 |
 | Home | Contact Us | FAQ | Search & Site Map | Link to Us |
 | Sign In | Join | Other 45 Sites in Network |
| HomeDiscussion GroupsElectronicsBasicsRepairDesignCADComponentsEquipmentElectrical Engineering ElectronicsKB.com Contact UsLink To UsSearch & Site Map |
Electronics Forum / CAD / April 2005How to solve Protel "Warning - net contains unplated pads" ?
Dear Sir: When I DRC in Protel DXP I get much this message "[Un-Routed Net Constraint Violation] PCB1_998.PcbDoc Advanced PCB Net DSP_AAOE Warning - net contains unplated pads " Someone can help me? thanks a lot! > Dear Sir: > When I DRC in Protel DXP I get much this message [quoted text clipped - 3 lines] > > Someone can help me? thanks a lot! I suspect that your routing involves a track that passes though a pad from one layer to another. Verify that the pad(s) involved are plated through. Graham Holloway WPS/Accuphon Audio >Dear Sir: > When I DRC in Protel DXP I get much this message [quoted text clipped - 3 lines] > >Someone can help me? thanks a lot! Find the guilty pads and make them plated.... In Protel, even surface mount pads must be declared as "plated", with a hole size of zero.  SignaturePeter Bennett, VE7CEI peterbb4 (at) interchange.ubc.ca new newsgroup users info : http://vancouver-webpages.com/nnq GPS and NMEA info: http://vancouver-webpages.com/peter Vancouver Power Squadron: http://vancouver.powersquadron.ca Thanks Graham Holloway and Peter Bennett. The problem had solved just as you said. I have a new problem in DRC message "Warning - Pad/Via touching plane splitting primitives" Although I can disenable this option in DRC'option,But I want to know if this is a really problem. Can someone give me some advisement. Thanks you will have to look and see if its a problem. Usually they aren't, but its best to move the split plane boarder by 10 thou to get rid of the error so the next guy doesn't get it too. And you should never disable DRC options.. except for component clearance and acute angles. Simon > Thanks Graham Holloway and Peter Bennett. > The problem had solved just as you said. [quoted text clipped - 4 lines] > if this is a really problem. > Can someone give me some advisement. Thanks >you will have to look and see if its a problem. Usually they aren't, but >its best to move the split plane boarder by 10 thou to get rid of the error >so the next guy doesn't get it too. > >And you should never disable DRC options.. except for component clearance >and acute angles. It is sometimes impossible to get rid of all DRC errors. It is OK to have some on a finished board, as long as you know _why_ they are there, and are sure the board is the way you want. Having DRC errors does not prevent you from finishing the design process and producing Gerber and drill files. SignaturePeter Bennett VE7CEI email: peterbb4 (at) interchange.ubc.ca GPS and NMEA info and programs: http://vancouver-webpages.com/peter/index.html Newsgroup new user info: http://vancouver-webpages.com/nnq True.. I often have 4 or 5.. but as you say.. each is documented. One thing I'd like to see in the schematic ERC is the ability to put a limited "no-erc" marker.. for example.. "no-erc-if-pin-not-connected" so that anything other than not connected is an error.. in fact.. the pin connected is also an error (invert the warning status) Simon > >you will have to look and see if its a problem. Usually they aren't, but > >its best to move the split plane boarder by 10 thou to get rid of the error [quoted text clipped - 9 lines] > Having DRC errors does not prevent you from finishing the design > process and producing Gerber and drill files. Hey Simon, Peter, Are you forgetting something or has it been corrected in DXP ( and does the user have the DXP SP# that solved the issue). The connection issues with pads or vias on a split plane boundary? It either doesn't connect or shorts the two split planes together, remember? Then considering the split plane has calculated negative image connections and ties you can't actually get a true DRC determination on the issue. The original poster needs to know precisely where that DRC is originating (or multiple locations) and then either fix it by moving the split plane boundary or at the very least manually inspect the Gerbers very closely at those locations to make sure there isn't an unexpected disconnect or short at those points. I would go for moving it rather than waiting for Gerbers and then finding out you had to move it anyway after it means more work to move it. Or he could test the Gerbers now and pray it didn't change at all in the final board because of some further interactions with other file details. SignatureSincerely, Brad Velander > True.. I often have 4 or 5.. but as you say.. each is documented. > [quoted text clipped - 4 lines] > > Simon good point.. I've never seen this particular bug as I always make sure there's no plane connected via thru a split plane boundary. 99SE suffered a similar fate from memory with direct connected vias. Simon > Hey Simon, Peter, > Are you forgetting something or has it been corrected in DXP [quoted text clipped - 28 lines] > > > > Simon |
Reply to this Message |
 Sign In
 Join
 My Latest Posts My Monitored Threads My Blog My Photo Gallery My Profile My Homepage Start New Thread Enable EMail Alerts Rate this Thread
|
©2009 Advenet LLC Privacy Policy - Terms of Use
This website includes both content owned or controlled by Advenet as well as content owned or controlled by third parties.