Updating multiple comonents simultaneously in Orcad Capture

[ewall...@gmail.com]

I have been given a legacy product that has had a series of updates "hand annotated" on a printed version of the schematic.

I have been asked to bring the out of date electronic version up to date with the hand annotated version as we have a major modification that needs completing due to component obsolescence.

A major problem I am facing is there are some minor changes that affect many components. For example there are 53 identical capacitors who's values have been changed.  I'm trying to find a way to update all 53 capacitors in one go instead of opening all 53 instances on the schematic and making changes individually.  Is this possible?  I imagine something like a BOM type listing where I can make changes that are then back annotated onto the schematic. 

I hope I have been able make myself clear.

Thanks. Ed

[lwdco]

Hi Ed,

I think you want to use the Edit Object Properties function (select .dsn file on the .opj page, then Edit Menu -> Object Properties).  It will give you a list of everything and you can edit most properties, including part values, which will then be updated on the schematics.  But before you do that, please consider using the BOM Include File function.  It lets you rename items and add as much detail as you want in your BOM, based on combinations of the individual part values.  As you are already finding out, updating the schematic is time-consuming and, if not performed perfectly, can screw up your reference netlist.  For example, simply calling a cap 0.1uF on the schematic, while the include file has the WVDC, Manufacturers' part numbers (and alternates), footprint, etc. referenced to the 0.1uF part.  Then, when you get a BOM change for obsolescence, you only change the include file (a simple text file) and re-run the BOM process -- your schematic and netlist remain untouched.  Those are also vital to maintain a system that has obsolescence problems and you don't want to accidentally mess them up while just changing a part number.

I attached a small document I wrote long ago on how to use an include file to stuff different assemblies.  I know this isn't what you are looking for, but it also provides an introduction into using the include file on a simple design so you can see how it works.  The OrCAD screen may have changed since then (and I haven't used the include feature on version 17+), but the basic include file format and setup is there.  If you need more info, please contact me...
 
Best of luck to you!
David

[lwdco]

I just noticed that the schematic in the PDF is missing all the text.  Here it is...

[Ron_O]

An easy way to do this is to use the Browse Properties spreadsheet at the root schematic or design level. To do this, select the *.dsn entry in Project window; in menu, click Edit, then Browse, then Parts, use Instances. The Browse Parts spreadsheet will appear. Select the top entry, press shift + End to select all items; press Ctrl-E. This will bring up the Browse Spreadsheet for all part properties in the design. From here you can go to the column you want to edit, select the entry, click Copy, then select another entry or entries (use Ctrl or Shift while clicking to select multiples) and then Paste to update those entries.  To keep the Ref Des in view, squish the columns by hovering mouse over the column header separator until it changes to a plus with arrows, click and drag it to the left until it meets the other separator. When you are done edits, click OK and close the first Browse window to complete edits.

The other way to do this is to export the BOM to Excel make edits, then generate a backannotation format file to load new values back into Orcad. This is a bit trickier as you need to create the correct BA format for Orcad to read. If you are good at Excel it can be done with just simple commands.

RonO