# 'Footprint Field' visibility options in Eeschema (Kicad)

I have added the footprint information to various components in Eeschema (e.g. added sm0402 to a resistor).

A purple label then appears indicating the that a footprint has been assigned.

Is there anyway of globally turning the visibility of the the footprint fields on or off? So I can chose to view or not view all the little purple labels.

• Unfortunately, there is no way of doing that as far as I know. Off-topic; Why are you putting sm in front of 0805? – abdullah kahraman Feb 11 '13 at 17:41
• @abdullahkahraman: It might stand for "surface mount" - but yes, it's not necessary. – Chris Laplante Feb 11 '13 at 17:42
• The 'sm' prefix is because the default/distributed Kicad footprint/'land pattern' library calls them sm0402 or sm0603 etc. This way the correct footprint will be used when laying out the circuit. – Senthil Seveelavanan Feb 11 '13 at 18:07

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$/F 2\10001 C CNN/  you can try sed or any kind of text-processing app to do it. • Thank you. This was very helpful. I ended up making a shell script that looped over :%s^F${i}... as this darned option in KiCAD caused ALL fields (including datasheet, part number, vendor, etc) to become visible. Very frustrating. – Cloud Nov 2 '14 at 17:46

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.

• I'd like to point out that in the newer versions of KiCad, where you don't use CvPCB to make the associations, you can still export them from pcbnew (File/Export/Component (.cmp) file), and then reimport to eeschema. This way you don't change any of the associations, but you get to change the visibility. – Timo Mar 24 '16 at 11:07

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.

sed -i.bak_sch 's/^F 2$$.*$$0000 C CNN\$/F 2\10001 C CNN/g' *.sch