Thursday, December 04, 2008     Register | Login | Search | Contact Us
     
   
     
     

Many of you already received communications about the move of the Cadence user community into cadence.com. And many of you have already joined, with over 4000 registrations in the first two weeks.

The new Cadence Community enhances the ability of Cadence users to connect and collaborate. In addition to moving the community into cadence.com -- enabling single sign-on for community, Sourcelink and Cadence events -- the new site is organized around nine technology segments, giving you easy access to product information, training, forums and blogs. Some of the new features include:
  • Ability to respond to posts via e-mail
  • Technology-specific blogs
  • Latest Web 2.0 social networking capabilities
  • Public profile options
  • Private messaging
  • Friends lists
Visit the new Cadence Community today at www.cadence.com/community and join the discussions!

Registration note: Due to the scope of the enhancements and the new SSO registration system, we were not able to migrate existing cdnusers.org member accounts. So new registrations are required, but this enables a broader set of functionality we think you'll enjoy.

Forum note: Under the guidance of forum moderators, we have taken the 20+ cdnusers.org forums and consolidated them into 11 forums on the new site. Posts have been brought over so you can leverage that posting history. CDNusers forums will be set to read only starting 7/30, and cdnusers.org will be redirected to the new community on 8/4.

Best regards,
Mike and Tom

Michael A. Catrambone - Steering Committee Chairman
Distinguished Engineer
PCB/Mechanical
UTStarcom, Inc.

Tom Diederich
Cadence Community Manager
Home
Forums
Forums > Silicon-package-board > PCB Design

Subject: Panelization
Posting to forums is available to community members only.
Login or Register
Rate this topic:
   
Author Messages
parveen@amdlsed.com
Posts: 8
Online: User is Offline
7/14/2008 1:50 AM  
Hi All,

I want to panelized my design in Allegro PCB Editor??? How it is possible?? Please advice.

Thanks & Regards,

Parveen
Parveen
bluecad
Posts: 16
Online: User is Offline
7/14/2008 5:36 AM  
Hi Parveen,

For panelization, you can use Gerber programs such as CAM350, GerbTool...
But if you want panelization in Allegro, you must write skill codes.
Look at Dave ELDER from TAIT CDNLive document September 2006.
It is name of "An Advanced Fabrication Array Utility"

Regards

FERHAT YALDIZ
Hpattie
Posts: 33
Online: User is Offline
7/14/2008 8:23 AM  
It is also possible to use a simple panel drawing, showing the outline of the boards, the spacing, and the tooling holes and fiducials. Then let your fabricator duplicate your data to match this drawing.
Regards,
Harold Pattie C. I. D.+
Dave Elder
Moderator
Posts: 150
Online: User is Offline
7/14/2008 1:14 PM  
Hi Parveen,

It is certainly possible using Skill. I wrote a utility that uses the step and repeat features of ODB++.
However it wan't a trivial task and the utility is heavily customised for my company's requirements.

Valor itself can do a reasonable job of creating a panel, if you have it.

Try posting here from now on:
http://www.cadence.com/community/forums/27.aspx

Cheers, Dave
Dave Elder
Tait Electronics
cadpro2k
Posts: 45
Online: User is Offline
7/14/2008 3:42 PM  
Hi,

I ditto Hpattie. That's my mode of operation. Let the people that specialize in the task do the job (the board manufacturer).

Couple things: 1) If you don't know what to do, or how to do it; get with you fabricator, and let them give you guidelines, or 2) have your mechanical folks do a panelization detail in mCAD (Pro-E, autoCAD, etc) and import that into allegro as the panelization details.

Another note, if your panelization is on a separate page, be sure and call it out in your notes, just to make sure the fabricator doesn't overlook it. :)

Good day.
mitch
cadpro2k
Posts: 45
Online: User is Offline
7/14/2008 3:44 PM  
BTW, I've been designing PCBs since the early 80's and I've NEVER once created a duplicatiing database to handle panelization. Why go through the hassle? (Unless your a "government" company)
purikku
Posts: 20
Online: User is Offline
7/15/2008 6:07 PM  
hi,
mostly in our design we do panelization of boards ( at least in our old software we can combine different board into one). but now in allegro i still dont know how to put the master board to the panel board. But i think there is way but still do not know how to because our japanese support will do it for us, the task given to us was just to make the panel board itself given its parameters (dimensions). then its up to the support how to put the master board to the panel board. if i learned how to, i will be back in this post.

GD
eric
cadpro2k
Posts: 45
Online: User is Offline
7/15/2008 9:29 PM  
Ahhhhha! I had forgotten what Cadence was working on. If you know your Cadence Support people where you're at, contact them, and ask them if they have their panelization SW tool working. We were shown this add-on tools some months ago, and I had completely forgot. It was pretty nifty! I'm sure it will do EXACTLY what you're intending.

Give them a call.

Good day.
Mitch
cadpro2k
Posts: 45
Online: User is Offline
7/15/2008 9:32 PM  
Solution:
Cadence has created an MSWare module which has the ability to create panelize data
from the Allegro PCB Editor software. For
for more information and pricing please contact your local Cadence sales rep.

Alternatively you can use the following method :
*** NOTE : This solution will only work with the Allegro Performance option and above
***
1. Open the design that you would like panelized and ensure that the data is correct
2. Enable the relevant colors that will be used to replicate the necessary elements
from the database
3. Select Tools > Create Module and enable all of the necessary items in the Options
tab. Select, by window, the items needed for the panelized items. This will be
referred to as a module
4. Select an origin for the module. e.g. x 0 y 0
5. Save the module (it will be saved as a .mdd file)
6. Create a new database that will be used to do the penalization. The new database
must have the same cross section as the database in which the modules were created.
You can use the techfile functionality of Allegro to save the design intent and
import it into the new design
7. Select Place > Manually. In the Advanced Settings tab ensure that "Library" is enabled
8. In the Placement list tab select "Module definitions"
9. Click on the module that you had created in step 5. If you do not see the module
listed you may need to review you modulepath setting(s)
10.Once the module has been selected and placed in the design a fillin will be presented to
you which asks you to add the "Module instance name"
11. The Instance name will be the "Prefix" number for ALL Nets and Symbols, i.e. 1_GND
(module 1) 2_GND (module 2)
12. Place as many modules as you like to create the Panel
13. Perform any necessary checks on the database and create your manufacturing output

Note:
One limitation with this method, which is available in the MSWare Module, is you are NOT
able to mirror the module in the Panel, i.e. all the modules will be on the same
side.
purikku
Posts: 20
Online: User is Offline
7/15/2008 9:58 PM  
cadpro2k,

i tried your method now using the panel board i made and it worked. thanks for the info. now i will not wait for the jap to teach me. hehehehe

GD
eric
parveen@amdlsed.com
Posts: 8
Online: User is Offline
7/16/2008 1:28 AM  
Thanks to all for their kind replies. Module option I can't use as I have only PCB Editor no performance options as well as I asked about the MSWare tools from the cadence but not able to get the pricing. Is it possible by PCB Editor without performance option?? Is there any skill program which I can use for the same. Please advice.

Thanks & Regards,

Parveen
Parveen
Posting to forums is available to community members only.
Login or Register


ActiveForums 3.6
     
Copyright 2006 Cadence Design Systems, Inc.