Hi all.
needing some help.
i have converted a picture into a component. but in the board layer outline option there is non to make it into a f.paste. i am making a card and want to add my qr code onto it and will come out gold once made. but only way i can find to do it is by selecting the individual dots and turning each one to f.paste in footprint editor, if i select the whole logo the options tab goes. how can i easily convert it into a f.paste instead of silk?
steve
There is a QR code generator wizard in the Footprint Editor.
Footprint Editor / File / Create Footprint / 2D Barcode QRCode
Very recently a bug was discovered (and fixed) in the QR code wizard, but it does not affect everybody. It depends on locale. If you get bitten by this bug:
Also:
KiCad V5.1.7 is being released right now. For Windows apparently already last week, For Linux I expect it in a few weeks or so, and this should have the bug fix in it.
Wouldn’t you need (*) to modify the mask layer for that instead of the paste layer?
*) I assume by ‘gold’ you mean ENIG (https://en.wikipedia.org/wiki/Electroless_nickel_immersion_gold).
My previous post probably will not help much.
You already have a QR code, no need to generate a new one…
That said.
I’ve grabbed some B/W clipart from some random website, then use bmp_to_component to transform the “.png” into a “.kicad_mod”, put it in a library, placed it on a PCB and am now trying to change the layer from F.Silk to F.Paste…
But anyway.
A simple workaround is to do it with a text editor.
Just open your “.kicad_mod” file in a regular text editor and do a search & replace for: “( layer F.SilkS)” to: “( layer F.Paste)”
Including the parentheses, “layer” text and spaces and such in the search reduces the chance of accidentally replacing other places where that text is used. I was not too careful, as I only did it as a test, but if you do it for real, then first make a backup of your files, then check carefully what you replace.
Longer strings give more security agains accidentally replacing too much.
A string like: “)) (layer F.Paste) (width 0.01))” may work even better.
A completely different question is why you want to place this on F.Paste?
Solder paste is yucky stuff.
I think your intention is to have the whole PCB coated with ENIG, and then make cutouts in the solder mask, to make some parts shiny.
For this you want F.Mask, and the Bitmap to Component Converter can already export directly to “Front Solder Mask”:
Hi. thanks for the help. yes you are correct is saying i want the text and qr code gold against the black solder mask. so just having it set so solder mask is the write way to do it then? cheers
Yes, you create pads which will be ENIG plated (so you need copper there and a no solder mask there), but have no solder paste applied to them (no paste layer), so they are not being covered with solder.
For a bit of inspiration.
The picture below is made with a regular PCB process. Copper, Solder mask and Silkscreen, but you have to stare at it a bit to realize that.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.
