Hi all, I'm working my way through transitioning from OrCAD 10.0 to 16.5.
I've started a new design and have a few questions regarding board outlines in OrCAD PCB Editor:
1) How can I create board oultines where the lines are not at 90degree angles?
2) How can I type in coordinate points for my board outline?
3) Is there a way to copy a board outline from an existing .brd file and paste it into an existing design? The Help -> Documentation mentions a "boardoutline import" which is supposed to be under File -> Import -> Board. This doesn't seem to exist and the command is not recognized when I type it into the console. Am I missing something? I did notice the documentation pulls up Allegro PCB Editor and there is no entry for OrCAD PCB Editor...
Add>Line, Options: Board Geometry / Outline, Line Lock set to "Off" for any angle, 90 or 45 are possible, also Arc can be used instead of Line for arcs.
Add>Line, Options: Board Geometry / Outline, type x<space><XLoc><space><yLoc><enter> at the Command line for each point, you can also use the incremental "picks", ix<space><xInc><enter> and iy<space><yInc><enter> if you prefer increments. Like:x 0 0ix 250iy 1000
and so on, you will need to add points until the outline is completed in one go. Entering co-ordinates won't care about the line lock.
You could display only the outline and Export a DXF from that and then Import the DXF to another BRD file. You could copy and rename the BRD file in Windows Explorer and load the Logic into it - in 16.6 one BRD file can be a template for another design.
Thanks, oldmouldy. I'm surprised under Setup -> Outlines -> Board Outline, the same options for line locks don't exist!
It sounds like unless the board outline is really complex, it will be easier just to construct a new board outline.
Is it true that it is impossible to copy shapes, lines, etc from design to another? This was a very normal part of OrCAD 10 which I miss. I can't even find a way to open 2 designs simultaneously just to visually compare them.
You will find many things you miss from the old program.
You can not open two files at once. You shouldn't have been able to do it in the old one either, but you could. I had a designer at one time who kept opening two files at once and saving the wrong one................
Can you not do a file>export>sub-drawing of the outline in orcad? That's an easy solution in Allegro.
Actually you can open two designs if you are running Allegro PCB Editor.
Make sure to also have an install of OrCAD PCB Editor, even if you don't have a license.
You can open open OrCAD PCB Editor in demo mode and have the other board open in Allegro PCB Editor.
I do this a lot to compare changes between the same boards.