 |
 | 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 / December 2004Protel 99SE
I'm drawing up a power circuit, the footprints and all the rest are all ok however when i update the PCB there are errors generated around the diodes saying: ERROR: Node not found. When i take the diodes out the circuit updates without error. All the foorprints libraries are available to the PCB. Any help would be great, Thanks Graham Taitt >I'm drawing up a power circuit, the footprints and all the rest are >all ok however when i update the PCB there are errors generated around >the diodes saying: ERROR: Node not found. When i take the diodes out >the circuit updates without error. All the foorprints libraries are >available to the PCB. Any help would be great, Thanks >Graham Taitt Check that the pin numbers on the schematic symbol and the PCB footprint agree. You will likely find that the schematic pins are A and K while the PCB pins are 1 and 2 (or something like that) - edit the schematic symbol or the footprint (or both) to make the pin numbers match. It appears that Protel's schematic library creators and their PCB counterparts weren't permitted to collaborate - there are many such discrepancies in the libraries. Also - check hole sizes on the PCB. On many footprints, the holes are too small for my liking (and sometimes too small for the intended part - particularly the .025 square post headers).  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 > >I'm drawing up a power circuit, the footprints and all the rest are > >all ok however when i update the PCB there are errors generated around [quoted text clipped - 16 lines] > too small for my liking (and sometimes too small for the intended part > - particularly the .025 square post headers). On the diodes the foot prints are numbered 'A' and 'C' on the schematic they are 1 & 2 so you will need to change them. Hello Graham, > I'm drawing up a power circuit, the footprints and all the rest are > all ok however when i update the PCB there are errors generated around > the diodes saying: ERROR: Node not found. When i take the diodes out > the circuit updates without error. All the foorprints libraries are > available to the PCB. Any help would be great, Thanks > Graham Taitt take care that you use the "Pin Number" from the schematic symbol as the reference to create the pad designators in the footprint! Although the name is listed above the number of the pin, it is ONLY the number that Protel uses to link schematic symbols and footprints. There is NO WAY tho change this behaviour. >Hello Graham, > [quoted text clipped - 12 lines] >footprints. >There is NO WAY tho change this behaviour. I have also seen where someone had the lead (or pins) backwards. It looks "ok" on the schmatic because the display pin and name are turned off. But, its not hooked up to anything.... |
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.