I am designing a PCB in Kicad and I can define any diameter and hole of a via, but when I send it to be manufactured in china (JLCPCB, PCBWAY, etc) they can put any size of via or will it adjust to the closest value they have? The via I'm using must carry 5A, what standard value do you recommend? with a diameter of 1.6mm it should be enough but I am not sure if it is a commercial value
\$\begingroup\$
\$\endgroup\$
4
-
\$\begingroup\$ Depends on the manufacturer. Some prefer the Gerber to be final hole size, others prefer pre-plating size. From my experience some manufacturers will also round via sizes (i.e. all holes smaller than x will be made y, and so on). But they generally make it very clear. (I mean, a good fab house SHOULD make it very clear). \$\endgroup\$– Wesley LeeCommented Jul 7, 2021 at 18:25
-
3\$\begingroup\$ Not a full answer since it doesn't quite answer your question, but consider a number of standard size vias instead of larger ones if feasible. \$\endgroup\$– nanofaradCommented Jul 7, 2021 at 18:27
-
3\$\begingroup\$ Make all vias the same size and use more than one via for high-current links.It saves board space and it's cheaper. \$\endgroup\$– JankaCommented Jul 7, 2021 at 19:21
-
\$\begingroup\$ This may be an X-Y problem. I Just want to reinforce what nanofarad said: For high currents, multiple smaller vias are almost always better than one large one. \$\endgroup\$– evildemonicCommented Jul 7, 2021 at 19:51
Add a comment
|
3 Answers
\$\begingroup\$
\$\endgroup\$
One approach is to use the minimum size for minimum cost PCB if that works for your design. For example, for PCBWay there is a delta between 0.3 and 0.25mm for regular FR-4 boards, so if you can use 0.3mm or larger for all your vias it will save a bit of money (or a lot of money if you're tempted to use very small vias). The next steps are at 0.2 and 0.15mm.
For higher currents such as 5A you can refer to the design guides that many manufacturers supply. Probably 5 0.3mm (~12 mil) vias would be fine, according to this King Sun data assuming 10°C rise is acceptable. According to this calculator your suggested 1.6mm hole is also fine. They don't specify the rise allowed in their calculation though. Altium claims:
As long as your PCB traces are sized according to the minimum trace widths specified in the IPC 2152 standard, and your vias are sized to comply with DFM standards and applicable IPC standards, you won’t have to worry about temperature rise in your vias. The excess heat in the interior of the via gets dissipated into the substrate and the nearby traces. In the case where the traces are very wide, they have a larger surface through which to dissipate heat compared to the via. In this case, the heat leaves the trace at a faster rate than it leaves the via, thus the trace will reach a lower equilibrium temperature. This was confirmed in the experimental study by Douglas Brooks and Johannes Adam in SIJ.
Generally you can request any size hole you want, within the capabilities list, and they will produce the holes within the specified tolerance after plating. For example, for PCBWay a 0.6mm drill results in a finished hole size between 0.52mm and 0.68mm.
answered Jul 7, 2021 at 19:18
\$\begingroup\$
\$\endgroup\$
1.4 mm is the minimum drill size rated for a 5A PTH, so 1.6 mm is adequate.
Using teardrop trace to via connections for large pads makes them more rugged.
\$\begingroup\$
\$\endgroup\$
1
The board shop doesn't know or care whether a hole is for a via, for a component lead, or for a mounting hole, or just for ventilation - regardless of your purpose, to them it is just a hole to be drilled, so when specifying a hole size for any purpose, you must follow the shop's requirements for hole sizess.
answered Jul 7, 2021 at 19:31
-
1\$\begingroup\$ Almost, but if the hole is to be plated then PCB packages typically specify the finished size, so the drill size will be slightly larger. \$\endgroup\$– FrogCommented Jul 7, 2021 at 19:51