Modify a footprint

Layout
1

I am at the final stages of my pcb. There are a a few footprints with too much paint and I would like to modify them. I get to the existing footprint in footprint editor. I make a small change. How do I save this edit and get it to appear in pcbnew? Thank you.

2

Use the ‘Insert footprint into current board’ to get it into your current board. If you want to keep your changes to re-use the footprint, you will need to save it to a personal library.


(nightly screenshot)

1 Like
3

John,
When I open Footprint Editor, I see the component and "Footprint Editor(no active library) at the top. Also the insert footprint into current board looks like a grayed out 8 pin component.
What am I doing wrong?

4

I just tested the modify footprint stuff in kicad stable 4.0.6 on linux. It should work the following way:
In open gl:

  • Either press ctrl+e while above the footprint
  • Or select open in footprint editor after right clicking
  • Or use the Edit in footprint editor button in the footprint properties dialog (press e do open this dialog)

This opens the footprint editor with your current footprint extracted from the board.
Do your changes and use the update footprint on board button to get the changes back into the pcb file.

If it does not work this way maybe give us a bit more details about your installation (Kicad version, operating system)
And about the changes you are trying to make. (Maybe some changes can not be made this way.)

2 Likes
5

Thank you. It works well.

6

Here is how I solved the problem, after rather long time of confusion:
0. Create a project to create a board with only my custom footprints
2. Places existing versions of the components I know I will need. (1 diode, 1 resistor. one 8-pin DIP, 1 capacitor with radial leads, etcetera…
2. Open File->Archive footprints and Select “Archive footprints”->“Create library and archive footprints”.
3. I chose the nickname “Footprints” because it is my personal library and also it is already located
4. Look in the project folder to find a new folder called Footprints.pretty. Each file in this folder represents a footprint.
5. Now start the footprint editor by pointing at a component (the middle cross) and then pushing ctrl-e
6. Do some change in the footprint.
7. No change visible on the board.
8. In the footprint editor, above the black window, there are several icons, looking like circuits. You have to hover over all these icons to find the one having the help text “Update footprint in current board”. Do not confuse it with the icon “Insert footprint in current board” (which is greyed out for me). Push this button.
9. Still nothing happens on the board (pcbnew).
10. Close the Footprint editor.
11. Still nothing happens on the board.
12. Repaint the screen in pcpnew (F3 or look under the view menu).
13. Yippee. The changed footprint is now visible on the board.

7

This works for one instance, the other parts have still the old footprint. If I have a dozen parts of the same type, how do I update all parts with a changed footprint?

8

If you need to modify a footprint for multiple instances (or for all of them) you really need to do this at the library level.

  • This means open the footprint editor from the kicad main menu
  • load your footprint,
  • do your changes,
  • save the footprint to a fitting lib (see note 1)
  • And either assign the newly created footprints from within eeschema (via the assign footprint tool formal known as cvpcb)

Note 1: (what is a fitting lib)

  • If the footprint is in one of your personal libs and the change should apply to all future projects that use this footprint then overwrite the existing footprint. (use update footprints from lib feature to update the footprints in your schematic. In kicad 4 this was hidden in the change footprint option)
  • If the original footprint is part of the official kicad libs then you should store the modified version in a personal lib of yours. (otherwise an update of kicad will overwrite your changes) This means you need to reasign the footprint in the schemaitc
  • If the footprint modification is special for this project i would suggest to add a project footprint lib (place it somewhere in the project folder, add it to the local fp-lib-table) This again means reassigning is necessary.
1 Like
9

Sometimes it is really much easier to “see” the needed changes and clicking “Ctrl+e” brings up the editor without all the extra navigation.

The problem with doing it this way is that it brings in the actual Ref Des text. U5 (for example) will have to be edited back to “**REF”. Then the Footprint does need to then be saved to a fitting library.

And, the Footprint can also be pushed into the board with the “Update footprint into current board” icon. At this time the changes can be visually seen on the board and approved, or the process repeated.

Then all similar Footprints can be updated by editing one of them and updating from library.

With V5 it seems that this step by step process keeps the F.SilkS and F.Fab layers text locations intact (I have not yet tested going all the way back to Eeschema, but I suspect it may not work as neatly).