We are in the process of updating numerous Concept-Allegro designs to version 15, from version 13 (and below). We have it all fairly well figured out, with regards to the migration path.We are not spinning artwork and cannot easily and automatically verify the conversion by way of comparing Gerbers. (Issues with differing output formats AND hand manipulation of aperture lists prevent a smooth process.)Have any of you come across a comparison utility that would allow us to compare the Allegro Design Entry V15 databases to our Concept V13 databases?There are methods whereby you can extract netlists, and run Unix diff utilities. This may not work too well due to netname changes across the versions. I worry there may be too much to filter out.Help....Kory JohnsonGE Medical Systems - OEC
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 etcPretty much everyhting InterComm can read, EDACompare can compare it.http://www.ptc.com/WCMS/files/25639/en/25639en_file1.pdfhttp://www.ptc.com/appserver/mkt/products/home.jsp?&k=3285I hope this helpsAndy
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 CatramboneUTStarcom, Inc.
Update: The XML comparison (inside Allegro) is fairly easy and provided the coursest look at design comparison.I have demoed DOCTAR and found it to be a very easy-to-use and helpful tool. From download to actually using the product was very quick and intuitive.PTC's EDA Compare is good and had the broadest scope. I believe it's not a stand alone product and is part of a suite of tools meant for sharing data between groups. It also had, or would soon have, the ability to filter the reports - this would aid me greatly.