editor might work.

[paulvdh]

You can simply open two KiCad instances, each with their own project, and then use copy and paste to copy sections from one project to another.

[bertrand_meneroud]

In kicad V8 (I don’t think that it was possible with previous version), you can copy the PCB of your module and past it in the footprint editor.
So you can easily create a footprint for your daughter board.

[eelik]

@bertrand_meneroud

you can copy the PCB of your module and past it in the footprint editor.

This is a working solution, but it has a bug: Copying footprint from board and pasting it to footprint editor mirrors graphics (#17518) · Issues · KiCad / KiCad Source Code / kicad · GitLab.

From the original board copy the footprints and graphics you need for creating the new footprint. “Disassembling” footprints before selecting isn’t possible, so you have to delete superfluous items after pasting in the fp editor. Then you can of course modify the pads and graphics to be suitable for the new footprint. Most probably you want for example the old edge cut to become the new fab layer outline.

[Moriambar]

thanks, but shouldn’t I include the symbols in the schema as well?

Cheers

[BlackCoffee]

Daughter Boards are easy - When you have the Board designed as desired, use the StepUp Workbench (in FreeCAD) to load the Board, Load the Pads/Traces… Then Export as STEP. Now, you can use it for a Footprint…

(Loading into StepUp will load the parts/footprints, too…

Examples

[Moriambar]

thanks this seems like a solution, I’ll have to fiddle arounf though 'cause I never have used the freecad feature of kicad nor am familiar with this procedure. Any suggestions on where to find docs or help to learn it?
Cheers

[BlackCoffee]

@Moriambar

Any suggestions on where to find docs or help to learn it?

There are plenty of posts and YouTube videos on making Footprints.

A Daughter Board (STEP file of it) is no divfferent than a a STEP file of a Transistor/etc wherein you (User) creates a Footprint and associates the STEP file with it.
STEP files can be created with many software’s and can also be downloaded from various sites.

Also, there are plenty of YouTube videos on using StepUp…

This Video may help with respect to loading in StepUp…

[jakketet]

Tried that on Mac but doesn’t work… No way to open a second instance, you CAN open a second (or more) Schematic(s) and/or Pcb(s) but NOT a real 2nd Project or I missed something(?)
Would be nice…

Version: 8.0.1, release build
Platform: macOS Ventura Version 13.6.1 (Build 22G313), 64 bit, Little endian, wxMac

[paulvdh]

I have been able to open multiple projects (Each in it’s own KiCad instance) for quite a few years. Probably since KiCad V5.

[Moriambar]

I’ll try, thanks. The video is ok, I’ll search in youtube 'cause I don’t understand the process (never used any cad software apart from kicad).
Cheers

[Moriambar]

ok clearly the freecad way is not the correct one. I think I’ll create a new symbol and try and copypaste from the first pcb (daughterboard) the connector and mounting hole in exactly the same spots so that I’ll be able to use them as a daughterboard.
It would’ve been nice transforming my currently pcb in a symbol+footprint too (when needed on the main board) but currently I’m clueless. Unfortunately (maybe due to my little free time) I haven’t been able to find good tutorials to do this on youtube, but it’s not critical now

Cheers

[paulvdh]

I don’t think there is a direct way to transform a PCB / project into a footprint in KiCad. What you can do is export various parts of the PCB, create a new footprint, and import those parts into your footprint.

It may help if you start by posting at least a screenshot of what your PCB looks like.

[BlackCoffee]

@paulvdh

I don’t think there is a direct way to transform a PCB / project into a footprint in KiCad.

@paulvdh, I think you’re incorrect…

@Moriambar
Do This (Everything is done in Kicad, Not using and other software)

Example:

Say the goal is to Create a DaughterBoard-PCB and Mount it onto a real Project’s PCB

• Step #1: Create a Real Project

• Step #2: Create a PCB to use as a DaughterBoard (DB)
Therefore:
• Export this DB from Kicad as a WRL
• Make a Footprint for it and link it to the WRL

• Step #3: You want to place the DB 30mm above the Real project’s PCB and you’ve located a STEP file (or, WRL file) of a Riser-Post to mount it to
Therefore:
• Make a Footprint for the Riser-Post and link it to the STEP or WRL

Now, you have:
• A Footprint of the DB
• A Footprint of the Riser-Post
• A Real Project you want to use the DB and Riser-Post in

• Step #4: In the Real Project, place the Footprint’s of the DB and the Riser-Post

Notes: You’ll need to assess and determine the Placement, Offset and Scale (WRL’s will most likely need Scaling/Setting)

I did the Above steps and, for the Real project, I created a dumb PCB for this Real Project’s example and Placed the DB and Riser Footprints…

NOTE: I did Not bother to Scale or Align stuff for this quick example. Full process took about 5 minutes.

