Reloading Footprints in PCBNew


Is there a way to get your layout file to pull footprints once they’ve already been placed? I have a layout I’ve created and finished and I’m now adding 3D models. I’d like to update the footprint and have the parts on the layout update automatically. As it stands, my work around is to delete the footprints and reread the netlist, but then of course you must replace the parts.

1 Like

To add 3D models, all you should need to do - in pcbnew - is edit the footprint (hover over the footprint, not the pad, and press ‘E’) and go to the 3D settings tab. Here you can add the 3D model.

Alternatively, you can add the 3D model in the footprint editor. Hover over the footprint and press CTRL+E and then follow the same steps as outlined above.

There should be no need to re-read the netlist for 3D models. In case you meant change out the footprints, then you can either - in eeschema - run the schematic through cvpcb to assign new footprints, then re-create the netlist and re-import that in pcbnew. Be sure to check the change footprints box.

Alternatively, you can embed the footprint property in the component, by editing the component (hover over and press E), click the footprint field, click the assign footprint button and then choose your new footprint. Don’t forget to rebuild the netlist.

In either case, there should be no need to delete any footprints on the pcb! I hope this helps.

1 Like

Hi Jules,

Say I have 7 identical parts, say diodes, on a board. Currently, if I add a model to one of them, the rest of the parts do not update to reflect the new change. I would like the rest of the footprints to update after the change. Can we accomplish this? This is really the heart of my question, I apologize for not being too clear.

1 Like

Ah, I get your issue. I guess that is related to the fact that you’re trying to edit the current footprint, and thus you’re only changing this property in that single footprint. You should create a new footprint from your desired new component with the model added, and then exchange the footprints via either pcbnew or eeschema/cvpcb. The ‘change footprints’ option in the footprint properties dialog in pcbnew can be helpful here aswell.

If the footprint you’ve created has the model info, you should be able to link that footprint to the required components in the schematic (either via the component properties, or cvpcb), then export a new netlist and load that in pcbnew so that it will know to use your footprint with model.

Maybe my explanatory skills are just not up to par, but you should be able to get there :wink:

Thanks Jules, I’ll try that. I may also submit a request to add a “re-pull
footprints” button to the developers.

1 Like

Change the footprint in the library.
Edit Footprint parameters/properties -> Change Footprint(s)
Select “Change same footprint” or “Change all”


This is exactly what I was looking for. Thanks!

Unfortunately there is no similar function in the Schematic! I am waiting for this to be added.

I have the same issue as you, I am updating footprints and adding 3D models and need to delete the footprint and re-read the netlist to get the updated footprint to show, Then the footprint needs to be moved back into position…

@NikB Thanks for the tip! I wish that button wasn’t buried and was more exposed in the menu ribbon.

@Jules Can you explain better how to “embed the footprint” into the component. I tried to do this via the component editor and it only gives a footprint filter.

In eeschema, edit a component’s properties. In the middle you will see all the fields and values associated with ithe component Click on the ‘Footprint’ field (probably is empty), and in the bottom right there should now be an assign footprint button. Click on that, select your desired footprint and presto! I guess this is the same thing cvpcb does, but only slower.

You might want to change the visibility of the footprint field (also on the right-hand side of the properties window) so your schematic won’t get cluttered up with unnecessarily long footprint name fields.

1 Like

Would it be possible to give some details on how to “embed the footprint in the symbol IN THE LIBRARY”. I have spent some time going through the library management windows and I can’t seem to find how to do this. While I’m at it, if anyone can help on some other questions, it would be appreciated. Using the method of updating footprints by editing a footprint in PCBNew took a very long time to find, and each time it takes me 7 mouse clicks to do; is there any more efficient way? Could this operation be included in a Toolbar, or if this is not possible, in a menu?

  1. Help: in PCBNew choosing help states the help file in states /usr/share/doc/kicad/help/en/pcbnew.html states AbiWord can not open it as it is the wrong format. Yet running xdg-open /usr/share/doc/kicad/help/en/pcbnew.html opens it fine in Chromium. Why is AbiWord being used, and how can one change the command to use a different browser that works?
  2. When starting a new board, choosing Net in PCBNew brings in all the components on top of each other and it takes a long time to separate them before placement can start; is there a better way to do this? For example, DipTrace has a menu item Place from List … or something like that.
  3. When the Keyboard shortcut window is visible, PCBNew doesn’t function properly; is there a way of leaving this window open while still using KiCad?
  4. Can a pour be done that automatically aligns to board edges? My board is irregular with rounded corners and trying to draw an accurately aligned pour by hand is problematic.
  5. Could File->Plot be changed to something a little more intuitive for exporting manufacturing files. I would prefer File->Export, but something like File->Manufacture_Files would be okay.
  6. In eeSchema, I got into real trouble putting GND components connected to other components without an intervening wire; this really made getting the Electrical Rule Check to pass. In addition, often power supplies come from header pins; one really does not want to have to customize the Header Component in the Library to specify pins a Power Outputs; is there a better way to do this.
  7. Finally, can someone point me to KiCad->FAQ? Not sure why, but I can’t find a link to this from any of, or, or even

Would had been better to open a new thread, especially as you got so many questions there…
What KiCAD version are you using?

for your footprint assignment:
…PartLibraryEditor > [FieldProperties] button (big black T) > FootprintField

updating footprints? What is your aim there? What do you want to do?
…if I want to update footprints in pcbnew I hover the mouse over it, hit [E] and then click on [change footprints] and then select if just this one, all similar or all on board and hit [Ok]… that’s like 3-4 mouseclicks

space footprints at start:
… search for the [Mode Footprint] button (white/green chip with arrows on top) in pcbnew, click it, then right click anywhere empty and take your pick in the menu… once done, deactivate [Mode Footprint] again

zone fills:
… just draw the zone so it covers everything, the fill will take care not to fill where there is no pcb :wink:

get used to plot, it’s 99.5% going to stay as is :wink:

anything not mentioned is to unspecified for me to answer… good luck.

I also would have liked a simple refresh.

I define the foot print in schematic on the symbol but if I move the same footprint to another library and the update the schematic to reflect this move A:Y -> B:Y you get a warning in pcbnew when you load the netlist, but he doesnt follow the netlist !!!
what ?, is not the netlist the master ?
He notices the change but chooses the ignore it.
trying to fix this you end up with a bunch of artifacts in your footprint and you need to delete and reload netlist to get it in fresh,

many strange things going on 4.0.1 stable