[PCB_FORUM] Re: Penalizing two different jobs in allegro

Hi Sushma,

Here is the way to do it.

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
refered 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 panelization. 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

Regards
Kumaran M


> Hi!
>
> I hared that In allegro, we can panelize two different jobs in one and
> send out a combined Gerber to Fab. Is it true?
> I tried to search on help but could not find any thing related to this. If
> this is true please help me finding how to do this.
> I will appreciate any help.
>
> Regards,
> Sushma
>
>
>
> ---- Original Message -----
>   From: Naren Thesia
>   To: icu-pcb-forum@xxxxxxxxxxxxx
>   Sent: Wednesday, June 14, 2006 10:00 PM
>   Subject: [PCB_FORUM] Need Solder Mask Keep out
>
>
>   Hi All,
>
>
>
>   We have panel board with so many metallic components like fuse & heat
> sink.
>
>   Due to board density we can not avoid via below them. For precaution we
> want to tent those vias.
>
>
>
>   1)     Is it possible to provide such kind of "Keep out" area for solder
> mask? So that it will give DRC for non masked vias.
>
>   2)     Is there any Skill file can help to detect such incidents?
>
>
>
>   Thanks in Advance
>
-----------------------------------------------------------
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: