I want to set settings for JLCPCB manufacture.
It specifies:
“Min. Trace Spacing”: 0.127mm → So in KiCad I go to Board Settup and set “Copper minimum clearence” to 0,127mm. OK!
But JLCPCB specifies a minimum “Pad to Track of 0.2mm”, and there is no GENERAL setting to do that.
In Eagle I could do set that easily.
As I understand, in KiCad, I need to go footprint by footprint on the PCB, go to properties and set “Pad clearence” to 0.2mm
That is a very repetitive and tiresome process :-S which is such a shame, because in everyother aspect, KiCad is a lot better than Eagle, and also free of course.
One solution is to go to Board Settup and set “Copper minimum clearence” to 0,2mm. But that will also affect trace to trace distance and it’s a waste of space for complex PCBs
This needs at least some answer after 3 weeks…
Edit: “2 MONTHS LATER” ??? Ah, it’s April instead of March. Still more reason to give it an answer…
Can you be more elaborate with which setting you set where?
There is a “Copper”Minimum clarance and Minimum track width, in: Pcb Editor / File / Board Setup / Design Rules / Constraints, but those are not numbers which are used when drawing the PCB. Those are global rules which generate errors when violated.
In KiCad, all nets are member of a Netclass, and if you do not set any properties for a net class, then all of your nets are in the Default Net class.
Settings for net classes are in: PCB Editor / File / Board Setup / Design Rules / Net Classes. Setting a few net classes is a normal part of PCB design. Usually signal tracks are thin, while power tracks are substantially wider. High voltage tracks may need a bigger clearance etc.
A new feature in KiCad V6 is that you can already define net classes in the schematic. (Schematic Editor / File / Schematic Setup / Project / Net Classes) When you do this, you can also set a custom line width and color to put a bit more emphasis on some of the wires in the schematic.
To keep your design organized, combine net classes with labels, so your nets have real names. With the auto generated names for nets you can easily loose track of what is what.
Thanks for tanking the time in answering
I found those, but one thing is distance between tracks, another thickness and another distance between pad and tracks.
For example there could be a 5mil distance between tracks and that’s fine according to PCB manufacturer specifications, but a 5mil distance between a pad and a track is less than the minimum specification.
If course you could use a distance between signals of 8mil for example so pad to track distance is within specs, but you are not taking advantage of a possible much less distance between tracks.
So what I had to do is edit all footprints individually of the parts I used, to have the minimum pad clearence I wanted (I don’t remember what’s that called in kicad)
Eagle has that feature, it’s very easy to change, kicad is missing it
To be honest, trying to decipher the JLCPCB rules and find out whether or not their images illustrate the rules or not gives me headache. They are ambiguous (unless you happen to know from some other context what they may mean) and it’s difficult to say why there are so many different rules.
Some years ago at work we used JLCPB for quite many board. We needed everything to be as small as reasonably possible, so we went to the limit. But I used only one clearance value for everything copper to copper, IIRC 0.17 mm was the smallest I used on some boards, and it was their recommended smallest clearance back then. They made them without a hiccup, and the boards worked. It’s very difficult to see why pad to track should now be 0.2mm.
But, as mf_ibfeew said, in KiCad v6 there is the possibility of using custom rules.
As a start:
(version 1)
(rule “Clearance track_to_Pads”
(constraint clearance (min 0.2mm))
(condition "A.Type ==‘Track’ && B.Type ==‘Pad’ "))
oh ok, awesome didn’t knew this!!
So it seems changing this rule is not possible in the GUI. Thanks!
But I would recommend to set the clearance generally to 0.2mm - working with reserve (and not on the bleeding edge) is mostly a good idea.
The thing is that it really makes a difference to use minimum track distance vs 0.2mm, it’s another world. And JLCPCB can really handle this well, it’s not a risk to use 6-8 mil of distance between tracks, I’ve done it several times.
Thanks awesomeeee, now KiCad has everything I need
Also, I checked on this rule AFTER I got the PCBs from JLCPCB and I can see now that there were some tracks that had less than 0.2mm and it got manufactured fine apparently as I can check on my multimeter. Tracks don’t overlap, but next time I will make sure to implement this.
