At 07:00 PM 5/18/2006, [EMAIL PROTECTED] wrote: >When I do a polygon plane pour and I set the clearance to 0 mils the pour >leaves large square gaps around my mounting holes.
You did not state what track width you are using to pour. >I need a solid plane because I am using it is as a ground plane for an >antenna. If I set the clearance to 1 mil then the plane no longer has large >gaps but has a small 1 mill gap around my mounting holes like it should but >I don't want that 1 mil gap. Why does it work with 1 mil but not 0 mil >clearance. 0 mil clearance is impossible if Protel thinks it is supposed to keep it from shorting. If your mounting holes are not assigned the plane net, Protel is not going to pour the plane over it. If it did, this would create a pad and a plane, in electrical contact but with different nets. No. No. Not allowed. (There are sometimes situations where you want this, most notably when building high-frequency copper "components." There are then ways to trick Protel into allowing it, but that is beyond the scope of this post. (DXP has a more direct method of allowing such "shorts" but it can be done in any version of Protel, though it helps to have microinch resolution....) >I can get around this by placing my ground plane and then adding my mounting >holes later but I would rather my polygon worked properly so I don't have to >move my mounting holes every time I "rebuild" my polygon. There are several ways to do this. First of all, you could use vias instead of mounting holes. If you put the plane down first, then pop the via down, it will assume the plane net and it will stay that way. But I don't like to use vias for fixed pad locations. Vias are not meant to be fixed to a particular location. You could put down pads for the mounting holes, but they might lose the net when you reload nets or synchronize. What I recommend, and what I always did, was to create a schematic symbol and a footprint for mounting holes. I put them on the schematic if I want them connected to ground. (You could also use this to call out mounting hardware on a bill of materials....) If you have the symbol and the footprint, the mounting holes will be connected to the plane. If you want a solid connection, you can control that with the Rules; I think thermal relief may be the option. If you want to use free pads, they might keep the net -- I forget -- but in any case you might want to set a rule. If you give the pads the name MH, you can then set a rule for Free-MH which will tell Protel to make a solid connection instead of a thermal relief. But I think it is safer to use a schematic symbol/footprint. In general, it is better to drive design to the extent possible from the schematic. About pours: generally the best setting for pour grid is zero. This is not the same thing as clearance. Normally, the grid will be the distance from centerline to centerline of tracks, but if it is set to zero, the programmers correctly recognized that someone doing this would not want an infinite number of tracks, so the made the program use the track width as the separate. Makes the most efficient pours. But if one is possibly worried about roundoff error and the like, then you could set it to a mil less than the track width, or something like that. There is no reason for overkill, unless you see some pour artifacts, due to various limitations on where you can pour and the line widths. I'm a bit puzzled that you got square openings with a setting of 0. Normally, Protel will surround a round pad with an arc or with an octagon. However, if you used square pads for mounting holes (why?), this is what you would see, and especially if you are using fat pour track. ____________________________________________________________ You are subscribed to the PEDA discussion forum To Post messages: mailto:[email protected] Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/[email protected] Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/[email protected]
