At 09:27 PM 1/15/2004, you wrote:
The "missing" hole is for a plastic locating pin in a blow moulded housing.
Hence no need for copper to allow for screw head size, as there is no screw.

I thought that was a possibility. No need for copper, but also, most likely, no harm. I would not make this an unplated hole unless maximum precision on hole size is important -- in which case you'll need to let the fabricator know that, they won't guess it. Fabricators routinely change hole sizes to a drill size that will reduce the number of different sizes needed for a board, provided the finished holes remain within tolerance, which is often +/- 0.003 inch.

Consider this: if you don't have a pad there, but you have a hole, does DRC verify that the hole doesn't take a bite out of -- or cut -- a trace? I don't recall a hole precision parameter in Protel, and this would be essential in doing a real DRC on this possibility. Having a pad makes checking automatic. And plating the hole keeps fabrication cost down; if it is a plastic pin and not a screw, the remaining argument, about a screw chewing up the hole plating and creating copper fragments that might do harm somewhere else, become irrelevant.

I'd make the pad diameter be at MMC for the hole.. Remember that plated holes are drilled oversize, typically 0.003, to allow for plating, maybe more because of the fabricator option mentioned above. Then the normal board clearance rule will guarantee no bites out of tracks.

And then you are dealing with a plain vanilla pad, nothing special about it. You don't need a special clearance rule unless you want to gain a couple of thousandths of an inch for track routing. It's simple.

In another post in this thread, single-side boards were mentioned. I've always designed single-sided boards as if they were double-sided; that way the same footprints can be used if desired. However, it is also routine to increase the pad sizes on single-sided boards to improve pad adhesion. Some of us will remember cut pads for ICs on Bishop Graphics decals; it is a deficiency in Protel -- albeit minor -- that the pad shapes are so severely limited. Cut pads were really necessary for single-sided design, because they allowed a trace between pads, while still having a larger pad area for adhesion.

The greater adhesion is necessary because hole plating with a top and bottom pad, covered with solder, act a like a rivet. Single-sided boards are most common with cost-critical consumer products, and what is the most common failure mode? In my experience, it is pad separation from the board at a place where there is some stress on the inserted part or wire, usually a connector that is held in place only by its pads. The pad separates and then the trace connecting to the pad cracks, resulting in an open circuit or perhaps an intermittent connection. A good designer will beef up the pads and will also attempt, if possible, to eliminate the stress on the solder joints, perhaps by gluing the connector down or with other mechanical steps.

A plot of the top side on a single-sided through-hole board would be the same as a padmaster; typically I wouldn't generate it (I'd eliminate it from the CAM setup, as well as any top layer related files unless they are to be used in fabrication.). If you want, you can disable the top layer in Protel, which I think would make the photoplot set come out correctly automatically when you automatically create the CAM setup. Or you can leave the top layer and use it for uninsulated jumpers, so that your schematic and PCB correspond (or you can put the jumpers on the schematic, which would have its advantages).

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Forum Guidelines Rules: * * * Browse or Search previous postings: *[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Reply via email to