Some questions regarding board design

Hi,

I have been designing boards for myself for quite awhile BUT I am
using a mechanical etch process to fabricate them on an IBC2222
BoardMaker machine. This process is quite different than going to a
vendor. My day has finally arrived that I have to rely on a vendor to
produce some one off boards for me. I have read the David L Jones
document available on the web but I still have a few questions I am
hoping that I can get some help on so here goes......

1.) How are non-plated thru holes handled? Do they still require a pad
ring to allow the plate thru process to work and then they get drilled
to the finished size.

2.) My CAD system is lacking in area fill capability. Do the PCB
vendors allow using a combined layer negative for the fill.planes and
combining it with a positive artwork layer to get the connections in.
Same goes for ground plane layers, do the vendors accept them as
negatives?

3.) What are typical clearances for solder mask artwork? Can the
openings go right up against the edge of pads? Can this artwork be a
negative too?

4.) How do I define the cut-out shape as the boards are circular so a
simple shear cross hairs in the corners won't do it. Do I provide a
layer with the shape to be cut-out?

5.) I require countersunk mounting holes around the periphery. How to
I indicate that? Would it be a see Note ### for more information?

Many thanks to all who are able to help me out.

regards,
al

 

[Rich Webb]

On Thu, 12 Mar 2009 06:00:28 -0700 (PDT), eyezkubed@yahoo.com wrote:

Hi,

I have been designing boards for myself for quite awhile BUT I am
using a mechanical etch process to fabricate them on an IBC2222
BoardMaker machine. This process is quite different than going to a
vendor. My day has finally arrived that I have to rely on a vendor to
produce some one off boards for me. I have read the David L Jones
document available on the web but I still have a few questions I am
hoping that I can get some help on so here goes......

1.) How are non-plated thru holes handled? Do they still require a pad
ring to allow the plate thru process to work and then they get drilled
to the finished size.

2.) My CAD system is lacking in area fill capability. Do the PCB
vendors allow using a combined layer negative for the fill.planes and
combining it with a positive artwork layer to get the connections in.
Same goes for ground plane layers, do the vendors accept them as
negatives?

3.) What are typical clearances for solder mask artwork? Can the
openings go right up against the edge of pads? Can this artwork be a
negative too?

4.) How do I define the cut-out shape as the boards are circular so a
simple shear cross hairs in the corners won't do it. Do I provide a
layer with the shape to be cut-out?

5.) I require countersunk mounting holes around the periphery. How to
I indicate that? Would it be a see Note ### for more information?

Take a look at the pre-order checklist and FAQs at
http://www.pcbexpress.com/index.php. That's just one vendor but the
general capabilities and limitations are similar.

You're probably far better off (in cost and in eventual satisfaction)
the less you depend on manipulation of your files by the board house.

It's possible to use tools like ViewMate http://www.pentalogix.com/ to
"swell" the pads in a Gerber layer to make a new Gerber for a mask
layer. Not available in the free version, though. Try 10 mils (0.01")
for your mask clearance.

--
Rich Webb Norfolk, VA

 

[John Devereux]

eyezkubed@yahoo.com writes:

Hi,

I have been designing boards for myself for quite awhile BUT I am
using a mechanical etch process to fabricate them on an IBC2222
BoardMaker machine. This process is quite different than going to a
vendor. My day has finally arrived that I have to rely on a vendor to
produce some one off boards for me. I have read the David L Jones
document available on the web but I still have a few questions I am
hoping that I can get some help on so here goes......

1.) How are non-plated thru holes handled? Do they still require a pad
ring to allow the plate thru process to work and then they get drilled
to the finished size.

My vendor says just to label them "NONPTH" on the drill chart. You
don't need a pad.

2.) My CAD system is lacking in area fill capability. Do the PCB
vendors allow using a combined layer negative for the fill.planes and
combining it with a positive artwork layer to get the connections in.
Same goes for ground plane layers, do the vendors accept them as
negatives?

Yes.

3.) What are typical clearances for solder mask artwork? Can the
openings go right up against the edge of pads? Can this artwork be a
negative too?

Yes it is normally a negative. Not sure about clearance - ask
them. Mine seem to increase the clearances themselves...

4.) How do I define the cut-out shape as the boards are circular so a
simple shear cross hairs in the corners won't do it. Do I provide a
layer with the shape to be cut-out?

I usually do it as part of the drill chart, just a thin line
whose center represents the edge of the board. I used to ask them what
router they use and carefully draw in a channel that wide, but don't
bother now. They seem to figure it all out themselves. You should ask
them though. They may need to leave little bits that keep the circle
attached to the rectangular panel.

5.) I require countersunk mounting holes around the periphery. How to
I indicate that? Would it be a see Note ### for more information?

Guess so, never tried asking for countersinking.

Many thanks to all who are able to help me out.

The Chinese vendor I use does each job separately, so it is no
problem. Some of the lower cost European and US services may offer low
prototype prices because they can combine your job as part of a larger
panel. They therefore have stricter rules about what you can and
cannot do while remaining in the low-cost scheme.

--

John Devereux

 

[qrk]

On Thu, 12 Mar 2009 06:00:28 -0700 (PDT), eyezkubed@yahoo.com wrote:

Hi,

I have been designing boards for myself for quite awhile BUT I am
using a mechanical etch process to fabricate them on an IBC2222
BoardMaker machine. This process is quite different than going to a
vendor. My day has finally arrived that I have to rely on a vendor to
produce some one off boards for me. I have read the David L Jones
document available on the web but I still have a few questions I am
hoping that I can get some help on so here goes......

1.) How are non-plated thru holes handled? Do they still require a pad
ring to allow the plate thru process to work and then they get drilled
to the finished size.

No pad required. Note in the Drill Drawing which holes are non-plated.
I assume they drill after the final plating process is done. We supply
a separate drill file for NPTH, but that isn't necessary.

2.) My CAD system is lacking in area fill capability. Do the PCB
vendors allow using a combined layer negative for the fill.planes and
combining it with a positive artwork layer to get the connections in.
Same goes for ground plane layers, do the vendors accept them as
negatives?

Ask your vendor. They should have the capability to merge layers, even
flip a negative, then merge with positive. I've done this in the early
days using PCAD.

3.) What are typical clearances for solder mask artwork? Can the
openings go right up against the edge of pads? Can this artwork be a
negative too?

Ask your vendor. A good vendor can hold 2 mil clearance. Don't use
zero or you will get mask on your pads. The clearance is for
registration issues.

4.) How do I define the cut-out shape as the boards are circular so a
simple shear cross hairs in the corners won't do it. Do I provide a
layer with the shape to be cut-out?

You can show this in the Drill Drawing. Show the board outline and
dimensions. Complicated outlines, I include a drawing of the outline
showing all the dimensions. Some places will route along an outline
you provide on one of the layers, good board houses will go off a
drawing. Shear cross-hairs aren't necessary. The board house will use
their own targets and drill holes to align the stackup. The final
board is routed out of the panel, not sheared.

5.) I require countersunk mounting holes around the periphery. How to
I indicate that? Would it be a see Note ### for more information?

Ask you vendor if they can do this. Put that in the drill drawing or a
separate mechanical drawing. Also, note it verbally in your readme
file that explains each layer name and how you want those layers
processed (copper weight, layer separation, material, special
features, layer merging, ...). We have a blind drill hole in one of
our boards thats done after the final lamination. They're pretty good
at controlling the depth.

Many thanks to all who are able to help me out.

Bottom line, you need to talk to your vendor. If they are a quick-turn
prototype house, much of what you want can't be done at cheap prices.
You'll need to resort to their full service offering.

regards,
al