ADDED: Oh, for the DB’s footprint, I copied the PCB’s Edge-Cut shape and pasted it into the Footprint and changed layer to Front-Silkscreen

The Footprint Scaling for the WRL (if using mm in the export panel), is 0.3904

[eelik]

I’m not surprised at all this feels complicated. After all, this involves symbols, footprints, 3D models and two boards. Additionally, the relation of the two boards isn’t necessarily clear in general case. If there are only two boards, how to call them and which one is actually the more “basic” one? The bigger one, or the one having more powerful MCU controller, or the one which has been designed first, or the one which is attached to different kinds of boards or to which different kinds of boards can be attached? Which one actually defines the physical connection? In this case it looks clear enough, though. But because the OP doesn’t know how exactly to ask, even the seasoned KiCad users confuse the actual problem – and I don’t still know what the OP needs to know.

First, we have a board which already has the connector and the mounting hole (B1). The connector and the hole are there as footprints. If I have interpreted correctly, the OP needs to have those same connector and mounting hole pads in the same location in another board (B2). At least that’s how I interpret the question,

@Moriambar

Is there any way to kind of “import” the mymodule position for headers and mounting hole (as if it were a footprint) whithout doing manual measuring on the mymodule pcb project?

I don’t see a mention of a 3D model there, and the question of a symbol is brought up later.

There are two options for this, and those two answers have already been given. Which option is better depends on several details. Do you want to possibly reuse the B1 in several projects? Do you need a 3D model for the combination? Which one comes to top, which one to bottom?

If you ever need only this one B2, it may be enough to have two projects side by side opened in different KiCad instances and copy the connector and mounting hole footprints from B1 and paste them into B2.

If you want a reusable B1, it would be better to make a footprint which represents it and which can be used in other projects. This has also been described: copy the needed footprints and edge cuts from B1 and paste it to a footprint in the footprint editor. Then add that footprint to B2. If you need 3D model to see the combination, export B1 as a STEP model and attach it to the new footprint.

For creating the schematic for B2 you need a symbol or symbols which represent B1. That should be straightforward because there’s only one connector in B1 for this connection. Even a standard KiCad connector_generic symbol with correct amount of pins is enough. Attach the new footprint to it, and remember that the symbol pin numbers and the footprint pad numbers must correspond.

So, you first should understand your own needs better and communicate them to us better. Then we can tell which solution is the best, and how to continue with details.

[paulvdh]

@BlackCoffee

@paulvdh, I think you’re incorrect…

Why?

@BlackCoffee

• Make a Footprint for it and link it to the WRL

@BlackCoffee

• Make a Footprint for the Riser-Post and link it to the STEP or WRL

What steps do you take to “Make a footprint”?
Exporting a 3D model of a PCB is not the same as making a footprint.

[BlackCoffee]

@Moriambar

Is there any way to kind of “import” the mymodule position for headers and mounting hole (as if it were a footprint) whithout doing manual measuring on the mymodule pcb project?

@paulvdh

I don’t think there is a direct way to transform a PCB / project into a footprint in KiCad. What you can do is export various parts of the PCB, create a new footprint, and import those parts into your footprint.

I suppose “a direct way” could imply to some users that nothing should be required beyond just a single click but, to ‘me’, a direct way implies using the embedded Kicad Tools/Resources without a lot of hurdle-jumping.

And, Exporting a single WRL yields All the Parts, Pads/Traces so, no need to export individual Parts/items.

Thus, if a User has created a PCB (of even ‘only an Edge-Cut layer rectangle’ without any parts on it) then,
File>Export>vrml… produces a WRL that can be linked to a Footprint.

That Footprint can be nothing more than a Silkscreen (other) of a Rectangle (for example).
In the Video example, Step #4, the Small Rectangle is all that I placed first and is all that was needed. And, the only reason I used that was to yield a visual of having a placed footprint (otherwise, only the ‘Ref’ and name would be shown, (if visibility enabled).
I added the Daughterboard-PCB’s shape only to make it more clear visually (to Users).

The Footprint was done in the usual way: New Footprint, added the Silk (mentioned) and linked to the WRL. Done and Simple.

The Footprint - Worth mentioning: The Image-Converter Tool Creates&pushes out a New Footprint, so a User can create a very simple drawing (or a Screenshot of the PCB) and use the Image-Converter tool to create the Footprint so, it this sense, Kicad does have a direct way to Create a Footprint of the PCB. That image can also be used for the Front Silk…etc. User just needs to Link the Footprint and WRL.

The Footprint for the Riser Post - also simple, just a Circle on Silk layer and linked to a STEP file.

@Moriambar , No measuring of Parts, Headers… need to only place Origin, Re-Set the Cursor/Grid X/Y readout (press Spacebar) at bottom of Window to gain info of where Holes/Parts/Item’s are with respect to where User sets the Grid origin (spacebar) and where Cursor is currently pointing.

And: User can get the Positions of items/contents from the ‘File>Fabrication Output>Component Placement’ file

From Image Converter… (I used a Screenshot of the Step #4 )

[maui]

just for reference there was a thread about this subject:

Is there a way to convert whole PCB in new footprint?

Hi everyone ! I’m wondering if there is a way (or magic tool ^^) to make a new footprint from a PCB file ? In my case, i’m doing a small PCB which will be plug on others biggest PCB (like mother board). It’s easy to make a schematic symbol, but when I’m face to drawing the footprint… but since I designed the PCB of my small card, with all pads at right position, is there a way to transform the PCB file into a footprint ? I think we have to use only pads and edge cut layout which will give us …