[PCB_FORUM] Re: Netlist conversion from mentor tool to Allegro tool

Satish,
 
Once you run the net list from DxDesigner, the device files are
generated automatically and can be found in the dashboard. Once these
files are found, move them to an appropriate location. For example, I
have three directories for devices, padstacks, and dwgs. In User
Preferences, make sure you point to the correct directories. As Sue
indicated, you must generate the .dra & .psm with their appropriate
padstacks.
 

Cheers, 

Ron Scott C.I.D.+ 
Texas Instruments 
Storage Products Group 
Tel:   214.567.4715 
Cell:  972.816.7978 
rg-scott@xxxxxx 

 

________________________________

From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Reade, Sue
Sent: Tuesday, July 11, 2006 15:50
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: Netlist conversion from mentor tool to Allegro
tool


Sathish,
If you do not have access to the device (.txt) files from Designer AND
you have all of the allegro models built and placed in allegro, you can
FILE, EXPORT, LIBRARIES, select DEVICE FILES.
put all of those .txt files into a separate directory.
Edit your ENV file to add a DEVPATH statement pointing to the new
directory containing the device files.
 
________________________________

From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of sathish kumar
Sent: Tuesday, July 11, 2006 3:35 PM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: Netlist conversion from mentor tool to Allegro
tool



Thanks Reade, Sue for the info. I tried importing the .tel file as you
mentioned. whle importing with syntax check enabled in first step its
showing error file for eg:

$PACKAGES
CDRH6D38 ! '3A_3P3UH_SMT_IND' ! '3.3UH' ! '20%' ; L17 L18 L5021 L13008 ,
                                                 ^
ERROR: Cannot find device file for '3A_3P3UH_SMT_IND'.
------------------------------------------------------------------------
-------

I got only the .tel file right now. I think its searching for Device
files and library path. How to create config and .txt device files from
mentor tool and how to assign the path in env directory.

Thanks in advance!!!!!!!

With Sincere,

Sathish.

" Efforts may fail but, dont fail to make Efforts " 

 

 

        
________________________________

        From: "Reade, Sue" <Sue.Reade@xxxxxxxxxxx>
        Reply-To: icu-pcb-forum@xxxxxxxxxxxxx
        To: <icu-pcb-forum@xxxxxxxxxxxxx>
        Subject: [PCB_FORUM] Re: Netlist conversion from mentor tool to
Allegro tool
        Date: Tue, 11 Jul 2006 13:49:47 -0500
        
        
        I think you may have more questions in mind, but I'll take the
simple track.
        Allegro reads in .tel files with no problem. 3rd party netlist
        File
        Import
        Logic
        Other
        find your .tel file in the ... button
        run the syntax check only first to make sure your netlist is
structurally sound.
        then select supercede all logical data (this actually means read
the netlist).
        Now for the problems, you will need a config file on the mentor
side so that you translate correctly - this may take some work - talk to
your mentor vendor.
        also you will need to have the .txt files that are created at
the time you run your netlist (these are the devices files) and point to
them through your env file. I have not run designer in a long time but I
think you need to select the option to create them.

________________________________

        From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of sathish kumar
        Sent: Tuesday, July 11, 2006 2:31 PM
        To: icu-pcb-forum@xxxxxxxxxxxxx
        Subject: [PCB_FORUM] Netlist conversion from mentor tool to
Allegro tool
        
        

        
        Hi,

        I need to convert a netlist from mentor DX designer tool to
Cadence Allegro appropriate tool. Is there anyway to translate the
netlist from mentor to Allegro. Pls share the possibilties to do this
conversion and i need to know this as quick as possible.

        Thanks in advance for everyone

With Sincere,

Sathish.

GDA Technologies, Inc.

" Efforts may fail but, dont fail to make Efforts " 

 

 
</TB 

----------------------------------------------------------- To
subscribe/unsubscribe: Send a message to
icu-pcb-forum-request@xxxxxxxxxxxxx with a subject of subscribe or
unsubscribe To view the archives of this list go to
http://www.freelists.org/archives/icu-pcb-forum/ Problems or Questions:
Send an email to icu-pcb-forum-admins@xxxxxxxxxxxxx
----------------------------------------------------------- 


----------------------------------------------------------- To
subscribe/unsubscribe: Send a message to
icu-pcb-forum-request@xxxxxxxxxxxxx with a subject of subscribe or
unsubscribe To view the archives of this list go to
http://www.freelists.org/archives/icu-pcb-forum/ Problems or Questions:
Send an email to icu-pcb-forum-admins@xxxxxxxxxxxxx
-----------------------------------------------------------

Other related posts: