PCB Holes, Drill Sizes and Clearances?

[NivagSwerdna]

I just got a PCB back and it was unfortunately made perfectly to specification!  I have a device (a IN12A Nixie) that was intended to mount through the board, I measured the Nixie pins at approx 1mm diameter but sadly I must have got distracted when creating the pattern (in DIPTRACE) and I specified holes which where 0.9mm....

... which got me thinking.... if I have a pin of diameter x mm then how big a hole do I need and are PCB manufacturers equipped with only a finite set of drill bit sizes?  which sizes?

i.e. Should I re-order with 1mm holes, 1.1mm holes, 1.2mm holes, 1.05mm holes?

Thanks in advance

[NivagSwerdna]

I found... https://www.olimex.com/PCB/FAQ/DrillHoles/

When I send my Drill tools sizes are they before or after the plating?
The drill tools sizes are assumed the drill tool sizes for drilling. After the plating in double side PCB the finished hole size will be -0.1 mm. i.e. 0.7 mm drill size will produce 0.6 mm final hole size. You should take this into account when you design your board. The general rule of tumb when you design your custom library parts is that if your component lead is X mm your drill hole should be X+0.3-4 mm i.e. if your component lead is 0.4 mm you must provide 0.7 - 0.8 mm drill hole, if you make the clearance bigger you will have more waste of solder when soldering and you may not fill your pads properly, if you make the clearance smaller you will have problems when you stuff your components.

This sounds feasible... so for my 1mm diameter lead I need to tweak my pattern to be 1.3mm?

[Siwastaja]

Plating won't be 50µm thick so adding extra +0.1 for plating already adds a bit more. It's still a good rule of thumb because it errs on the side of caution.

If your component lead is 1mm, a 1.1mm hole will give a tight fit, with a tiny bit of margin. It will fit.

HOWEVER, do note that component leads have tolerances as well - use the MAX value in the datasheet! If you measure it yourself, do note that your caliper may compress the lead a bit, giving a lower than actual reading. But a round lead in a round hole cannot compress when inserted to the hole.

A square or rectangular leg (think about pin headers, or TO-220 devices) is better, because it can compress a tiny bit when entering the hole, and the hole can stretch a bit as well, giving a snug fit. But for a round leg, you'd better add some extra margin. 1.3mm hole will indeed give you good margin if you have measured 1.0mm using a caliper.

Also note that with multi-pin components with rigid cases, you need to add the maximum cumulative position uncertainty of the leads as well. (Typically, the manufacturers make sure that the positioning error of the pins is non-cumulative, meaning that having a pitch of 2.54 +/ 0.01mm does NOT mean that the error between pins #1 and #100 could be 1mm.)

[DaJMasta]

"About 1mm" is also a bit of a coarse measurement, could be worth investing $20 or so in a cheap digital caliper so you can get a couple digits on your measurement.


That said, the IN12A is a common tube, you could look around for open hardware PCB layouts that have a footprint for it (or downloadable libraries with it), or you can actually look up the datasheet online.  Not the datasheet alone, but includes the mechanical drawings:
https://hackaday.io/project/1940-modular-nixie-display/log/11038-the-in-12a
1mm with +0.03 -0.07 tolerances



If I were to estimate, I'd probably go with 1.15mm or 1.2mm.  Those pins can bend a little and there seems to be slight variations between tubes, so I'd be slightly generous and the solder would bridge any gap just fine in any case.

[NivagSwerdna]

"About 1mm" is also a bit of a coarse measurement, could be worth investing $20 or so in a cheap digital caliper so you can get a couple digits on your measurement.

I do have such a device. 

.. the datasheet...
1mm with +0.03 -0.07 tolerances

Exactly. About 1mm 

[Benta]

The PCB CAD programs I know do not care about plating, but just about final size. The rest is up to the PCB manufacturer. If he doesn't supply PCBs with the specified hole size, it's his problem. Think about a single side PCB (I know, rare these days). The hole size is the drill size. For a through-plated PCB it's different, and only the manufacturer knows the size of his plating.

It's NOT your problem.

[IconicPCB]

Your design files should specify finished hole sizes.
It is up to the PCB shop to adjust the drill rack so that finished product hole size is correct.

On the other hand do specify finished hole size which is sensible. Keep in mind someone has to assemble the board and later on someone may have to disassemble the faulty garbage. Make the holes a comfortable size for disassembly purposes. Typically this may mean at least 0.2mm diameter oversize.

And just because the CAD program allows you to work with 0.1mm tracks and clearances and 0.2mm diameter via holes... don't do it.
Be sensible... do not push the envelop...  do not challenge the PCB shop production window. Save on reject rates .. save your money do that in Your design which will challenge the manufacturing ( and assembly ) process the least. It will be the most economic solution.  Your PCB shop will respect You.

You will save Your coin.

[langwadt]

Your design files should specify finished hole sizes.
It is up to the PCB shop to adjust the drill rack so that finished product hole size is correct.

On the other hand do specify finished hole size which is sensible. Keep in mind someone has to assemble the board and later on someone may have to disassemble the faulty garbage. Make the holes a comfortable size for disassembly purposes. Typically this may mean at least 0.2mm diameter oversize.

And just because the CAD program allows you to work with 0.1mm tracks and clearances and 0.2mm diameter via holes... don't do it.
Be sensible... do not push the envelop...  do not challenge the PCB shop production window. Save on reject rates .. save your money do that in Your design which will challenge the manufacturing ( and assembly ) process the least. It will be the most economic solution.  Your PCB shop will respect You.

You will save Your coin.

and just to pick a random example, jlpcb specs +/- 0.08mm on finished hole size

and holes that too big might be annoying but it's workable, holes that are too small might mean a scrap pcb

[Zero999]

How big are the pads?

If it's just a one off, then you could manually drill the holes bigger, rather than scrapping the entire PCB, but you lose the through hole plating and the pads will need to be big enough. If the pads are large enough and you can solder both sides, then drilling might be a viable option, for a one off.

[NivagSwerdna]

How big are the pads?

If it's just a one off, then you could manually drill the holes bigger, rather than scrapping the entire PCB, but you lose the through hole plating and the pads will need to be big enough. If the pads are large enough and you can solder both sides, then drilling might be a viable option, for a one off.

Indeed. That's my plan to drill out the holes using a 1mm bit. It might be touch and go since the pads are not large, the through hole doesn't matter since I will get connectivity through the pin as long as I can get solder on top and bottom pad.
This is only v1 and I am sure I will have other aspects that could justify a v1.001. Unfortunately I have six sockets with 12 pins each so 72 holes to drill for a single board... Almost just worth tweaking the design and reordering... Sorry Planet Earth!