Hi Guys. I would like to expose part of copper traces on my board(high current traces), in order to add coating so they can sustain current needed, while remaining part of the board should not be exposed. How can i do this? Thank you.
one way seems to be to draw a graphic-line on the F.Mask (or B.Mask) layer, on top of your trace, and then edit that line to be the same width as the trace. 3D view should show a hole in the soldermask where you drew the line.
Maybe in the future a more flexible keepout-zone tool would be nice where mask-layers could also be selected for the keepout?
As above, you can draw-over on F.mask.
There is no direct way to clone/move-layer on many traces, if you have a lot to expose, but there are some indirect ways.
If you create a temp file, and unroute non-exposed traces, then plot exposed traces left, then GerbView can open and Export to PCBnew, selecting F.mask as export layer.
You can then Open/edit/save and then append that design to the original.
Thank you guys. It works very well.
I used copper zones in order to widen the tracks, and then I place same zone on a mask layer.
But you have to take into account, that just adding solder will not increase current capacity much, as solder has significantly higher resistivity. For serious current you will have to solder additional copper (solder wick wire is good from mechanical standpoint as it is soft and will not cause board bending that you get when soldering thick copper bars, but has much lower fill factor then solid copper bar)
1 Like
On the other hand more metal means more heat conductivity, which in the end may be as important as electrical.
If you start to worry about solder not being conductive enough then you might reach the point where copper inlays would be the best solution. Or placing the parts with that much current off board if you are not prepared to pay extra for inlays.
I was just pointing out if you take 35 um or 70 um PCB and then you add 0,5 mm of solder on top, the solder will not help as much as one would guess from the thickness only
I’ve heard rumours that the conductivity of PB-Free solder is also a lot less than of the old fashioned stuff.
Some manufacturers have been able to make PCB’s with copper of a mm or even more thickness (30x normal), but this is relaitively expensive because of long etching times and other constraints.
The Car industry with all the electric and hybrid cars have increased the demand for high current PCB’s and it seems tat sevaral PCB manufacturers have invented solutions of putting more copper on PCB’s at lower costs.
Browse a bit around on what’s available in this fast evolving world:
https://duckduckgo.com/?q=pcb+“heavy+copper”&iax=images&ia=images
Here are some numbers
Material Resistivity ρ (Ω·m) at 20 °C
Silver 1.59×10−8
Copper 1.68×10−8
Tin 1.09×10−7
Lead 2.20×10−7
So Copper is 6~7 times better than Tin, and Tin is better than Lead
ie to halve the resistance, you need a Tin solder layer applied of 6~7x the copper thickness
Probably easier to just buy thicker copper, unless you are already maxed-out there ?
Is there’s a better (and quicker way) to uncover tracks ?
I’d like to put a SMD proto area on a PCB but can’t manage to find a convenient way for doing it.
draw a zone over the area you want uncovered on the mask layer
Or just a graphical polygon (different than zone).
I think zones on non copper layers are the same as polygons. (Not necessarily on a file format basis but on a behavioral basis.)
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.