Searching \ for '[EE] Notched PCBs' in subject line. ()
Make payments with PayPal - it's fast, free and secure! Help us get a faster server
FAQ page: www.piclist.com/techref/pcbs.htm?key=pcb
Search entire site for: 'Notched PCBs'.

Exact match. Not showing close matches.
PICList Thread
'[EE] Notched PCBs'
2005\11\21@214507 by David Van Horn

picon face

I haven't seen this covered anywhere, thought I'd ask.

I'm looking to make crenellations in the side of a PCB.
That is, to have "half a pad" so that pins can be laid alongside the PCB
and soldered into the circuit, rather than being threaded through a
hole.

Does anyone know how to do this without the mill putting copper kerf
into the hole?




2005\11\21@231526 by Bob Blick

face picon face
Hi David,

You need to make your pad U-shaped and leave clearance for the
cutout. Some CAD packages may not allow pads like that so you'll
have to do some trick like add another layer with the right copper
shape. And then ignore clearance errors when you verify the design.

Designing a car amp?

Cheers,

Bob

On 21 Nov 2005 at 21:53, David Van Horn wrote:

{Quote hidden}

2005\11\22@043231 by Alan B. Pearce

face picon face
> I'm looking to make crenellations in the side of a PCB.
> That is, to have "half a pad" so that pins can be laid alongside the PCB
> and soldered into the circuit, rather than being threaded through a
> hole.
>
> Does anyone know how to do this without the mill putting copper kerf
> into the hole?

You may be able to do this by using suitable sized pads with the centre of
the hole right on the edge of the PCB, and carefully specifying to the PCB
house that you want to cut right through them.

2005\11\22@074437 by olin piclist

face picon face
David Van Horn wrote:
> I'm looking to make crenellations in the side of a PCB.
> That is, to have "half a pad" so that pins can be laid alongside the PCB
> and soldered into the circuit, rather than being threaded through a
> hole.
>
> Does anyone know how to do this without the mill putting copper kerf
> into the hole?

That's how I've done it.  Why do you care if the mill cuts copper as long as
the PC house is willing to do it?


******************************************************************
Embed Inc, Littleton Massachusetts, (978) 742-9014.  #1 PIC
consultant in 2004 program year.  http://www.embedinc.com/products

2005\11\22@074729 by olin piclist

face picon face
Bob Blick wrote:
> You need to make your pad U-shaped and leave clearance for the
> cutout.

Not in Eagle.  I've done this by making a normal pad, then adjusting the
dimension outline to cut part of it away.  The first time I did this I was
wondering whether the board house would complain, but the boards came back
exactly as expected with no comment.


******************************************************************
Embed Inc, Littleton Massachusetts, (978) 742-9014.  #1 PIC
consultant in 2004 program year.  http://www.embedinc.com/products

2005\11\22@113943 by Bob Blick

face picon face

Bob writes:
>> You need to make your pad U-shaped and leave clearance for the
>> cutout.

Olin writes:
> Not in Eagle.  I've done this by making a normal pad, then adjusting the
> dimension outline to cut part of it away.  The first time I did this I was
> wondering whether the board house would complain, but the boards came back
> exactly as expected with no comment.

You totally missed the point. David does not want to cut copper. So he
needs unusually shaped pads, which are certainly OK and supported by many
CAD packages, perhaps even low-end ones like Eagle, without having to
resort to creating fake pads with multiple copper objects.

Now that I've insulted Eagle, perhaps you will enlighten us as to whether
it can make U-shaped pads?

Cheerful regards,

Bob

2005\11\22@123624 by Darrell Wyatt

picon face

You can try a metal shear.  Sounds crude, I know, but
you use what's available sometimes.  Actually, it worked quite
well when I used it for cutting blank perfboards.  I don't know
if this is quite what you are looking for - Bear in mind that the
pads will probably get buggered up at the shear point.

D.



{Quote hidden}

2005\11\22@130718 by gacrowell

flavicon
face


> -----Original Message-----
> From: .....piclist-bouncesKILLspamspam.....mit.edu
> [EraseMEpiclist-bouncesspam_OUTspamTakeThisOuTmit.edu] On Behalf Of Olin Lathrop
> Sent: Tuesday, November 22, 2005 5:48 AM
> To: Microcontroller discussion list - Public.
> Subject: Re: [EE] Notched PCBs
>
> Bob Blick wrote:
> > You need to make your pad U-shaped and leave clearance for the
> > cutout.
>
> Not in Eagle.  I've done this by making a normal pad, then
> adjusting the
> dimension outline to cut part of it away.  The first time I
> did this I was
> wondering whether the board house would complain,

Some will, some won't.  It's useful to add a fab note telling them that
the routed board edge is expected to contact copper features in
(x-number) places.  That avoids your order being put on hold, weekend
phone calls, etc.

Gary Crowell, CID+
Micron Technology

2005\11\22@132059 by gacrowell

flavicon
face


{Quote hidden}

While he can make U-shaped pads, I don't think he is going to get a
U-shaped plated hole without running the routed edge thru it.  While I
think I can imagine a combination of drilling & routing that might
accomplish something like that, I'm pretty sure it would be cheaper to
just deburr the hole after routing.  OTOH, the cuts I've seen like this
have been very clean, so I don't know that there would really be a
problem.

