Solder Jumpers

[John Luciani]

In Eagle there are a couple of solder-jumper footprints. To jumper between pads
you create a solder bridge. The two pad jumper looks like two half
circles with a
gap in between. The three pad jumper consists of a half circle on each
end with a rectangular pad in between.

I am looking for the dimensions of the pads and gaps or some recommendations.

I was thinking of making 20x50 mil rectangular pads with 10 mil gaps.

Thanks.

(* jcl *)

[Ben Jackson]

Post by John Luciani
gap in between. The three pad jumper consists of a half circle on each
end with a rectangular pad in between.

I'm sure you have a reason for using special pads, but I'd just use some
SMT resistor footprint. I've made 3-pad strapping setups by putting a
pull up and down in the schematic and then overlapping the common pad so
a resistor can be installed either way. Of course they cannot just be
bridged with solder.

As for gaps, why not pull out an old unpopulated board and try a few
existing footprints? QFP, TSSOP and maybe SO have gaps in the range
you'd like to try. See what bridges well enough for your app.

[John Luciani]

Post by Ben Jackson

Post by John Luciani
gap in between. The three pad jumper consists of a half circle on each
end with a rectangular pad in between.

I'm sure you have a reason for using special pads, but I'd just use some
SMT resistor footprint. I've made 3-pad strapping setups by putting a
pull up and down in the schematic and then overlapping the common pad so
a resistor can be installed either way. Of course they cannot just be
bridged with solder.

The Arduino (and various 'duino brethren) have these configuration
jumpers. Since these
boards are built by novices I wanted to find the size jumper that they
typically use.

Post by Ben Jackson
As for gaps, why not pull out an old unpopulated board and try a few
existing footprints? QFP, TSSOP and maybe SO have gaps in the range
you'd like to try. See what bridges well enough for your app.

If I can't find out some actual dimensions that people have used or seen
then it's down to the cellar ;-)

Thanks.

(* jcl *)

[Ben Jackson]

Post by John Luciani
boards are built by novices I wanted to find the size jumper that they
typically use.

The round pad with split "affords" bridging. Two square pads don't quite
have the same effect. Too bad PCB can't make the semi-circular pads!

http://en.wikipedia.org/wiki/Affordance

[DJ Delorie]

Post by John Luciani
If I can't find out some actual dimensions that people have used or
seen then it's down to the cellar ;-)

If you want a test board, I can probably etch one tomorrow and mail it
to you. Just send me a .pcb file. Or a postscript file, if you want
to try semicircles also.

[John Luciani]

Post by DJ Delorie

Post by John Luciani
If I can't find out some actual dimensions that people have used or
seen then it's down to the cellar ;-)

If you want a test board, I can probably etch one tomorrow and mail it
to you. Just send me a .pcb file.

Thanks for the offer. These footprints are for future use so there
is no rush.

Post by DJ Delorie
Or a postscript file, if you want to try semicircles also.

I am hoping to build two footprints.

Is there a secret PCB file format change that would permit
the creation of semi-circular pads and that also implements
that PCB datum request?

Could be time to upgrade ;-)

(* jcl *)

[DJ Delorie]

Post by John Luciani
I am hoping to build two footprints.

I was thinking of a range of gap sizes, so you could see how well they
bridge.

Post by John Luciani
Is there a secret PCB file format change that would permit
the creation of semi-circular pads and that also implements
that PCB datum request?

No, no changes like that since the ancient version you use ;-)

[Kai-Martin Knaak]

Post by John Luciani
I am looking for the dimensions of the pads and gaps or some
recommendations.

You might look at JMP_SMD.fp in my section of gedasymbols. These jumpers
have been proven to work with my last couple of boards. The gap is narrow
enough to be bridged. Yet, it is wide enough to easily yield two separate
solder pads. I deliberately combined a rounded and a rectangular pad, to
get rid of the corners at the far end. This allows for a more roundish
drop of solder and makes it easier to bridge the gap.

Unfortunately I haven't done a three terminal jumper yet.

Post by John Luciani
I was thinking of making 20x50 mil rectangular pads with 10 mil gaps.

The gap is ok. But narrow pads would make it more difficult to open the
jumper without a solder pump.

