At 10:54 PM 1/14/2004, Drew Mills wrote:
I completed the layout of a small PCB (99SE) designed for enclosure in a
moulded case, then realised I needed an additional hole for mechanical
locking. So I added a free pad, with no copper - just the correct hole size.
Everything looks good in PCB, but now, when I output the gerber files I need
to panelise in Camtastic, there is no trace of the hole, except for a tiny
pin-prick on the top soldermask layer. Why is it so?


Here is what is going on. The soldermask layer is a calculated layer, it is generated from the pad size. In order to make a "pad with no copper" you made the dimensions of the pad zero. The solder mask is generated as an oversize from the pad size, so that it clears the pad. That's what is creating the "pin-prick," it would probably be a pad with a diameter of twice your solder mask clearance, perhaps 20 mils, about the size of a pinhole.


What did you expect to see on the gerbers?

I usually create mechanical holes as a pad with clearance, the pad being made the size of, for example, the MMC of a screw head for a screw going into the hole. That way my DRC guarantees that a screw can't bite into a track.... I've often left it just like that, but there is some thought that hole plating in mounting holes can create problems with fragments of copper. I'm not sure how much of a real problem it is, but if you don't want the hole plated, then you can request that from the fabricators (it may be enough to uncheck the Plated box on the Advanced tab of the pad edit dialog). Unplated holes can be a bit of extra cost, they have to be treated specially.

If you don't want the pad to be there, you can made the pad size smaller than the hole. I wouldn't make it zero, though. Invisible pads give me the creeps.... If you want solder mask to be clear of the hole, you can set a rule for that pad. You might give the pad a name like "MH" for "mounting hole" and then you can create design rules for the pad Free-MH. This would allow you to define sufficient clearance rules to prevent possible shorts, if that is relevant for this design, as well as a solder mask expansion that will make the solder mask opening be larger than the hole.





* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
*
* To leave this list visit:
* http://www.techservinc.com/protelusers/leave.html
*
* Contact the list manager:
* mailto:[EMAIL PROTECTED]
*
* Forum Guidelines Rules:
* http://www.techservinc.com/protelusers/forumrules.html
*
* Browse or Search previous postings:
* http://www.mail-archive.com/[EMAIL PROTECTED]
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Reply via email to