Plated hole in SMD pad

Question

Hi

I've been using eagle for over 10 years. Currently using Eagle 5.12.

I am using some smt bottom feed through recepticles from mill max PDFs below.

actual part -http://www.mill-max.com/pdf/datasheet/pin_rec_catalog/8874-0-15-01-11-27-10-0.pdf

footprint- http://www.mill-max.com/pdf/datasheet/sockets/388-44-102-11-740799.pdf

How do I make a pad with a plated through hole in it's center, without causing an error?

Thanks,

Kim S.

Former Member · Answer

RadioCtrlDWife wrote:

Hi

I've been using eagle for over 10 years. Currently using Eagle 5.12.

I am using some smt bottom feed through recepticles from mill max
PDFs below.

actual part
-http://www.mill-max.com/pdf/datasheet/pin_rec_catalog/8874-0-15-01-11-27-

10-0.pdf

footprint-
http://www.mill-max.com/pdf/datasheet/sockets/388-44-102-11-740799.pdf

How do I make a pad with a plated through hole in it's center,
without causing an error?

Thanks,
Kim S.

It's not possible to make that footprint in Eagle without errors

Eagle Version 6 cannot make it either.

Plated holes can only exist if you use a pad the DRILL of which is plated

through.

A HOLE which is not plated through does not meet your requirements.

So it seems you need to use a PAD. Alas the DRC will adjust the pad so the

restring has width and that will spoil your footprint.

So it's back to the hole again.

You could instruct the board house merge the HOLES and DRILLS files so the

HOLES are plated through. You could manually do this yourself.

A ULP would be useful for that. Maybe there is one.

So the package becomes two SMD pads with holes. Alas there will be DRC

errors that you will need to approve.

I have suggested previously that Eagle needs a HOLE parameter named 'PTH'.

If it is 'true' the HOLE is treated as a DRILL, is plated through and the

signals (pours) don't keep clear of it so the PTH connects to copper. In a

package this hole/drill would need to be considered part of the SMD /Contact

and not generate a DRC error.

HTH

Warren

--

Viewed / responded via the newsgroup at

news.cadsoft.de

Former Member · Answer

Good to see your usage on a board.

Remember the PTH is done before the traces are etched so the barrels will

be fully formed and you need only approach the pad from one side as

soldering in the socket should fully fill the hole and attach to the other

side of the pad.

There is a way to make it work if you don't mind negating the RESTRING

settings/protection of the Design Rules (DRC)

In essence, what I'm about to suggest here results in the behaviour most

people expect work when they begin with Eagle so it should not be an issue

working this way.

If I make an incorrect statement during this explanation I hope someone

will correct me.

Two areas need changing

The DRC rules for the RESTRING

The PAD diameter of all parts in the library that you use in this design

with the changed DRC

Change all the RESTRING settings (top, inner, bottom)

% of drill diameter = 0%

Minimum = 0

This causes the DRC to calculate the RESTRING with a width of zero.

What appears on the board is the greater of the DRC calculated width or

that specified in the library package.

For most of the packages provided with Eagle the diameter is set to AUTO

which for this point in our discussion means 'use the DRC calculated size'.

Note that what you see in the library at this point (diameter set to

AUTO)is not the DRC calculated size but a size based on, I suspect, the

default DRC setting. But that is simply to provide a reasonable looking pad

in the package view. In the background the diameter is likely zero so the

DRC calculated size will always win.

So with AUTO set for the pad diameter and our new 0% DRC settings, above,

we get no restrings!!!!Just what we need for your footprint. But it happens

for all pads on the board. We have to fix that.

For the other packages used on the board we need to change the PAD diameter

from auto to a specified size. That then becomes the larger of the two

sizes(zero is the other size) and it is displayed on the board. This is the

way novices think it should work, i.e. The way it is in the library is how

it should be on the board, with no change.

What has been lost from the DRC is the automatic creation of minimum

restrings as specified by board houses.

It is not hard to ensure when you set pad diameters manually that you

exceed typical requirements.

In v6 you can make a footprint exactly as depicted in the datasheets you

identified. There would be no DRC errors(still requires the above

arrangement though).

With v5 you could compromise by using a LONG PAD which results in a length

close to that in the datasheet. Just accept it has round ends.

I feel some board houses may advise that there is insufficient copper

(Restring) around that PTH hole so you should advise in the documentation

you send them that it is not a design flaw and is required.

The method may cause quite a bit of work if you have many pads in your

libraries set to a diameter of AUTO.

If your board is basically a SMD design with only a few devices with PADs

then you could modify only those library packages involved.

For other boards you would set the DRC back to its defaults or what is

normal for your usage. The DRC settinga are retained within the board so

there is no issue as you move to other boards that used the more normal DRC

settings.

I feel this restring functionality is one of a few legacy behaviours in

Eagle that need changes due to the reducing geometries and higher densities

experienced these days.

Hope this helps

Warren

--

Web access to CadSoft support forums at www.eaglecentral.ca. Where the CadSoft EAGLE community meets.