Database comparisons - Version 13 to Version 15

Kory,

There is a design_compare utility bundled in the software. This utility will import two (or more) different XML files and compare the results graphically. Signal names can be different but if the contents are logically equivalent, it resolves them as being the same. It works very well.

The structure of these xml files is fairly straight forward. There is a nets section and packages. Here's a snippet.



CRK_SCL_RX_N
R3.2
U3.11
J6.B5

CRK_SCL_RX_P
R3.1
U3.12
J6.B6

...
RM1005
RESISTOR_2PIN-/03,200K,1%,0.1W-0.1W,1%,200K
R17


RM0502
RESISTOR_2PIN-/01,7.32K,1%,0.02W-0.02W,1%,7.32K
R15


...


So the trick here is to convert your 13.x and 15.x pst files to xml. The File->Import Logic in Allegro has an option to Create the PCB XML and launch the design compare utility.

I haven't tried what I'm about to suggest, but logic suggests it should work.

1. Open a blank board and import the 13.x pst files, using the generate the XML option.
2. You should have a file in the board directory called something_sch.xml. Rename it to 13x_sch.xml.
3. Open a blank board and import the 15.x pst files, using the generate the XML option.
4. You should have a file in the board directory called something_sch.xml. Rename it to 15x_sch.xml.
5. Launch the design compare and load the two files.

I hope this helps.

Kory,

Sorry, it looks like the XML tags got removed from my last post. If you get the jist of what I'm talking about, you should be able to see an example after you run the import.

Kory,

Here is another try at the XML sample.  See attached.

Try EDACompare from PTC.

The Cadence compare tool Charlie mentioned only does netlists really.

EDACompare does parametric comparisions and geometric comparisions (brd to brd, gerber to gerber etc.). It reports Refdes changes netname changes attrinbute changes etc

Pretty much everyhting InterComm can read, EDACompare can compare it.

http://www.ptc.com/WCMS/files/25639/en/25639en_file1.pdf

http://www.ptc.com/appserver/mkt/products/home.jsp?&k=3285

I hope this helps

Andy

The design compare inside of Allegro actually works well. We migrated from DxDesigner to ConceptHDL and used the Design Compare in Allegro to verify the schematic logic from both tools. I needed to load the logic from each schematic tool into Allegro to generate the required XML files used by the Design Compare but other than that it did what I needed.

Every so often I am asked to generate a difference reports between design revisions and the Design Compare in Allegro works flawlessly.

Good luck,
Mike Catrambone
UTStarcom, Inc.