Kicad questions

[pucho812]

what does it mean exactly when it says silkscreen clipped by solder mask?
Can I ignore it and if not how does one solve it. It shows as a warning on a few of my footprints and layouts.

 

[ijzerpro]

what does it mean exactly when it says silkscreen clipped by solder mask?
Can I ignore it and if not how does one solve it. It shows as a warning on a few of my footprints and layouts.

https://www.eurocircuits.com/pcb-design-guidelines/legend-print/

 

[ccaudle]

how does one solve it

You should just be able to move any silkscreen text a little farther away from the contact to solve that. Check to see if there are any locations where the text extends into an area without soldermask, onto the exposed copper pad.

 

[pucho812]

I'll investigate further as visibly I don't see that. But DRC should be correct and not throw those flags up.

 

[zamproject]

silkscreen clipped by solder mask?

As already say it's when silk layer overlap a forbidden area (like a pad)

After DRC check you should see arrows on the pcb (red or yellow depending on violation type)
Also in your DRC box/window, by clicking on a warning/violation, the pointer at pcb editor will show the coordinate of it.

 

[pucho812]

As already say it's when silk layer overlap a forbidden area (like a pad)

After DRC check you should see arrows on the pcb (red or yellow depending on violation type)
Also in your DRC box/window, by clicking on a warning/violation, the pointer at pcb editor will show the coordinate of it.

Yes I see that. It's on a custom part for a cinemag transformer. In fact all the warnings are for that one part.

 

[zamproject]

So if it's not the variable text data (Ref, Value) that you can move in pcb editor, but graphic lines for component, you should edit the footprint and clean/adjust graphic element at silk layer.

 

[MidnightArrakis]

what does it mean exactly when it says silkscreen clipped by solder mask?
Can I ignore it and if not how does one solve it. It shows as a warning on a few of my footprints and layouts.

[what does it mean exactly when it says silkscreen clipped by solder mask?] -- This means that there is a DRC error between your silkscreen and your soldermask both occupying an area of the same space, which is a NO-NO!!!

All that you need to do is to move the silkscreen item away from the soldermask of a pad enough to meet the spacing requirements of the DRC. However, it also depends upon -- WHAT PART -- of the silkscreen is causing the error. If the errors are being caused by the component -- REF DES -- then it should be easy enough to move those out of the way. But, if the errors are being caused by the component outline silkscreen, then you will either need to:

A) Edit the PCB-footprint silkscreen in such a manner as to remove the violation, "Save" the edited footprint and then replace the current PCB-footprint with the newly-edited one, or.....

B) Send me your GERBER files.....as I have an industry-standard "GERBER Analysis & Editing Program" that has a routine within it called, "Clear Silkscreen", which will automatically remove any silkscreen (graphic or text) that creates an error by overlapping (i.e., being "on top of") a pad or soldermask. Then, I can send your "clipped" GERBER files back to you. Other members of this forum have sent me their GERBER files so I can do exactly just that, plus also correct some other silkscreen (like the "lineweight" being too thin) and soldermask (like the mask area being the "same size" as the component pads) issues with their designs. Just a thought.....



/

 

[zamproject]

As a side note...

It's on a custom part for a cinemag transformer

footprint editor have DRC too, it a good practice to check a footprint design before load and use from a library.

 

[Matador]

KiCad by default will subtract the exposed areas of the soldermask from the silkscreen layer when you generate your Gerbers. The DRC violation is just telling you that some silkscreen items will be subtracted. I believe you can disable this, however then the board house may print silkscreen directly on plated traces where you intend to solder (which may or may not be great). Some board houses will do the subtraction on their end unless you explicitly tell them not to.

The vast majority of the time you can just ignore this, as it's just a warning. A ton of the default KiCad library parts have silkscreen that extends over soldermask openings (especially the SMD diodes), and it just means a few lines may be broken around the outline of the part.