[PCB_FORUM] Re: Allegro ODB++

Hey George,

 

I would agree that custom thermals are a limitation of the current ODB++
Inside translator and Allegro tools in general when it comes to voided
shapes in thermals.  I configured the Valor Thermal model file based on
drill size using our thermal relief formulas for Vias and Pins so the
thermals get generated on the fly while the thermal flash name is
ignored which seems to do the job, as you said this type of setup works
efficiently for standard thermals.

Sincerely,
Michael Catrambone
UTStarcom, Inc.
Chairman
Cadence Designer Network
CDNLive! Worldwide Web Site: http://www.cdnlive.com
<http://www.cdnlive.com> 
Cadence User Community Web Site:  http://www.cdnusers.org
<http://www.cdnusers.org> 

________________________________

From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of
george.h.patrick@xxxxxxxxxxxxxx
Sent: Friday, April 27, 2007 10:56 AM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: Allegro ODB++

 

To add my two cents worth:

 

ODB++ Inside is fine if all you use are standard thermals.  If you have
special thermals it will not work correctly unless you have that flash
defined in the Thermal Models file, which is only possible for a range
of shapes.

 

If you are using WYSISYG mode in Allegro, you no longer need the Thermal
Models file, but since Allegro does not allow flash symbols to use
voided shapes we can not use it.

 

So:

- are you using ODB++ for fabrication, manufacturing, ICT
    No, we can't use the Allegro ODB++ export.  One vendor gives us a
tooling break 
    for ODB++ so we import the gerbers to Valor and export a native
ODB++
- does the Allegro "ODB++ inside" translator produce accurate and
reliable data
    No, unless you can set-up the special thermals in the Thermal Models
file.  Since 
    our special thermals are constructed using lines, we can't use the
WYSIWYG 
    mode which would require a voided shape for some of them.
- how do you verify the accuracy of your ODB++ data
    We use Valor so if we could use the ODB++ Inside we could import
that and verify.
- if using ODB++, do you provide additonal data/drawing formats
    N/A
- any other pros/cons of ODB++ use

    No

 

-- 
George Patrick
Tektronix, Inc.
Central Engineering, EDS Applications Support
P.O. Box 500, M/S 39-512
Beaverton, OR 97077-0001
* 503-627-5272 (voice)     * 503-627-5587 (fax)
http://www.tektronix.com <http://www.tektronix.com/>
http://www.pcb-designer.com <http://www.pcb-designer.com/> 
 
"Off-Grid and Proud of it!"

        -----Original Message-----
        From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Michael
Catrambone
        Sent: Thursday, April 26, 2007 16:16
        To: icu-pcb-forum@xxxxxxxxxxxxx
        Subject: [PCB_FORUM] Re: Allegro ODB++

        We have been using ODB++ Inside for a while now, since 2001, and
I believe they worked most of the bugs out of it since it first was
released.  We are using ODB++ Inside version 7.05 and all of our film
records get mapped over to the appropriate layer names in the Valor
matrix so sst is actually our Top Silkscreen film record and ssb is
actually our Bottom Silkscreen film record.  We do get some extra layers
that are classified "documentation" in the matrix, they are sqa_areas
which is the Constraint Areas and smt_top & smt_bot which are empty.
Maybe there is some assumptions made by the translation when building
the matrix but we have not had any problems at this point. I would like
to see the matrix names actually match our film records names but I
guess I can't have everything.

         

        To answer the original questions:

        - We are using ODB++ for fabrication data (still generate gerber
files for those few vendors that don't use it)

        - The data generated by the ODB++ Inside does produce accurate
and reliable data (At least in our environment)

        - As far as verifying the ODB++ data we routinely compare it to
our traditional outputs, which we still generate just in case.

        - The only issue I have with the ODB++ Inside generation is that
it takes long on larger designs because it feels the need to run the
field solver.

        My two cents,
        Michael Catrambone
        UTStarcom, Inc.
        Chairman
        Cadence Designer Network
        CDNLive! Worldwide Web Site: http://www.cdnlive.com
<http://www.cdnlive.com> 
        Cadence User Community Web Site:  http://www.cdnusers.org
<http://www.cdnusers.org> 

        
________________________________


        From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Dave Elder
        Sent: Thursday, April 26, 2007 5:28 PM
        To: icu-pcb-forum@xxxxxxxxxxxxx
        Subject: [PCB_FORUM] Re: Allegro ODB++

         

        Richard raises a couple of good points that need some
clarification:
        
        "The issue I currently have is not with ODB++, but with 'ODB++
Inside'. It creates extra layers that you may not necessarily want in
your outputs. If I wanted to include them, I would liked to have
specified them.
        
        For example, it takes what it assumes is the Top Silk film and
renames it 'sst' . Anything else it thinks maybe silk films it calls
'sst+1', sst+2', etc, which include subclasses nothing to do with silk.
(Someone feel free to correct me here if I'm wrong, but that's what I've
always found.) In other words, lack of control does not impress me." 
        
        The outputs are totally configurable. ODB++ Inside does a
reasonably good job of identifying the artwork type but you can change
the defaults by editing the artwork layers (as you would with Gerber
outputs) or by using the built-in matrix editor. In Richard's example it
is easy to change sst+1 to, say, "doc_top" or delete it altogether.
ODB++ inside uses the same artwork setups as you would use for Gerber/NC
outputs.
        
        Cheers, Dave
        
        richard moffat wrote: 

        Hi
         
        Whether to use ODB++ or other formats can be a religious
argument.
         
        Rather than repeat what I've said before, read 
        
http://www.freelists.org/archives/icu-pcb-forum/05-2006/msg00104.html 
        instead.
         
        Once ODB++ is more flexible, we may look at it again.  (I have
other slight reservations that I won't go into here.)
         
        Until then, we have Allegro and Gerbtool customised to an extent
that gives us a 'one button click' solution for all our generation,
electrical validation, and CAM validation.
         
        Cheers,
        Richard
         
         
         
          
        __________________________
        Richard Moffat
        PCB CAD Team Leader
        Allied Telesis Labs
        ph. +64 (3) 3393000
        richard.moffat@xxxxxxxxxxxxxxxxxxx
         
          

                                Dave Schaefer <dave.schaefer@xxxxxxx>
<mailto:dave.schaefer@xxxxxxx>  27/04/2007 5:37 a.m. >>>
                                        

        Would like to get other user's thoughts on the use of ODB++:
         
        - are you using ODB++ for fabrication, manufacturing, ICT
        - does the Allegro "ODB++ inside" translator produce accurate
and reliable data
        - how do you verify the accuracy of your ODB++ data
        - if using ODB++, do you provide additonal data/drawing formats
        - any other pros/cons of ODB++ use
         
         
        Thanks,
        Dave
         
        Dave Schaefer
        dave.schaefer@xxxxxxx 
        -----------------------------------------------------------
        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 
        -----------------------------------------------------------
         
        NOTICE: This message contains privileged and confidential
        information intended only for the use of the addressee
        named above. If you are not the intended recipient of
        this message you are hereby notified that you must not
        disseminate, copy or take any action in reliance on it.
        If you have received this message in error please
        notify Allied Telesis Labs Ltd immediately.
        Any views expressed in this message are those of the
        individual sender, except where the sender has the
        authority to issue and specifically states them to
        be the views of Allied Telesis Labs.
        -----------------------------------------------------------
        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: