Maker Pro
Maker Pro

Eagle PCB Drill Hole Sizes question?

S

Squareness Wafer

Jan 1, 1970
0
Hi,
I'm a total newbie with designing PCB's. I have been struggling with
Eagle for the past couple of weeks and finally getting the hang of it.
I am doing a double sided PCB for a guitar effect pedal that will
include IC's, resisters, caps, microchip, the standard stuff.

In general, what are some good hole sizes to use? I would prefer to
minimize the number of different drill bits. This will all be hand
soldered, and I just need to make sure everything has a decent enough
fit.

Also, when using EAGLE, what is the best way to change the hole
diameters in the pads? All of the components from the library just
uses whatever it is they use, and it doesn't even say!

Thanks so much for any help. This is definitely a struggle, and I
really want my first professional PCB to turn out right! :)
 
M

Mario Trams

Jan 1, 1970
0
Squareness said:
In general, what are some good hole sizes to use? I would prefer to
minimize the number of different drill bits. This will all be hand
soldered, and I just need to make sure everything has a decent enough
fit.

As Tilmann said, we cannot tell you "some good hole sizes". The
data sheets of the devices you are planning to use will tell it
instead.
Also, when using EAGLE, what is the best way to change the hole
diameters in the pads? All of the components from the library just
uses whatever it is they use, and it doesn't even say!

In order to check the diameters of the library elements, you may
open the desired library/package and check it there (i.e. with
"info"). As an alternative, put the library element in your design,
select a high-resolution grid and use the pointer position to
calculate distances. You also might place the "mark" (the virtual
zero-point of the coordinate system) at on end, and the pointer
to the other one. You don't need to subtract in this case...

Regards,
Mario
 
E

EEng

Jan 1, 1970
0
Hi,
I'm a total newbie with designing PCB's. I have been struggling with
Eagle for the past couple of weeks and finally getting the hang of it.
I am doing a double sided PCB for a guitar effect pedal that will
include IC's, resisters, caps, microchip, the standard stuff.

In general, what are some good hole sizes to use? I would prefer to
minimize the number of different drill bits. This will all be hand
soldered, and I just need to make sure everything has a decent enough
fit.

Also, when using EAGLE, what is the best way to change the hole
diameters in the pads? All of the components from the library just
uses whatever it is they use, and it doesn't even say!

Thanks so much for any help. This is definitely a struggle, and I
really want my first professional PCB to turn out right! :)

For standard components such as 1/4W resistors, basic tantalum,
ceramic, electrolytic, mylar, etc...capacitors, inductors,
transistors, chips, etc...the most common used hole size is .035
finished. Depending on the board house you use, you may have to tell
them that you want .035 FINISHED because when they thru-plate, it
adds a few mils of material, thus reducing the prescribed hole size.
Now, most board houses know you want your dimensions as finished sizes
and will increase your hole size accordingly so it ends up at what you
specified, but check with them anyway.

As you begin using parts with larger leads such as any of the 1N40XX
diodes, jump it up to .040 or .045.

The BEST way to determine hole size for non-standard parts is to
measure the lead's widest point (on square pins that would be the
diagonal from corner to corner) then add 7-10 mils. Example: Standard
resistor lead = .028 + .007 = .035mils (most common hold size used).

Now you have the issue of the annular ring, that is, the pad.
Depending on circuit density, you may have to go with smaller pads
than you like. Some people like 50mil (way too big), some like 10mil
(almost too small although I've used it with great success many times)
and for those who intend to do everything by hand, it seems 20mils is
comfortable. You're going to have to make a judgement call, its
purely subjective.
 
S

Squareness Wafer

Jan 1, 1970
0
To get a correct board, you must use the drills that are required
for the parts you put in there. If the libraries are correctly
defined, they contain these drills that really are needed.
I agree that the mechanical data in the "default" libraries are
not always correct. (I use only self-defined libraries.)

If you can accept some tolerances, simply set the tolerance values
in the CAM processor accordingly and reduce your drill rack to the
diameters you really want to use. However take care that some of
your parts might not fit anymore, or might be to loosely.

Hi,

as for the user defined parts, the diameters they allow me to choose
are still limited. i'm trying to do, like, a 0.9 mm drill size, but
the closest drill size they have is .032 IN. which is .003 off. any
way to change these default values?

thanks again!
 
T

Tilmann Reh

Jan 1, 1970
0
Squareness said:
as for the user defined parts, the diameters they allow me to choose
are still limited. i'm trying to do, like, a 0.9 mm drill size, but
the closest drill size they have is .032 IN. which is .003 off. any
way to change these default values?

Don't care about this.
As I said, the mechanical data in the default libraries often are
not perfect, honestly speaking. They also are almost completely
dimensioned in imperial units...

Just set up your own drill rack file (look at drillcfg.ulp) containing
the drills you can use and accept, and then set tolerances in the CAMP.

--
Dipl.-Ing. Tilmann Reh
Autometer GmbH Siegen - Elektronik nach Maß.
http://www.autometer.de

==================================================================
In a world without walls and fences, who needs Windows and Gates ?
(Sun Microsystems)
 
Top