I've dealt with a similar problem in the past. I exported the PCB as ASCII format, opened it up in Notepad and did a search for Polygon. I then deleted the offending one (with vertices in the negative region).
This works especially well if the Polygon is a 'phantom' one i.e. invisible. It was a while ago, so my details may be sketchy, but definitely on track if the Select-Drag method fails... TC -----Original Message----- From: [EMAIL PROTECTED] [mailto:[EMAIL PROTECTED] On Behalf Of Darcy Davis Sent: Thursday, 11 November 2004 4:41 AM To: PEDA (E-mail) Subject: RE: [PEDA] HOW to DELETE parts, etc ,in the negative regions? Board Crashed! See answers below... Darcy Davis Design Engineer, Dynastream Innovations Inc. -----Original Message----- From: [EMAIL PROTECTED] [mailto:[EMAIL PROTECTED] Behalf Of Leif Erickson Sent: November 10, 2004 10:20 AM To: [EMAIL PROTECTED] Subject: [PEDA] HOW to DELETE parts, etc ,in the negative regions? Board Crashed! Hi there, Having phun with Protel 99, and have a major problem! I have some parts of a polygon under the zero line on the system, showing up in the negative quadrant areas in DRC. I deleted one, and apparently not all of polygon was removed during a selection and cut process. Now it shows up in DRC. HOW DO YOU get to them!?!?!?!?!?! 2 of us have crashed databases trying to fix it [Darcy] Sounds like a well known Protel bug. Try the following: 1) Design->Options->Layers: Turn all layers on. 2) edit->select->all 3) edit->deselect->inside area: Draw a box around your PCB (and any overlay/mechanical layers) to deselect it. 4) view->zoom out: repeat until you are fully zoomed out. 5a) edit->move->move selection: click and drag your mouse till you see the bounding box for your "move." Move the offending parts into the document area. or 5b) If you know you don't need the parts/primitives, hold down the shift key and press delete. The gerbers won't plot, saying film is too small! Ends up being a 36 MB file after trying to save during the crash/ignore crash warnings, and is not right after that. [Darcy] Once you get the offending primitives taken care of, the Gerbers should generate OK. How can you copy a pcb board, just the traces and parts, so to leave behind the parts outside the board, and below the 0 line, and put it into another clean database? Tried doing the schematic first, but inside the original database, and made a new ddb file for the new board. Tried doing just a pcb copy, and still have problems...........netlist won't see connected tracks, puts up rats nests, wants to put rooms on the pcb, and shows some trace errors, still not sure of........ [Darcy] You shouldn't have to do this if you get the steps above to work. If for some other reason you would like to do a copy-paste...When you do a simple copy-paste, Protel "forgets" the net of all pasted primitives (tracks, arcs etc). You must do a "edit->paste special" and select "keep net name" for this to work. I'm guessing Protel tries to add rooms because you tried to synchronize the PCB (with the schematic) and left "generate component class..." and "generate net class..." selected. What CAD system won't let you go into negative territory, if it has 3D capabilities? Or is there a 'trick' to it? [Darcy] In a way, Protel will let you go into negative territory. You can set the relative origin anywhere you like in the workspace (edit->origin->set & select the new location). Anything to the left or below the new origin will have negative coordinates. However, the symptom you are seeing is components/primitives that have been accidentally moved off the workspace. This is a bug where Protel allows you to move something off the screen if it happens to be selected while you are moving some other selected parts. Thanks for ANY HELP!!! [Darcy] You're welcome! Leif Erickson ____________________________________________________________ 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] ____________________________________________________________ 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]
