1. Home
  2. Electronics Design
  3. PCB pad/hole size advice

PCB pad/hole size advice

I've found that many of Protel's hole sizes are a bit small for my liking - in particular, the holes in their post header footprints are definitely too small.

I use .035" for most through-hole parts, and .025" for vias. Post headers need .040, and 1 amp diodes and larger electrolytic capacitors will need larger holes (and pads)

If the board maker quotes unplated hole sizes, you have to allow .003 or so for plating. When I order boards from the local shops, I specify finished hole size, and let the board shop figure out what drill to use (I don't know, or care, what drill sizes they have).

I would expect the board shop to translate between English and Metric dimensions as needed. There should be no need to create artwork and drill files in both measurement systems.

--
Peter Bennett, VE7CEI  
peterbb4 (at) interchange.ubc.ca  
new newsgroup users info : http://vancouver-webpages.com/nnq
GPS and NMEA info: http://vancouver-webpages.com/peter
Vancouver Power Squadron: http://vancouver.powersquadron.ca
Reply to
Peter Bennett
Loading thread data ...

I am a rather novice amateur PCB designer. I have designed a PCB using Protel 99 SE, using their standard library components and I am looking at getting prototype PCBs manufactured. I now find that the libraries have used numerous different hole and pad sizes, and that more different hole sizes = increase cost! Further I find that some manufacturers use imperial drill sizes and others metric.

So, I have two questions:

  1. the libraries mainly use the following pad/hole sizes (in mil=1/1000th inch) pad=62, hole=28mil/0.7112mm = decoupling capacitors pad=62, hole=32mil/0.8128mm = resistors pad=50, hole=32mil/0.8128mm = dip packages pad=62, hole=32mil/0.8128mm = vias

It would seem to me that I could reasonably use a single hole size for all of the above. One supplier (Olimex) has standard drill sizes of 0.7mm (27.6mil) and 0.9mm (35.4mil). Would using 0.9mm for all of the above components be a sensible choice (finished hole size would be a little smaller due to plating)?

What metric hole sizes would normally be used for such components.

  1. I would prefer a design that I could send to whatever manufacturer can offer the best price/delivery terms. This may not conistently be the same company depending on circumstances during the life of the product. How can I have a single design that can use either imperial or metric drill sizes depending on the supplier? I don't want to have to have two different design files, one imperial and one metric.
Reply to
Andrew

I use Pulsonix, and there are no problems having mixed metric and imperial sized parts in a design. If I'm creating a design for a PCB supplier like Olimex, I go through the design modifying all the holes to suit their requirements; it's quite fast if I make the changes in the technology file. I'm not altering the footprints in the libraries, of course. I also have a specific technology file for Olimex, set up for their design rules.

Olimex hole sizes *are* unplated, BTW. You need to allow for that. I find it very irritating, as most suppliers specify finished sizes. 0.9 mm is what I use for most parts with Olimex, like ICs and passive components, resulting in 0.8mm after plating. You also need to watch the annular ring with Olimex, their drilling machines must be rather crappy. They will reject the files if they are wrong, so you won't get sub-standard boards.

Most other prototype PCB suppliers (like PCB-Pool) that I use don't charge extra for different drill sizes, and can use much smaller annular rings as they presumably have better drilling machines. I haven't found anyone cheaper than Olimex, though.

Leon

--
Leon Heller, G1HSM
http://www.geocities.com/leon_heller
Reply to
Leon Heller

ElectronDepot website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.