Hi every one
I have routed PCB board .brd file (no schematic). I want to edit some components footprint like capacitor and diode place on the board have no polarity. Any body have knowledge about the procedure to edit the already placed and routed footprints.
In reply to Bonz:
One thing more I have only .brd file no components library. Can you describe the step by step procedure from open the .brd file in ORCAD, generate library, edit the component, and replace the component.
Another thing I export the library but guide me where this library is place to interface with .brd file.
In reply to AamirZ:
Thanks for your the link. I have a this book, but not completely guide me about my problem. I sovle the problem with the help this book "Complete PCB Design Using OrCAD Capture and PCB Editor-VINY.pdf" this is very helpful.
If it were me...
1) Save a copy of the brd
2) File export placement
3) edit the placement.txt file created. Find U29 and update the footprint to what you want.
4) import the updated placement.txt back into the brd file.
hope that helps.
I'm unsure why it should be any different than placing the D2PAK. Nonetheless...
Dawn proposes a simple solution (though I can't vouch for its success because I've never done it).
If it were me, I'd delete U29, place a TO263 then go to the toolbar within PCB Designer to "Logic > Assign RefDes", specify U29 in the options panel and left click on the new TO263 package.
Thanks Bonz, when i do your define process following error is shown
For refdes 'U29' symbol 'TO263-3' is not legal for placement layer. Check ALT_SYMBOL and ALT_SYMBOL_HARD property settings.
In reply to DawnC:
Do you have the TO-263-3 footprint defined? A quick test, do a Place Manual (Advanced tab make sure "librry" is selected). Placement List pull down to Package Symbols. Do you see the TO-263-3?
Just export your library in the path where is you brd file by using the File-->Export--Libraries, check all the options, let the dot in the directory line and click OK. You obtain all your packages and pads file...
Export the netlist by using the File-->Export-->Netlist/w properties, edit the netlist.txt file then replace your package component in it. The file structure is easy to understand. Use the file import-->Logic, folder other and check supersede all logical datas, the clic on import...
You will see the changes immediately.