silkscreen_top? (other than redrawing it using the correct class/su">
     
Friday, May 18, 2012     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: How to change line class
Posting to forums is available to community members only.
Login or Register
Rate this topic:
   
Author Messages
wizlogix
Posts: 5
Online: User is Offline
3/26/2008 11:12 PM  
Hi

I'm a new user to Allergo PCB editor. I have a question on the line classes.
A line path was created in "top-etch" layer, how can i simply change it class to the correct package_geom -> silkscreen_top? (other than redrawing it using the correct class/subclass)?

Appreciate any help.

Thanks
Shawn
shiva
Posts: 57
Online: User is Offline
3/27/2008 12:54 AM  
It shouldn't possible to change one class to another. If you want, you can change one sub-class to another using the change command. It's possible to change one class to another using DXF command. Wish it will help you.
wizlogix
Posts: 5
Online: User is Offline
3/27/2008 2:37 AM  
can you explain how to use the DXF command method to change the line's class from Board Geometry to Package Geometry?
KenM
Posts: 18
Online: User is Offline
3/27/2008 4:41 AM  
you can do this:

file -> export ->sub-drawing. select the line(s). open the .clp file, change class and sub class to what you want.

read in the .clp file:

file -> import -> sub-drawing.
KenM
Posts: 18
Online: User is Offline
3/27/2008 4:41 AM  
open the .clp file with wordpad
shiva
Posts: 57
Online: User is Offline
3/27/2008 5:02 AM  
WOW!!! It's the easy way than DXF. Thanks a lot Ken.
Boma
Posts: 10
Online: User is Offline
3/27/2008 5:09 AM  
Another method that I use is a little skill code written by Uri Chaplin called copy_lines.  It runs from within Allegro and allows you to copy lines across classes.  A nice piece of code that we use to create our NC milling data on complex outlines to move a decomposed expanded shape lines from the Drawing Format Construction layer to the Board Geometry NCroute path layer.  I have included the code here for you to try if you like.

Boma

Attachment: copy_lines.zip
shiva
Posts: 57
Online: User is Offline
3/27/2008 5:38 AM  
Hello Boma, To which folder can i store this files? How can i continue? Please explain. Thanks.
Boma
Posts: 10
Online: User is Offline
3/27/2008 6:27 AM  
Shiva,

To run the code:
   1. unzip the skill code to your physical diriectory
   2. Type  skill load("copy_lines.il")  on the command line.
   3. To run the command type  copy_lines  on the command line.

Boma
wizlogix
Posts: 5
Online: User is Offline
3/27/2008 7:20 AM  
wow, thanks a lot guys....its really help.
shiva
Posts: 57
Online: User is Offline
3/29/2008 3:05 AM  
Hello Boma, Physical directory means, the current working directory or the source directory of allegro? I got an error that is "commond not found". Please explain in steps. Thanks.
Boma
Posts: 10
Online: User is Offline
3/29/2008 6:24 AM  
The physical directory is the directory where your board file or .brd file resides.

Boma
redwire
Posts: 73
Online: User is Offline
3/30/2008 12:08 PM  
You might not have the license level to run Skill. You need performance L or higher.
shiva
Posts: 57
Online: User is Offline
3/30/2008 9:51 PM  
Oh it's true. Now we have licence only for PCB Design L. Thanks redwire and thanks to all.
BillZ_EMA
Posts: 51
Online: User is Offline
3/31/2008 6:19 AM  
Allegro L will execute skill code. .il files
Allegro Performance and higher executes skill commands.

Regards,
BillZ
EMA Design Automation
redwire
Posts: 73
Online: User is Offline
3/31/2008 9:24 PM  
Bill (EMA)
Could you elaborate? I have never successfully run Skill on less than Perf L license. When I type the command skill (as shown in the example) it bombs out.

I'd love to learn this.

Thanks.
BillZ_EMA
Posts: 51
Online: User is Offline
4/01/2008 1:20 PM  
There are 2 methods.

First you must load the skill file then you execute it.
method 1) load the skill file form the allegro command line
method 2) load the skill everytime Allegro starts using the allegro.ilinit
Sourcelink contains both solutions.

Here is the method using the command line from sourcelink
How to load and execute SKILL from a local directory.

Error Message:
None

Problem statement:
I want to load and run SKILL files that are kept locally, but I don't want to set
up an allegro.ilinit file. How can I do this?


Solution:
You can load a SKILL file by typing at the Allegro command line:

Command > (load "skill_file_name.il")

This will load the SKILL file and if it is successfully loaded, the Allegro command line
will report a "t" as the last entry. The SKILL file will only load if the file is in
the SKILL search path. To find the SKILL search path the user can type at the
Allegro command line:

Command > (getSkillPath())

SKILL will echo the current SKILL search path. If the file that you wish to load is not in
the search path then you must choose one of the following:

1. Move or copy the file into the SKILL search path.
2. Specify the full path to the SKILL file. Use slashes / to separate the paths,
instead of \ (even on a PC)
3. Modify the search path to include the path to your SKILL file. Again you must use
the slash / in the path.

Example: using g.il

Command > (load "g.il")
function _viewr redefined
function _repCallback redefined
function _lfsBuildForm redefined
function lfsViewReports redefined
t
Command >


To execute the file, open the file in an ASCII text editor and review any comments
about running the program or look for the registered command. As an example:

axlCmdRegister ("aa" "Reports")

In this example, "aa" is the command that the user types at the Allegro command prompt
and "Reports" is the name of the SKILL function that is called by that command.

Regards,
BillZ
EMA Design Automation
redwire
Posts: 73
Online: User is Offline
4/01/2008 2:18 PM  
Good info! Thanks.
bills
Posts: 4
Online: User is Offline
4/08/2008 12:14 PM  
Redwire,
Thank you for the copy_line skill file. I am aware of the methodology Billz_EMA uses to execute skill files in the Allegro PCB Editor tool. I have gone one step further and have my skill files activated from a custom made pull-down menu I have added to my PCB Editor. This was easier for me as I have multiple skill files and have trouble remembering the commands I have to type into the command line to activate them.

Regards,
Bills
EMA Design Automation
Posting to forums is available to community members only.
Login or Register
Forums > Silicon-package-board > PCB Design > How to change line class


ActiveForums 3.6
     
Copyright 2006 Cadence Design Systems, Inc.