Mark, You're welcome. But I just wrote an alias that replays Cadence solution ;-)... As far as I know (and seems to be confirmed on the solution below), the only way to disable CM is by removing files and folder about it. William. The solution number on Sourcelink is 11051882: Error message: When doing Export Physical, after deleting the constraints folder, the following error is reported: ERROR(300) Net Rev fatal error detected. Design flow is Constraint Manager enabled, pstcmdb.dat and pstxnet.dat do not appear to be from the same packaging step. Problem statement: The Constraint Manager has been used in ConceptHDL to setup several ECSets and rules. The customer is now finding that it will be easier to do all the rule setup from Allegro and would like to disable the CM enabled flow that is now active. The constraints folder was deleted and now when trying to do Export Physical, the design will not go through the process. What other steps are necessary to get back to a clean flow? Solution: There are several steps we must go through to back out of the CM enable flow. The first thing we must do is determine if you have the level of 14.2 that has this capability built in to it. If you are in Allegro and do Help>About Allegro you will get a window that says something like 14.2-s041. This is the first patched version of Allegro that allows us to back out of enable flow. Once that is done, the other steps are: 1. In Allegro type: skill <return> type: axlDBControl('cmgrEnabledFlow nil) <return>. You should see a 't' in the command area which indicates the command was successful. This will reset the branding flag inside the database so netrev will not look for pstcm*.dat files. type: exit <return> to exit the skill interpreter Save the .brd file. 2. Delete the 'constraints' folder under <project>/worklib/<design name> 3. Delete the 'opf' folder under <project>/worklib/<design name> 4. In the 'packaged' directory - delete cmdbview.dat, cmdcview.dat, pstcmdb.dat, pstcmbc.dat, pstcmback.dat 5. Run Export Physical to regenerate the netlist files. 6. Run Import Logic in Allegro. 7. From this point on, constraints are managed in Allegro. Whenever you run Export Logic from Allegro, the checkbox 'Export using Constraint Manager enabled flow' should be unchecked. Important: This procedure assume the design is flat and has been back-annotated ________________________________ From: icu-pcb-forum-bounce@xxxxxxxxxxxxx [mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Mark Salberg Sent: 17 October, 2007 4:07 PM To: icu-pcb-forum@xxxxxxxxxxxxx Subject: [PCB_FORUM] Re: Two Concept error questions William, Excellent feedback! It did work, but here is what I had to do. Since we do not even have any of the required *cmdb.dat files files I ran (axlDBControl('cmgrEnabledFlow nil)) in the Allegro command line, saved the board and re-packaged. And it WORKED! Question...is this the only way to disable the Constraint Manager Flow? I could not find anything in the setup or packager options. Is there a secret place that this is documented? Seems like there should be a selection box for this. Again...THANKS! That one had us going! Mark William Billereau wrote: For the first point, you have to call File/Change Suite in Concept and select Allegro PCB design HDL. It works for us. For the second point, the error300, I added an alias in Allegro's alias file named error300 that calls the command: alias error300 "osdelete ..\packaged\pstcmdb.dat;(axlDBControl('cmgrEnabledFlow nil))" maybe the pstcmdb.dat is not enough, sometimes it needs to remove all *cmdb.dat files.... You have to load the BRD, run this alias, save the BRD and re-run the export physical. William. ________________________________ From: icu-pcb-forum-bounce@xxxxxxxxxxxxx [ mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Mark Salberg Sent: 17 October, 2007 12:02 PM To: icu-pcb-forum@xxxxxxxxxxxxx Subject: [PCB_FORUM] Re: Two Concept error questions Thanks for the feedback. We can not get any combination of tools to work. 1. Here are my choices when launching proj manager. 2. When loading Concept, I get: 3. Here are my choices When choosing Legacy, then no warning #2, but when packaging I receive the following error. Any ideas what the board could have been saved in (Allegro)? and which tool should be able to create the .dat files needed? pstcmdb.dat and pstcmbc.dat Thanks again for any feedback. Mark Van Os, Richard (GE Healthcare) wrote: The first case is a warning. Follow the message to turn this check of in the schematic. The error listed below it means the previous schematic was package with an expert tool versus a lower tier tool. So going futher into the error message Design Constraint Manager Enabled. Basically the repackage in the expert tool this will generate the missing files pstcmdb.dat and pstcmbc.dat Search on Design Constraint Manager Enabled in the help file for a full explaination. ~Richard ________________________________ From: icu-pcb-forum-bounce@xxxxxxxxxxxxx [ mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Mark Salberg Sent: Tuesday, October 16, 2007 11:55 AM To: Cadence User Group Subject: [PCB_FORUM] Two Concept error questions We are experiencing the following two errors in Concept V.15.7 Any thoughts? We can not save the schematic or package to Allegro. 1. While saving the schematic, errors appear. INFO (voltage_on_hdl) HDL Power Symbol doesn't have voltage property. To turn off this warning please goto Tools->Options->Check and uncheck 'Voltage on HDL Symbols' option. 2. Packager error...there is nothing in Constraint manager. Thanks in advance, Mark ________________________________________________________________________ _____ Scanned by IBM Email Security Management Services powered by MessageLabs. For more information please visit http://www.ers.ibm.com ________________________________________________________________________ _____ ________________________________________________________________________ _____ Scanned by IBM Email Security Management Services powered by MessageLabs. For more information please visit http://www.ers.ibm.com ________________________________________________________________________ _____