Re: [PEDA] Find and delete Tracks without net
> thanks for the answer, but Edit > Select > Net > clicking on a > No-Net-Track got > no effekts on my Design, huh!?! It works well when I choose an other > net. > Andys way helped me to select the tracks, I had to check "same layer" > to > prevent that Keepouts and Mech where chousen. > Gisbert, thanks for your answer, but there are nets on the components > I wanted > to stay and run to the other components behind them... Another method is to create a class of all nets (after you've updated the netlist). Select all tracks on top and bottom layers and then use the class to unselect the ones with nets, leaving the ones without. Steve. == Steve BaldwinElectronic Product Design TLA Microsystems Ltd Microcontroller Specialists PO Box 15-680, New Lynn http://www.tla.co.nz Auckland, New Zealandph +64 9 820-2221 email: [EMAIL PROTECTED] fax +64 9 820-1929 == * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Find and delete Tracks without net
[EMAIL PROTECTED] schrieb: > > Hi Waldemar, > > I tried this Edit > Select > Net > clicking on a No-Net-Track > Clear > and oops, all tracks and vias with No Net diappeared in my PCB. > I manually changed them from different nets to No Net before, just as a test. > > I hope this will fit for you > > Mit freundlichen Grüßen > > Matthias Trebeck > > Infineon Technologies AG > Automotive Industrial > AI MC AC EMC > > fon: +49 89 636 83244 > fax: +49 89 234 723831 > > mailto:[EMAIL PROTECTED] > > VISIT US AT: http://www.infineon.com Matthias, Andy, Gisbert thanks for the answer, but Edit > Select > Net > clicking on a No-Net-Track got no effekts on my Design, huh!?! It works well when I choose an other net. Andys way helped me to select the tracks, I had to check "same layer" to prevent that Keepouts and Mech where chousen. Gisbert, thanks for your answer, but there are nets on the components I wanted to stay and run to the other components behind them... Thanks to all. Waldemar * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Find and delete Tracks without net
This is what I did to delete old tracks from components that had been deleted: 1. Design, Netlist Manager, Menu, Update Free Primitives from Connected copper (this sets the tracks to No Net, but it doesn't completely forget about the old net so a global edit won't work) 2. Save the pcb file and close it. Then reopen it. (this seems to reset the net name so all the No Net are now accurately tagged as No Net) 3. Edit a No Net track and Global Edit to search for same net. It should now find all No Net tracks (including those on Mechanical layers and such so you may want to limit the search by layers also). 4. Check the selection and delete it. Andy Lintz > Hello out there, > > I am currently working on a design based on an older one. There are a lot of > parts in the Schematic that should disappear. After deleting them in the > Schematic I updatet the PCB and found, naturely, a lot of tracks with no Net. > Now here is my Problem: trying to select them with "Global Edit" to delete > them, I discovered that these function only select the tracks who once belonged > to the same net. Other "No Net" tracks are not touched. Is there a way to > select/delete al tracks without a net? > > I would appreciate your help > > Waldemar > * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Find and delete Tracks without net
Hi Waldemar, I tried this Edit > Select > Net > clicking on a No-Net-Track > Clear ...and oops, all tracks and vias with No Net diappeared in my PCB. I manually changed them from different nets to No Net before, just as a test. I hope this will fit for you Mit freundlichen Grüßen Matthias Trebeck Infineon Technologies AG Automotive Industrial AI MC AC EMC fon: +49 89 636 83244 fax: +49 89 234 723831 mailto:[EMAIL PROTECTED] VISIT US AT: http://www.infineon.com > -Original Message- > From: Waldemar Kulajew [mailto:[EMAIL PROTECTED]] > Sent: Thursday, December 13, 2001 1:09 PM > To: ProtelForum > Subject: [PEDA] Find and delete Tracks without net > > > Hello out there, > > I am currently working on a design based on an older > one. There are a lot of > parts in the Schematic that should disappear. After deleting > them in the > Schematic I updatet the PCB and found, naturely, a lot of > tracks with no Net. > Now here is my Problem: trying to select them with > "Global Edit" to delete > them, I discovered that these function only select the tracks > who once belonged > to the same net. Other "No Net" tracks are not touched. Is > there a way to > select/delete al tracks without a net? > > I would appreciate your help > > Waldemar > * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
