Hi, Matt; Let me ask first how you created the circular board with the segmented Planes. Did you draw a circle using a 50mil arc of, say, Internal Plane 1, then add 50 mil Tracks of Internal Plane 1 copper to force segmentation of the circle? If so, you are creating endless headaches for yourself, as Protel's DRC machine will probably not be able to correctly resolve what it will interpret as many overlapping physical Planes and many Planes connected to overlapping Nets.
A better (maybe the only) way to place multiple planes is to: 1- Create a physical board using an arc of say 1mil width on the Keepout Layer, having the arc laying on the edge of the desired finished board. 2- Create a Design Rule for Power Plane Clearances of , say, 20mils. This will insure that all copper is at least 20mils inside the boundary of the physical board. Fabricators are generally happy with 20mil plane clearances, though they will work to clearances much tighter if requested to....but their fallout will be higher during test and they will charge accordingly. 3- Load your Netlist. You can leave the components unlocated for now. 4- Use Place Split Plane to add each desired Plane, assigning it to the proper Net and Layer using the dialog box for each Place Split Plane. If for instance you want a "pie-shaped" board, begin each Plane at the center of the "pie" and extend the plane _beyond_ the keepout arc so that all portions of the Split Plane Boundary are outside the arc. Then move to the next "wedge of the pie" and Place the next Split Plane. Extend _all_ Split Planes as you add them to extend beyond the Keepout arc. You can place the boundary track of one Split Plane directly on top of the boundary track of another Split Plane, though you don't _have_ to. You will be able to edit the Plane segments later if needed by using Edit/Move/ SplitPlaneVertices; when it asks you to click on the desired plane, the planes boundaries will be highlighted and can be clicked on to grab the vertices etc. NOTE: Do Not Overlap Planes! Mother Protel doesn't like it. You should wind up with a bunch of Planes whose edges either coincide or lie adjacent to each other. Any copper not enclosed by a Plane boundary will be dead copper, and although not electrically connected to circuitry, may act like an antenna. Try to avoid dead copper areas. If you double click on any Plane segment, the resulting edit dialog box should show you the plane as having the correct Layer and Net. Note also that the width of the track used to Place the Plane is in effect the width of the boundary "void" in the copper plane when the Gerbers are generated. So, two adjacent planes having 20mil boundaries will generate Gerbers having the planes separated by 20mils total. On the clearance issue, best to set up the Design Rules for Power Plane Clearances and let Protel manage copper setbacks during Gerber generation. To try to do it manually is frustrating and nedlessly time- consuming. Keep in mind that the board house only sees Gerber data and won't be confused by the means used to create the data. As an aside, Polygon Pours are placed in a similar manner. However, their screen presentation is very different, being displayed in Positive rather than Negative copper. You can use both on the same board, but NOT on the same layer. A Plane Layer must have ONLY the Plane on it. Anything else is used to indicate a Plane Keepout Object unless electrically connected in the Netlist. DO NOT try to form conductors in Plane Copper by forcing voids to create traces or Planes-within-Planes. Protel becomes very troubled, and the DRC will NOT report these "pseudo-objects" correctly. If you must mix "Plane"-type areas with Track-type areas on a given layer, use Polygon Pours and Tracks on a Mid Layer. Good luck! Brian Foothill Services LLC At 03:02 PM 5/19/02 -0700, you wrote: >I'm working on laying out my first board with power >planes and I have a few questions. > >1. I placed an arc on the plane (my board is circular) >to form a circle all the way around the edge of the >board. The idea is to keep the plane away from the >edge of the board. The assigned net for the arc is >"No Net". Is this the correct procedure for keeping >the plane away from the edge of the board? > >2. The arc is 50 mils wide. Since I placed the arc >directly on top of the board outline, I expect to get >25 mils of clearance from the board edge to the plane. > In general, is that enough clearance? > >3. I have split the plane into multiple nets. The >tracks that indicate the boundaries are 45 degree and >90 degree tracks. Recall I have an arc on my board >edge. Because the 45/90 tracks and the arc are not >"compatible", the tracks extend outside of the arc to >avoid tiny slivers of plane near the board edge. Is >there a better way to do this? For example, can I >define the regions with mostly 45/90 tracks but add an >arc at the board edge to complete the region? Will >the way I have done this likely confuse the board >house? > >I'm using Protel 99 SE sp6. > >Thank you, >Matt > >__________________________________________________ >Do You Yahoo!? >LAUNCH - Your Yahoo! Music Experience >http://launch.yahoo.com > * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
