Hii
After upgrade from Kicad 6 to 7 i got warnings silkscreen clipped by solder mask.
but my silkscreen is on front side and solder mask is on back side.
If that’s really the case it would be a bug and should be reported at the gitlab bugtracker.
But before doing so it would be good to attach the project in this thread, so we can confirm the behaviour (or find a different reason for the DRC-warning).
note: as a new user you are not allowed to attach files, you need at least the next forum user level. It would be good if you could read and follow this link: New Member Information.
If you fulfill the requirements (read at least 30 answers for at least 10minutes, in at least 5 different topics) you promote yourself to the next “basic user” level and are allowed to attach something to your posts.
Thanks for reply
Later that i found kicad is creating pads on both side of board and front side pads showing warnings with front solder mask. how can i remove pads from front side or do i need to change all silk screens?
The silkscreen clearance is probably set different in v7 than you and in v6 and now throwing warning.
They are not errors. Warnings only. Check you Fab house capabilities. Perhaps the footprints are correct, but you need to lower the minimum clearance value. Alternatively if only corners of silkscreen cap or resistors shapes are affected they will be clipped in the manufacturing process, but still readable, so not a big deal (unless the fact you have warnings bothers you).
A bit off topic, but I really don’t like the R10 angle 
Single sided PCB’s are becoming so rare that KiCad does not have many specific functions for it. You can disable the top copper layer for THT pads, but if you do that, your libraries become unusable for double sided PCB’s.
It is probably a more sensible solution to modify the footprints in such a way that silkscreen does not overlap with the pads at all. From the looks of it you just have to modify a few library footprints and then update your PCB with them.
But why does this happen in the first place? I guess that all KiCad’s default footprints are checked for this, and none have silkscreen overlapping with their own pads.
Alternatively, you can also just disable the DRC check. When you generate gerbers, you can also set a setting to clip the soldermask, so you would never have to scrape off solder mask from pads to be able to solder to them.
Well the solution is to modify footprints and whenever create new footprint have some clearance for solder mask clearance.
This r10 is pain 
i can’t do it 90° nor 180° and don’t want to increase length. I am thinking to remove it and give it directly to customer with chargers they will put it where ever they want.
It could be that you are still using the v6 library footprints or even foreign ones. See if you can replace all those rectangular capacitor footprints with one from v7 library which should have suitable clearance between pad and silkscreen line. Your capacitors all look like the same profile so it’s very easy to change the all footprints in one go.
For example here’s one from the v7 library with the correct clearance.
PS: It may be my bad eyesight, but you seem to be using a fairly large pad to soldermask clearance. For example the mask apertures of the transistor overlap. What’s your board setting for that?
There is nothing wrong with R10. Just omitting it and having your customer figure it out is about the worst solution.
If you really want to put it vertical, then you can put it closer to the IC, so all tracks under it are horizontal.
You can also put it horizontal just under R5 and then route the track to the inside of the IC.
And you can also use a bigger footprint to make more room to route tracks under it.
@Vikas_Dagar : one additional reason for this warning is probably that you have some expansion value set in File–>Board Setup–>Solder mask/paste–>solder mask expansion.
This value increases the size of the solder mask around a pad → therefore decreases the distance between designed silkscreen (in the footprint definition) and the pad mask. The silkscreen definition in the footprint (at least in the generic kicad libraries) can’t account for this extra distance as every user can set a different value.
I personally would:
- disable this DRC-check
- rely on the pcb-manufacturer to remove all overlapping silkscreen (depends on the manufacturer)
- but make sure that all references can be read either from bottom or from right side (not from top/left). compare R12 (ok) and R13 (not ok)
well thanks to all for reply.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.