Gary Crowell, CID+
Micron Technology


2005\11\22@152549 by olin piclist

face picon face
Bob Blick wrote:
> You totally missed the point. David does not want to cut copper. So he
> needs unusually shaped pads, which are certainly OK and supported by
> many CAD packages, perhaps even low-end ones like Eagle, without having
> to resort to creating fake pads with multiple copper objects.

That's not how I understood it.  I thought he wanted to create pads on the
edge of a PCB so that the pads are cut in half by the edge.  The pads would
be open sideways to the outside world.  Perhaps the OP can clarify?


******************************************************************
Embed Inc, Littleton Massachusetts, (978) 742-9014.  #1 PIC
consultant in 2004 program year.  http://www.embedinc.com/products

2005\11\22@201242 by Peter

picon face


On Tue, 22 Nov 2005, Olin Lathrop wrote:

{Quote hidden}

Aren't those pads on the side made such that the hole plating continues
on the edge to the full width of the pad ? That would not be done by
cutting there.

Peter

2005\11\22@211722 by David Van Horn

picon face

> That's not how I understood it.  I thought he wanted to create pads on
the
> edge of a PCB so that the pads are cut in half by the edge.  The pads
> would
> be open sideways to the outside world.  Perhaps the OP can clarify?

That's what I'm looking for.  The idea is that the connection is made by
wires that lay into the pads from the outside.

The problem that I'm seeing, is that the router shoves the kerf over
into the drill hole. Manually clearing them is possible, but not
practical.
I've seen this done on other systems, so I believe that it is possible
to do it in a practical manner.



2005\11\22@220929 by shb7

flavicon
face
Hi Dave,

I haven't read the whole thread but I did something like this recently, except I was soldering from SMT pads to a PCB laid on top of them. I put "fingers" on the edge of the pcb. I used http://www.pcbfabexpress.com

Sean



2005\11\22@223224 by Bob Axtell

face picon face
shb7@netzero.net wrote:

>Hi Dave,
>
>I haven't read the whole thread but I did something like this recently, except I was soldering from SMT pads to a PCB laid on top of them. I put "fingers" on the edge of the pcb. I used http://www.pcbfabexpress.com
>
>Sean
>
>
>
>  
>
I understand what you are trying to do, but why not actually use a round
thrupad as well as the flat surface? You will strengthen
your connection about 500%. That's what I always do.

--Bob

--
Note: To protect our network,
attachments must be sent to
KILLspamattachKILLspamspamengineer.cotse.net .
1-520-777-7606 USA/Canada
http://beam.to/azengineer

2005\11\23@073657 by olin piclist

face picon face
Peter wrote:
> Aren't those pads on the side made such that the hole plating continues
> on the edge to the full width of the pad ? That would not be done by
> cutting there.

The ones I made only had the hole plating in the hole.  The were just normal
round pads with plating sliced in half.

2005\11\23@075847 by olin piclist

face picon face
part 1 928 bytes content-type:text/plain; (decoded 7bit)

David Van Horn wrote:
> The problem that I'm seeing, is that the router shoves the kerf over
> into the drill hole.

I haven't seen that.  In fact my sliced pads were actually at the ends of
channels routed in from the edge, not at the edge directly.  I made the pad
hole just a little wider than the channel, and made sure the router stopped
just short of the center of the pad.  That way I got maybe a 2/3 ring of pad
and plated hole.  We are doing this because it will be a lot easier to
attach an assembly with pre-formed leads to the board by sliding it in
sideways then soldering it on.  So far we've only had a few prototypes
built, but none of the boards had any krud in the holes when they came back
from the PCB house.  I have attached a small piece of the Eagle board view.
Green is pads, red is top layer copper, and white is the outline the board
house mills the board to.


part 2 2466 bytes content-type:image/gif; (decode)


part 3 35 bytes content-type:text/plain; charset="us-ascii"
(decoded 7bit)

2005\11\23@082846 by Vasile Surducan

face picon face
On 11/22/05, David Van Horn <RemoveMEdvanhornTakeThisOuTspammicrobrix.com> wrote:
>
> I haven't seen this covered anywhere, thought I'd ask.
>
> I'm looking to make crenellations in the side of a PCB.
> That is, to have "half a pad" so that pins can be laid alongside the PCB

Are you working for HP? Only damn HP photo cameras have such cheap
connections between various sandwich boards inside...
The drill is necessary only if you expect to get the crenellation
shape using the drill itself. Which by the way it's clever. But will
request some cheating methodes for the DRC or a second cut.

cheers,
Vasile

2005\11\23@100447 by Mike Young

picon face
What's  the bigger picture around why you're doing this? Mechanical strength
is next to nothing. The hole plating is not bonded to the board substrate,
leaving only the pad's attachment to the board and the scrawny trace.

Is this a mezzanine between a daughterboard and the mainboard?

I'd been following the discussion with a faint air of disbelieve, "Nah. That
can't be what they're talking about..." And then I see in your picture that
it is.



