I have added the footprint information to various components in Eeschema (e.g. added sm0402 to a resistor).
A purple label then appears indicating that a footprint has been assigned.
Is there anyway of globally turning the visibility of the footprint fields on or off so I can choose to view or not view all the little purple labels?
I don't know the direct method, but you can manually modify the text file *.sch (remember to backup before modifying). For every component, there is a record in .sch file, and the footprint field is normally field number 2, e.g:
$Comp
...
F 2 "Name" V 10000 2500 50 0000 C CNN
...
$EndComp
the value of 0000 near the end indicates that this field is "visible", and you need to change this to 0001 ("invisible")
How? by regular expression. I used the following command in vim:
:%s/^F 2\(.*\)0000 C CNN$/F 2\10001 C CNN/
you can try sed or any kind of text-processing app to do it.
Source: http://en.wikibooks.org/wiki/Kicad/file_formats#Description_of_a_component
:%s^F ${i}... as this darned option in KiCAD caused ALL fields (including datasheet, part number, vendor, etc) to become visible. Very frustrating.
\$\endgroup\$
if you back-import footprint information into a schematic in eeschema, first you are asked: Do you want to force all the footprint fields visibility?
if you answer No (because you DONT want your footprints to become visible) you may end up with a lot of visible footprints, because they were already visible but they were empty, and you have not changed their visibility.
If you answer Yes, it then asks (in a new dialog box): Do you want to make all the footprint fields visible?
you can choose No, Cancel, or Yes. Choosing No makes all footprints invisible, choosing yes makes them all visible.
This is very confusing.
After creating the schematics, use cvpcb to assign footprints to components. there is a small icon on the menu bar of cvpcb named 'create export file'. this creates a .stf file . save this in the project folder. open the schematic once again, click on back annotate component foot prints. dialogue appears offering visibility option for foot prints. select yes, and all the foot prints become visible. If you want to make them invisible, click on back annotate again, and choose no.
this is for KICAD 2011-5-25 build on 32 bit GNU/Linux.
This is a simple solution to edit the footprint filed or change its visibility : Move the cursor to the field you want to change and right click on it or press F, a pop up menu appears where you can edit the text or make it invisible.
Happy kicad footprinting.
In order to hide footprint field in multiple schematics files, I ended up running this script in the project's folder:
sed -i.bak_sch 's/^F 2\(.*\)0000 C CNN$/F 2\10001 C CNN/g' *.sch
It makes a backup (*.bak_sch) of any *.sch file in the folder and set the footprint visibility field to hide.
Unfortunately, the old way using the text file doesn't seem work as well in the new schematic format (basically because there is only a entry for "hide" and none for "show"). But current versions of KiCad's Schematic Editor (I'm using 6.0.6-3a73a75311~116~ubuntu20.04.1) has a "Change Symbols..." entry under the Edit menu. If you select a component then launch this dialog, you can mass-hide some fields for that kind of component.
You can bulk edit the text and graphics properties (including visibility) by using the Edit->Edit Text and Graphic Properties dialog box. Simply select the "Scope" i.e. which items you wish to modify, and then toggle things such as Visibility on or off as desired. In your case, you wish to modify the Footprint label visibility, so you should select "Other symbol fields" and then fill in "Footprint" under "Filter other symbol fields by name" and then deselect "Visible (fields only)". You can also toggle things like bold/italics and text sizes. I'm surprised none of the other answers mentioned this dialog as it meets your requirements perfectly (perhaps it is a new feature in KiCad 6?)
KiCad 7:
