Browse icu-pcb-forum: This Month's Archive • Main Archive Page • Related posts • Previous by Date • Next by Date

[PCB_FORUM] Re: Two Concept error questions

From: "Chad Saathoff" <chads@xxxxxxxxxxx>
To: <icu-pcb-forum@xxxxxxxxxxxxx>
Date: Wed, 17 Oct 2007 07:46:36 -0700

This is documented in Sourcelink under Solution Number 11087996.

Chad

 


________________________________

        From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Mark Salberg
        Sent: Wednesday, October 17, 2007 9:07 AM
        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
        
________________________________________________________________________
_____

References:

[PCB_FORUM] Two Concept error questions
From: Mark Salberg

[PCB_FORUM] Re: Two Concept error questions
From: Van Os, Richard (GE Healthcare)

[PCB_FORUM] Re: Two Concept error questions
From: Mark Salberg

[PCB_FORUM] Re: Two Concept error questions
From: William Billereau

[PCB_FORUM] Re: Two Concept error questions
From: Mark Salberg

[PCB_FORUM] Re: Two Concept error questions

Other related posts: