Elecrow Design Rules

Hi all

I tried to find a guide for this but was not so successfull as i hoped

Anyone that has used elecrow before and can post screenshots of how the design rules are set up?

gerber generation is not the issue for me

using v5 of kicad

From https://www.elecrow.com/pcb-manufacturing.html

Multi Layers 1-2-4
PCB Material FR-4
Available Color Green, Red, Yellow, Blue, White, Black
Silk Screen White, Black (For White Solder Mask only)
Maximum Size 45cm X 120cm
Minimum Qty 10pcs
Board Thickness 0.6mm,0.8mm, 1.0mm, 1.2mm, 1.6mm
Thickness Tolerance (t≥1.0mm) ± 10%
Thickness Tolerance (t<1.0mm) ± 0.1mm
Insulation Layer Thickness 0.075mm–5.00mm
Minimum PCB track (Recommend >8mil)
Minimum Track/Vias Space 6mil (Recommend >8mil)
Minimum pads Space 8mil
Minimum silkscreen text size 32mil
Out Layer Copper Thickness 1oz(35um)
Inner Layer Copper Thickness 17um
Drilling Hole (Mechanical) 0.3mm—6.35mm
Finish Hole (Mechanical) 0.8mm—6.35mm
Drill Diameter Tolerance (unplated) 0.05mm
Drill Diameter Tolerance (plated) 0.1mm
Outline Tolerance (Mechanical) ±0.20mm
Aspect Ratio 8:1
Solder Mask Type Photosensitive ink
SMT min Solder Mask Width 0.2mm
Min Solder Mask Clearance 0.2mm
Solder Mask Thickness 15um
Surface Finish HASL, HASL (Lead Free), ENIG

I am convinced that the minimum plated through hole size is 0.3mm (After reading the eagle dru file) -> This means the minimum via drill size is 0.3mm.

yep but things are called at little different in kicad and that is what confuses me badly

i found an old guide for kicad but the screeenshots in that did not look anything like in v5

currently i have them set to

“Clearance” is “space between”, is there anything else? Change the net class clearances to 8mil (0,2032mm) minimum, otherwise they seem to be OK. You don’t need µVias, I think. You have to take care that each footprint doesn’t have too small pad-to-pad clearance.

EDIT: some track widths are too narrow, too.

got you on the net class clearance

but you say track widths are to narrow? do you have the diff pair in mind? because those are the only ones i can see that are under 0,2032mm

Sorry, my bad! I don’t know what I was thinking. Well, the time was 1AM…

hehe, same thing happens to me, some times yo just cant let go from things and get tired and then mistakes happen

Elecrow can actually do better than the specs they publish, it’s worth checking with them if you are getting to the limits and asking them what they’d prefer. For instance I had issues getting no solder mask between some fine pitch pads (which means they often bridge during reflow). After a bit of back and forth the minimum width of solder mask they can do is 0.15mm and you need 0.075mm either side of the pad. So for, eg, 0.5mm your max pad size is 0.5 - 0.15 - 0.075 - 0.075 = 0.2mm. They also said they prefer if I want minimum pad clearance to specify it as 0 and they’ll increase it to the minimum, instead of specifying the 0.075.

All the boards I’ve had done since then I’ve spec’ed this way and I have had solder mask where I needed it.

This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.