PCB pad/hole size advice

[Andrew]

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.

2. 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.

 

[Leon Heller]

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.

2. 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.

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

 

[Peter Bennett]

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

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)

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)?

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).

2. 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.

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