Hi! I have finished a board and would like to include some silkscreen items, but essentially, silk screen should just contain some text items I have manually placed. no Reference designators, no labels, no graphics that are contained inside the footprint´s library such as “outline”.
I found that topic which suggests this should be easily possible
Unfortunately, It does not behave as I would expect in V 8.0.4 (haven´t tested older versions). If I uncheck the “visible” mark, the silkscreen “outline” items all persist on the silkscreen and If I re-enter the shown menu (i.e. " Edit Text and Graphics Properties"), the “visible” tick is checked again.
Edit: All this is a bit complicated, a much simpler method is described in another post below
You can change visibility of text from footprints, but you can not change the visibility of graphics embedded in footprints directly in the PCB editor.
Doing this “properly” is a bit involved / complicated.
One way that is guaranteed to work is:
Export all footprints on the PCB to a project specific library.
Push the links to the new footprint library back to the schematic.
One by one, edit the footprints in that newly created library.
Update the PCB with the new footprints.
This is a bit of work, but it may be not as bad as you would guess at first. You only have to change the footprints, not each instance of all footprints. By changing a single resistor footprint, and updating the PCB, all instances of that footprint get updated.
There are some other methods you can try.
Leave the file as is, but after generating gerber files, swap the file that normally is the silkscreen for another layer. For example, draw your custom silkscreen on the User.1 layer. Renaming files is not enough. Gerber files have a text string embedded in them that defines the FileFunction. And you have to change that too with a text editor.
KiCad’s PCB file is text based. You can close KiCad, then open the file in a text editor, and replace (nearly) all occurences of the silkscreen layer name with another layer. Be a bit careful, there may for example be a table which defines all layer names, and you do not want to change such a table. Changes you made this way will be lost if you ever update the footprints from their libraries.
In PCB Editor / File / Board Setup / Board Stackup / Board Editor Layers you can either rename or disable the silkscreen layers. This may (or may not) help a bit when you attempt either of the two alternative methods.
Be sure to create backups before attempting weird things in KiCad.
Thanks for the detailed response, I will try one or the other method - indeed seems a bit “complicated” but I will try - am not a fan of manually text post processing since that calls for errors, but I will change layer and modify the gerber plotting/generation.
If that is the case then I really wonder about the meaning of the checkboxes of “PCB graphic items”, and “Footprint graphic items” in the “Edit and Graphic Properties” menu, though =)
Put the silkscreen items you want on a user layer.
Suppress the generation of the silkscreen layer when plotting in the first checkbox column.
Edit: I think you need to move all the existing silkscreen items to another layer before the next step.
Plot a second time, selecting only the silkscreen layer in the first checkbox column, and using the second checkbox column Plot on All Layers to select only the user layer.
You will end up with Gerber files where all the non-silkscreen layers are plotted normally, and the silkscreen layer is plotted from the user layer.
Yes but why do I need to move the items to an user layer and cannot use the settings as you have them in the screenshot and unselect the “visible” tick so you can keep the silk screen layer the silk screen layer?
Your solution works, also the one mentioned by @retiredfeline but I just want to understand the KiCAD menu =)
I am not exactly sure. All the other checkboxes under Visible are only applicable to text. (Bold, Italic, Keep Upright, Center on footprint) Also most other options in the Action / Set to specific values panel are also only for text. I checked and the Line thickness works for all graphic lines, but unchecking the Visible checkbox does not work for graphic items. I think this is a bug in KiCad but I am not sure.
This Visible checkbox is on again because it is a generic dialog to change the text and graphic properties. Nothing is changed unless you actually change the status of the text box. If you want the text to re-appear, you have to click on the Visible checkbox twice before you click the OK button.
The Bold checkbox also appears to be broken, I’d have to check that in a recent nightly someday…
Edit: I changed the mark of “The Soltion” from this post to my post above with the screenshot, as I believe it is a more direct answer to the original question. The main purpose for this “Solution” thing is for others who search this forum to find answers quicker.
