At 04:49 PM 6/4/2002 +0300, EDA Software Technical Dpt. wrote:
>My PCB file contains Polygon Plane with 5 mils Clearance from the 18 mils 
>pads.

Ouch! 5 mils clearance from a plane is much more difficult to fab than 5 
mils clearance between ordinary objects, because the plane clearance is 
*everywhere* within the plane. I would normally set a higher clearance for 
plane pours than for ordinary primitives (the Rules make this possible now, 
in Protel 98 it was necessary to pour with the larger clearance and then 
change the rules for the rest of the board).

If I need to get plane track between pads and this requires 5 mils 
clearance, then I might add pieces of track to create the connections. Note 
that such connections may also be made with thinner track than one would 
otherwise use, since the failure of an occasional connection like that is 
not serious, provided that the connections are redundant.

I'd more normally use a 12 or 15 mil clearance for polygons from pads, 
though one might go down from there, especially if the board has fine 
clearances in general; i.e., I might use 10 mils on a 6 mil board.

>When I create the gerber file the clearance ring around the pads on the 
>plane appears
>to be polygonal at the Gerber file (small lines "emulating" a cicle) and 
>not circular
>as it is on PCB.

As another pointed out, we can now tell that you have "software arcs" 
enabled in your gerber settings. This causes the arcs to be drawn with 
straight line segments, instead of using the newer gerber arc command.

>!!!!  NOTE:  !!!!
>In the Polygon Plane properties dialog, at the ''Surround pads with''  option
>I have select Arcs instead of Octagon.

Yes; if you selected octagons, they would be drawn with eight pieces of track.

>I try to convert the polygon plane to a set of primitive objects by selecting
>Tools  Convert  Explode Polygon to Free Primitives but the problem 
>remains the same
>when I create the Gerber file.

Right. It has nothing to do with the fact that it is a polygon, but only 
that the polygon pour routine creates arcs or octagons, you had it set for 
arcs (which is generally the best setting.)

>What I found is that the voids on a Polygon Plane are converted to the 
>Gerber file as small polygon lines.

You mean "arcs," not "voids."

>Other programs like Or-CAD, convert the Arc or the Circle exactly as Arc's 
>or Circle's in the Gerber file
>without using the small polygon lines.

Other recent CAD programs have -- or should have -- the option to do it 
either way, just like Protel.

>  Is there a way or a workaround in order to solve this problem?

As was stated by Mr. Hendrix, just change the setting of your gerber 
control file.

CAM Outputs for ..../
gerber file, default name Gerber Output 1/
rt.click/
Properties/Advanced/uncheck "use software arcs"

I use software arcs, but that may simply be an old habit, besides being the 
default, if I am correct.

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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/proteledaforum@techservinc.com
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Reply via email to