{Original Message removed}

2005\11\23@104820 by gacrowell

flavicon
face


{Quote hidden}

That's neat.  I like it very much.  You are limited to fairly large
holes though, right?  .062" or so?  Will they do smaller diameter
milling?

One slight alternative I might suggest is to make the pad with no drill
at all, rather define the 'drill' as a plated slot that extends from the
center of the pad to beyond the board edge.  The board milling then just
cuts straight across the slot without deviating into the slot.  That way
the entire slot will be plated and there's no worry of edge milling
tolerance damaging the plaiting in the 'hole' area.  That would however,
leave plated material at the board edge (which may/may not be an issue,
depending on application), but you could eliminate that by deviating the
board edge mill slightly into the slot, beveling the corners.  

Gary Crowell, CID+
Micron Technology

2005\11\23@110236 by David Van Horn

picon face

> What's  the bigger picture around why you're doing this? Mechanical
> strength
> is next to nothing. The hole plating is not bonded to the board
substrate,
> leaving only the pad's attachment to the board and the scrawny trace.

There's a lot of them, and it's a client requirement.




2005\11\23@111302 by olin piclist

face picon face
Mike Young wrote:
> What's  the bigger picture around why you're doing this? Mechanical
> strength is next to nothing. The hole plating is not bonded to the
> board substrate, leaving only the pad's attachment to the board and the
> scrawny trace.

These pads will receive the leads for small helical antennas about 1 inch in
diameter.  These antennas are a separately built assembly.  They are a
carefully measured length of wire wrapped around a custom polyethalene
spindle which has its own mounting the PCB.  The antenna feed lines need to
be pretty exact, and are made from very stiff metal.  Trying to insert these
lines into holes while simultaneously aligning the spindle mounting parts
with the PCB is nearly impossible, especially when considering the
manufacturing tolerances on the exact position of the stiff antenna leads.

To solve this, we have the leads preformed so that their ends are at right
angles to the PCB.  They slide into the slots and are then soldered in place
by hand.  The spindle sort of snaps onto special holes in the PCB, and the
PCB and antennas are rigidly held separately by the case everything goes
into.  We don't need the leads mounted to the board to be strong at all.


******************************************************************
Embed Inc, Littleton Massachusetts, (978) 742-9014.  #1 PIC
consultant in 2004 program year.  http://www.embedinc.com/products

2005\11\23@112005 by olin piclist

face picon face
gacrowell@micron.com wrote:
> That's neat.  I like it very much.  You are limited to fairly large
> holes though, right?  .062" or so?  Will they do smaller diameter
> milling?

The routed channel I showed is .045" wide.

> One slight alternative I might suggest is to make the pad with no drill
> at all, rather define the 'drill' as a plated slot that extends from the
> center of the pad to beyond the board edge.  The board milling then just
> cuts straight across the slot without deviating into the slot.  That way
> the entire slot will be plated and there's no worry of edge milling
> tolerance damaging the plaiting in the 'hole' area.  That would however,
> leave plated material at the board edge (which may/may not be an issue,
> depending on application), but you could eliminate that by deviating the
> board edge mill slightly into the slot, beveling the corners.

I don't see how "the entire slot will be plated" in this case.  The routing
is done after plating and etching, so anything routed will not be plated
between layers.  In this case I don't want conductors extending to the edge
of the board, and what we have is pretty much what we want.  In the actual
boards, there is roughly 2/3 of a plated hole left.  That's plenty for
solder to flow around everything nicely.


******************************************************************
Embed Inc, Littleton Massachusetts, (978) 742-9014.  #1 PIC
consultant in 2004 program year.  http://www.embedinc.com/products

2005\11\23@115328 by gacrowell

flavicon
face


{Quote hidden}

Route the slots during the drill operation.  Plated slots are common,
but some fabricators might not like to do it.  As I said, I like what
you've got; just a suggestion.

Gary Crowell CID+
Micron Technology

2005\11\23@152047 by Peter

picon face

On Wed, 23 Nov 2005, Olin Lathrop wrote:

> Peter wrote:
>> Aren't those pads on the side made such that the hole plating continues
>> on the edge to the full width of the pad ? That would not be done by
>> cutting there.
>
> The ones I made only had the hole plating in the hole.  The were just normal
> round pads with plating sliced in half.

Ok. Was this enough to hold in a soldered pin ? Ime., such cut pads are
less strong than a 'wide' plated side finger. The next question would
be, is there a way to specify or order the kind of pad or finger which
is really metallized on the outside ?

Afaik, the technology for metallizing the edges is the same as the one
for making the holes but I suppose that the machine has a special holder
for the board and I think that there must be some way to specify the
mask for the edge since it would be covered in copper together with the
holes. I have only seen such pads on relatively expensive boards, so I
do not think one can order this feature for a small run. Exposing
photoresist on the edge must be a bear. They probably use silkscreening
of some sort for this. And I think that those boards were stamped, not
cut.

Also, would it be an option for the OP to specify side clip-on 'pins' as
used in certain modules instead of the cut pad ?

Peter

More... (looser matching)
- Last day of these posts
- In 2005 , 2006 only
- Today
- New search...