Am I right that it is not possible to draw negative shapes on Non Copper Zone? The only thing that seems to affect the “Silkscreen fill” is knocked-out text.
If anyone was wondering why I am doing the negative is that silkscreen creates an air gap between the PCB and stepper plate. So I am filling the air gap with more ink.
Hi, are you adding a homogeneous layer of ink to create a thick gap between the thing that goes on top? Did I understand it right? If this is the case, isn’t it possible to ask for a thicker Solder Mask layer, instead?
Is it just the “Apply thermal paste” rectangle you’re trying to knockout?
As a workaround you can select your silk zone, do a RMB click and then select Zones > Add a Zone Cutout (though you’ll have then have to trace over the rectangle).
I didn’t know about the cutout zone feature and it will be indeed a useful workaround!
Might be better for some things than drawing with dashes in the text field.
I wish there was a “knockout” for shapes though.
Ultimately, I am doing this to make the bottom as flat (or as much contact) as possible for better thermals and so that thermal paste may not be even needed.
Currently, the ink sticks out maybe 0.05-0.1mm - a visible air gap when sliding a ruler edge across.
In the future, I may want to subtract a via annular ring from the silkscreen, but I want to see how much it shows up through the ink first. Anyway to streamline this in Kicad? Maybe through gerbers?
Thank you
Yes, there’s a Gerber option “Subtract soldermask from silkscreen”. (That of course only works for vias if you don’t tent them.)
I ended up drawing lines with dashes ______----- in Text items with Knockout 
:
Also, temporarily switching to untented vias and Subtracting soldermask from silkscreen produces a silkscreen like this:
@JeffYoung What do you think Kicad would embrace next regarding “negative layers”?
I can think of many possible improvements here (graphics avoidance by non-copper fill, negative graphics, converting polygons to complex cutouts, improving overlapping textboxes, etc.), however, it all seems unnecessarily complicated.
→ I think the best experience for the user would be if non-copper zone fill had the power to invert all the occluded graphics or text (combined).
I’m inclined to agree with you. Inverting is the only thing that handles text which is part-in and part-out of the non-copper zone. (Whether or not that’s useful, I can certainly see it coming up.)
Let me report back on how the board came out.
In terms of flatness, negative silkscreen boards are better. - Little bumps are now little dips.
Also, I can no longer recognize bumps due to the vias’ annular ring over the paint.
The contact surface is not perfect though. The painting technique from JLCPCB leaves visible streaks behind:
In practice, I didn’t really notice an improvement in heat transfer from PCB to the motor. (But applying thermal paste still improves it and so now at least less is needed.)
I put a razor to PCBs with positive and negative silk screens for comparison:
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.
