8
\$\begingroup\$

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?

screen shot

\$\endgroup\$
3
  • \$\begingroup\$ Unfortunately, there is no way of doing that as far as I know. Off-topic; Why are you putting sm in front of 0805? \$\endgroup\$ Feb 11, 2013 at 17:41
  • \$\begingroup\$ @abdullahkahraman: It might stand for "surface mount" - but yes, it's not necessary. \$\endgroup\$ Feb 11, 2013 at 17:42
  • \$\begingroup\$ 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. \$\endgroup\$ Feb 11, 2013 at 18:07

7 Answers 7

6
\$\begingroup\$

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

\$\endgroup\$
1
  • \$\begingroup\$ 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. \$\endgroup\$
    – Cloud
    Nov 2, 2014 at 17:46
5
\$\begingroup\$

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.

\$\endgroup\$
1
  • \$\begingroup\$ 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. \$\endgroup\$
    – Timo
    Mar 24, 2016 at 11:07
1
\$\begingroup\$

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.

\$\endgroup\$
1
\$\begingroup\$

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.

\$\endgroup\$
1
\$\begingroup\$

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.

\$\endgroup\$
1
\$\begingroup\$

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.enter image description here

\$\endgroup\$
1
\$\begingroup\$

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?)

Edit Text and Graphic Properties dialog

KiCad 7: enter image description here

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.