[PCB_FORUM] Re: Design a complete layout using mentor schematics and Allegro Layout tool setup

Sathish:
 
So it sounds like, from your reply, that you will be using Mentor
"source" library parts converted over to Cadence.
 
Just so you know:
 
There are two modes of translation.
 
One method is the back-end translation (PCB layout) using the mbs2brd
translator. This works as a stand-alone executable or it can be found in
the Pull-down menu of SpecctraQuest (or currently known as Allegro
...SI) And exisitng Mentor layout to Allegro layout.
 
The other mode is a library part translator  (Mentor Graphics Corp. to
Cadence) : this may include schematic logic symbols and physical part.
(Translator made by Cadence)
 
So it sounds like you will be provided with parts from your "vendor"?   
 
Of course it appears like you are going down the path of the 3rd party
netlist approach and providing the package information to build it in
Allegro. (That is the way we used to do it when I was in the PCB service
Bureau many moons ago.) 
 
Just wanted to make you aware of those other two options in case you
have not explored those possibilities. 
 
Good luck.
 
Michael B. 
 

________________________________

From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of sathish kumar
Sent: Tuesday, July 25, 2006 4:06 AM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: Design a complete layout using mentor
schematics and Allegro Layout tool setup




Michael ,

You are right . iam going to use mentor schematics and design the layout
in cadence allegro. So the netlist and library has to be translated to
allegro required format for doing routing and gerbers. I found a way to
import the mentor netlist using thirdparty option in cadence. Iam yet to
get the mentor to allegro converted library parts from vendor. need to
confirm it soon. 

I hope you got my idea and i have already received some useful
information from some of the engineers in this forum. Lets make the
things happen. Thanks for a prompt response.


With Sincere,

Sathish.

GDA Technologies, Inc.

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

 

 

        
________________________________

        From: "Baumstark Michael-EMB043" <M.Baumstark@xxxxxxxxxxxx>
        Reply-To: icu-pcb-forum@xxxxxxxxxxxxx
        To: <icu-pcb-forum@xxxxxxxxxxxxx>
        Subject: [PCB_FORUM] Re: Design a complete layout using mentor
schematics and Allegro Layout tool setup
        Date: Mon, 24 Jul 2006 18:33:09 -0400
        
        
        Sathish:
         
        Hey I am not if you have considered this possibility in your bag
of tricks: have you thought about going to layout in Mentor, doing a
quick place in Mentor, then perform a File _import _Mentor using the CDS
SI tool (this runs the mbs2brd) translation from within the Allegro_SI
engine.  From there you will have an uncompleted Layout going on in
Allegro. Of  course if you need to supply Cadence Library footprints,
you could substitute them in an extracted placement file; otherwise you
would be using footprints generated from the Mentor Library. (Obviously
you could have a host of conventional differences (pin numbers/names
etc.) if you need to match up with a Cadence library of footprints.  
         
        I haven't really had to deal with this type of conversion before
and  I do not know your exact requirements are. But I have had the
similar task to use a Mentor schematic and mentor layout and then
continue the design in Cadence (no requirement to backannotate to
Mentor). Here we did use a native Cadence schematic capture then meshed
the translated layout to sync up. with the Cadence schematic. It takes a
little bit of work to get done. But this is for a special requirements
situation.
         
        Maybe that is a viable solution, depending on which Library
footprints you need to use. 
         
        Speaking of using the design compare utility, which I saw
Kumaran M, reply to you.   I have a question about Design compare
utility.  The other day I was using the Design Compare utility while
having a session of  Allegro open. I had cross probing capability going
on. For example, I could select a reference designator in the Compare
list and it would center up on hte screen in Allegro. I am trying to do
this again and my cross-probing feature is not working. (When I first
saw it happening it was a present surprise.) Now I cannot get it to work
again. Does anybosy have any suggestion to enable cross-probing from
Design compare utility and Allegro Layout?
         
        Sincerely yours, 

        Michael Baumstark 

        Staff PCB Designer - BSEE, CID+ 
        Motorola - Advanced Product Technology Center 
        8000 West Sunrise Blvd.  Mail Stop: 8E8 
        Plantation, FL USA 33322-9947 
        Intra: http://rprc.mot.com <http://rprc.mot.com/>   ;
http://pcbadvisor.mot.com <http://pcbadvisor.mot.com/>  
        web: http://www.motorola.com <http://www.motorola.com/>  
        
--------------^------------------^-----------------^------------------^-
------------- 
          >---^-.---                 >---^-.---
>---^-.--- 
        Motorola Internal Use                      [      ] 
        Motorola Confidential Proprietary    [      ] 


________________________________

        From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of sathish kumar
        Sent: Tuesday, July 18, 2006 2:49 PM
        To: icu-pcb-forum@xxxxxxxxxxxxx
        Cc: Sue.Reade@xxxxxxxxxxx
        Subject: [PCB_FORUM] Design a complete layout using mentor
schematics and Allegro Layout tool setup
        
        

        Hi

        I have a requirement to design a board from mentor schematics
and to work the layout in Cadence Allegro tool. I got some suggestions
from forum to translate the netlist from mentor to Cadence earlier.

        Can you provide your suggestions about this setup and
difficulties working on different tools so that i can prepare myself
about each milestones. 

        I have some questions on working on these ways. Pls provide your
answers.

        1) Once all the intial netlist .tel gets imported into Allegro
tool, if we need to import netlsit changes (eco) at many times in the
middle phase of project. How it can be imported each time without any
issues using third party allegro netlist.

        2) How can the back annotation process works from allegro layout
to mentor schematics. Isit possible?

        3) How can we compare the final layout and netlist with
different packages to go ahead on gerbers release.

        Pls let me know if any more problems expected in this design
execution process. This is a fairly complex design with around 22
layers.

        Expecting your valuable answers and suggestions. Thanks in
Advance.

With Sincere,

Sathish.

GDA Technologies, Inc.

" 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
----------------------------------------------------------- 


----------------------------------------------------------- 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: