What via sizes for cheap PCB Fab houses

[awardblvr]

Noob here…

On a 2-sided board 3"x4" (2oz copper BTW cuz of some heavy currents / MOSFETS) to be produced by one of the fab houses recommended by pcbshopper.com…

For my signal traces (500Khz highest, most in < 1 Khz) I would like the thinnest reasonable traces. I’m trying 6 mil (.153) and am trying to understand the appropriate drill hole and via sizes. Please help.

1. Are there “standard” drill sizes I should be aware of? Or, are these laser cut so that I can put in any size within a range and it will be done that size?

2. What are some recommendations for these track widths, clearances, and via sizes?

3. Do some fab houses do better than others with certain combinations of clearance+track_width+via_size? How would I know?

[LsDelancy]

I’m pretty sure that is all going to vary from fab to fab. The only way to know for sure is to check with whatever fab you are planing to use. Is this a prototype board or a production run with large numbers?

[davidsrsb]

The KiCad default is safe. Push further to the claimed fab limits and you can expect problems

[marcos]

Beware that with thicker copper the fab min width/cleareances will change. At 2 Oz some fabs derate their specs to 10mils/10mils. At 3Oz they derate more.
You should ask the factory about these things.

[dchisholm]

@awardblvr

For my signal traces (500Khz highest, most in < 1 Khz) I would like the thinnest reasonable traces. I’m trying 6 mil (.153) and am trying to understand the appropriate drill hole and via sizes. Please help. [/quote]
A minimum trace width of 6 mils is currently the most common value I see advertised for “standard” jobs, though it is far from universal. A few advertise the ability to do narrower traces, but at greater cost. It’s probably accurate to say that the great majority of fabricators can supply 8 mil traces or narrower. The closer your specified trace widths get to the fabricator’s advertised capabilities, the more likely it becomes that there will be problems. Remember that the “6 mil” value is subject to a manufacturing tolerance of plus-or-minus a few mils, so the trace width you receive may be only a fraction of the width you specified.

The same comments apply to copper-to-copper spacing. It seldom matters if it’s trace-to-trace, trace-to-pad, pad-to-pad, or some other copper feature: copper is copper. The minimum spacing is usually the same as the minimum trace width.

Note that both width and spacing requirements will vary from inner to outer layers, as well as various copper “weights” (i.e., thickness of the copper foil).

1. Are there “standard” drill sizes I should be aware of? Or, are these laser cut so that I can put in any size within a range and it will be done that size?

I think every fabricator of quick-turn prototype boards has a “standard tool rack” that can produce holes with specified finish sizes (with a tolerance of a few mils). Some have about a dozen “standard” sizes; others may have up to 25 or 30. Many vendors tell you what the standard hole sizes are; many don’t. And, no two fabricators seem to agree on what hole sizes belong in the “standard tool rack”. Every hole you specify will be mapped into the selection of standard sizes using an algorithm that the vendor may, or may not, describe. You can see one supplier’s description of their “standard” drill sizes at: Standard Drill Sizes Example

2. What are some recommendations for these track widths, clearances, and via sizes?

It is not easy to answer the question, “What is the minimum practical trace width for {some signal}?”. KiCAD includes a calculator to help answer that question, and there are several others on various web sites.

The board fabricator may specify a minimum via size (both pad and drill sizes). At the least, he will specify the smallest plated-through hole he can produce, and the minimum annular ring of copper around the hole.

Most fabricators will publish at least a summary of their capabilities. Some are much more informative than others. One example is PWB Manufacturing Capabilities

Another, very comprehensive (about 50 pages!) guide was published by SeeedStudio at PCB Design For Manufacture (OK, there’s only about 6 pages describing the fabricator’s requirements and capabilities - the rest is a more general guide to layout and board design.)

[quote] Do some fab houses do better than others with certain combinations of clearance+track_width+via_size? How would I know?

Over the last 15 years or so I have dealt with at least a dozen different board fabricators. Every one of them supplied a board that met their advertised specification. Some were well within their specification, while others were near the limits of their specification. Around two years ago I believe there was a thread on this Forum where members commented on the performance and quality of various vendors’ products. (Or maybe it was on the “DIYAudio” forum?)

Dale

[davidsrsb]

I have only had to use thinner than the default 10 mil on boards using BGA packages. As you push fabs to 6 mil and fine vias, the fab is going to get yield problems, which you are going to pay for, either in higher prices or by getting some bad boards

[dchisholm]

@davidsrsb

I have only had to use thinner than the default 10 mil on boards using BGA packages . . . .

The board I most recently finished was done primarily with 20-mil traces and 15-mil spacings. In a few places I had to step down to 15- or 10-mil traces and 10-mil spacing. This board was about 100 SMT components (1206, SOT-23, and SOIC; plus a few through-hole connectors) and will be hand-soldered.

Dale

[paulvdh]

@awardblvr

I would like the thinnest reasonable traces

There is a PCB calculator which calculates temperature rise for trace width & thickness.

For vias bigger is better for current handling.
Alternative is to remove the solder mask (un tented vias?) and fill the vias with solder.
You should also consider multiple vias to divide the current.

If your application permits it:
Putting the wires through a hole in the pcb (for mechanical stability) and then soldering them directly to the copper a few cm further is very good for current handling. You should put some vias through the PCB on the place were the wire is soldered for mechanical strength. This way the copper wil not be ripped of the PCB when the wires are pulled. (This also works good for SMD connectors)

[HiGreg]

@dchisholm

@awardblvr

Are there “standard” drill sizes I should be aware of? Or, are these laser cut so that I can put in any size within a range and it will be done that size?

I think every fabricator of quick-turn prototype boards has a “standard tool rack” that can produce holes with specified finish sizes (with a tolerance of a few mils). Some have about a dozen “standard” sizes; others may have up to 25 or 30. Many vendors tell you what the standard hole sizes are; many don’t. And, no two fabricators seem to agree on what hole sizes belong in the “standard tool rack”. Every hole you specify will be mapped into the selection of standard sizes using an algorithm that the vendor may, or may not, describe. You can see one supplier’s description of their “standard” drill sizes at: Standard Drill Sizes Example

I have included drill sets within KiPadCheck, but I have not yet included a variety of algorithms that manufacturers might use to select the specific drill size from their set. Obviously, the manufacturer may specify something different, but the drill sets in KiPadCheck are:

[dchisholm]

@HiGreg

. . . I have included drill sets within KiPadCheck, but I have not yet included a variety of algorithms that manufacturers might use to select the specific drill size from their set . . . .

I wouldn’t lose any sleep over trying to cover all possibilities. In the first place, if the PC board is fabricated by anybody living in the 21st century, you are buying the FINISHED hole size, which is a few mils smaller than the drill size that started the process. There are fairly accurate guidelines for how much smaller the finished hole will be, but it will vary from one vendor to another and depends on the details of their fabrication process.

As for the size mapping process, there seems to be two main algorithms. Some vendors fabricate the hole to the standard size that is nearest to your drawing’s requirement, while others sell you the next largest hole (if your requirement doesn’t match a standard size). About a dozen years ago I had a vendor who wouldn’t build my board until the hole sizes on my drawing matched his standard sizes - letting me decide whether a particular hole should be enlarged or reduced, if it wasn’t one of the standard sizes.

Dale