---<(kaimartin>)---

[John Luciani]

Post by Kai-Martin Knaak

Post by John Luciani
I am looking for the dimensions of the pads and gaps or some recommendations.

You might look at JMP_SMD.fp in my section of gedasymbols. These jumpers
have been proven to work with my last couple of boards. The gap is narrow
enough to be bridged. Yet, it is wide enough to easily yield two separate
solder pads. I deliberately combined a rounded and a rectangular pad, to
get rid of the corners at the far end. This allows for a more roundish
drop of solder and makes it easier to bridge the gap.
Unfortunately I haven't done a three terminal jumper yet.

Post by John Luciani
I was thinking of making 20x50 mil rectangular pads with 10 mil gaps.

The gap is ok. But narrow pads would make it more difficult to open the
jumper without a solder pump.

Thanks.

Those pads look like ~ 50x70 mil and the gap is ~ 10mils.

(* jcl *)

[DJ Delorie]

You can combine four rounded pads and a square one to form each half
of these:

Loading Image...

(the tiny one is one rounded + one square, for reference)

[John Luciani]

Post by DJ Delorie
You can combine four rounded pads and a square one to form each half
http://www.delorie.com/pcb/jumpers.png
(the tiny one is one rounded + one square, for reference)

The footprint in the lower right looks quite good.

Thanks.

(* jcl *)

[DJ Delorie]

Post by John Luciani
The footprint in the lower right looks quite good.
Thanks.

You need a .pcb, of figured it out already?

[John Luciani]

Post by DJ Delorie

Post by John Luciani
The footprint in the lower right looks quite good.
Thanks.

You need a .pcb, of figured it out already?

I am all set.

Thanks for your help

(* jcl *)

[Steven Michalske]

jcl,

I have made this the size of 0603 parts so that i can solder ball
them, or stuff them with an 0603 resistor.

Could we make a copper shorted version as well?
It allows for the reverse of the idea, by default it is connects two
nets that an exacto can cut out.

Hardkrash

Post by John Luciani
In Eagle there are a couple of solder-jumper footprints. To jumper between pads
you create a solder bridge. The two pad jumper looks like two half
circles with a
gap in between. The three pad jumper consists of a half circle on each
end with a rectangular pad in between.
I am looking for the dimensions of the pads and gaps or some
recommendations.
I was thinking of making 20x50 mil rectangular pads with 10 mil gaps.
Thanks.
(* jcl *)
--
http://www.luciani.org
_______________________________________________
geda-user mailing list
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user

[John Luciani]

Post by Steven Michalske
jcl,
I have made this the size of 0603 parts so that i can solder ball
them, or stuff them with an 0603 resistor.
Could we make a copper shorted version as well?
It allows for the reverse of the idea, by default it is connects two
nets that an exacto can cut out.

I don't see why not.

(* jcl *)

[Dan McMahill]

Post by John Luciani

Post by Steven Michalske
jcl,
I have made this the size of 0603 parts so that i can solder ball
them, or stuff them with an 0603 resistor.
Could we make a copper shorted version as well?
It allows for the reverse of the idea, by default it is connects two
nets that an exacto can cut out.

I don't see why not.

you know, solder bridgable gap footprints are a candidate for a keepout
layer to keep you from putting a trace through the gap. Of course you
may just want to make the gap narrow enough that you'd have drc
violations by putting a trace there.

-Dan

[DJ Delorie]

Post by Dan McMahill
you know, solder bridgable gap footprints are a candidate for a
keepout layer to keep you from putting a trace through the gap. Of
course you may just want to make the gap narrow enough that you'd
have drc violations by putting a trace there.

I think that should wait until we have more robust footprint options.

[John Luciani]

Post by Dan McMahill

Post by John Luciani

Post by Steven Michalske
jcl,
I have made this the size of 0603 parts so that i can solder ball
them, or stuff them with an 0603 resistor.
Could we make a copper shorted version as well?
It allows for the reverse of the idea, by default it is connects two
nets that an exacto can cut out.

I don't see why not.

you know, solder bridgable gap footprints are a candidate for a keepout
layer to keep you from putting a trace through the gap. Of course you
may just want to make the gap narrow enough that you'd have drc
violations by putting a trace there.

I was thinking of 10mils which would force a DRC violation for my
design rules.

(* jcl *)