[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  <mailto:dave.schaefer@xxxxxxx> <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: