Wednesday, December 03, 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 > Shared code - SKILL

Subject: How to check the mistaken Reference Text location
Posting to forums is available to community members only.
Login or Register
Rate this topic:
   
Author Messages
leonlee
Posts: 81
Online: User is Offline
8/21/2006 6:46 PM  
How to check the mistaken Reference Text location during arranging the silkscreen?
For example, the component R1 is close to R2, but the Text: R1 and Text: R2 have been exchanged their location. But Allegro can't check them out.
How deal with this situation by SKILL or other solution?
Leon Lee
Schneider-Electric
Dave Elder
Moderator
Posts: 150
Online: User is Offline
8/21/2006 6:53 PM  
Hi Leon,

Have you used the autosilkUtils.il code. It does that (and much more).

Cheers, Dave
Dave Elder
Tait Electronics
leonlee
Posts: 81
Online: User is Offline
8/21/2006 7:01 PM  
Hi, Dave,

I havn't use the routine: autosilkUtils.il. Is it written by you or Candece original function?
Leon Lee
Schneider-Electric
Dave Elder
Moderator
Posts: 150
Online: User is Offline
8/21/2006 7:55 PM  
Hi Leon,

I wrote it. Download it from the Allegro Skill Code area on sourcelink.
(Look for "Silkscreen violation checking" utility)

Cheers, Dave
Dave Elder
Tait Electronics
roger.green@alspcb
Posts: 8
Online: User is Offline
9/10/2007 2:51 AM  
Hi Dave

i have been using your silkutils skill code for some time and would like to change some of the default setting to make it a bit quicker, could you tell me how to do the following ( if thats OK by you) turn off Reference Des Locations, Solder mask on vias and set the default value to 5 in the boxes
This is to help speed up the checking in Valor.

Cheers, Roger
Dave Elder
Moderator
Posts: 150
Online: User is Offline
9/10/2007 1:42 PM  
Hi Roger, Edit the Skill file and change the following: To turn off Reference Designator Locations: In line 505 change the following line from: ASU_toggleField(form, "textloc", car(objectsExist)) to: ASU_toggleField(form, "textloc", nil) To uncheck Solder Mask Pads on Vias: In line 285 change the line: if(viaResist then when(ASU_checkVias, axlFormSetField(form, "vias", t)) else axlFormSetFieldEditable(form, "vias", 0)) axlFormSetField(form, "vias", nil), unless(viaResist, axlFormSetFieldEditable(form, "vias", 0)) To set the spacing defaults to 5 mils: search and replace on the following text that appears in three locations: axlMKSConvert(10, "mils") Change to axlMKSConvert(5, "mils") Note: These values are stored in the design - so if the utility has been run with 10 mils - that will still be the number that is in the booxes. Let me know if you have any problems. I can send you the modified code if you like. Cheers, Dave
Dave Elder
Tait Electronics
roger.green@alspcb
Posts: 8
Online: User is Offline
9/11/2007 2:11 AM  
Dave thank for the reply. I have managed to sort out the spacing defults and the ref des check box but when I did the other bit I lost both the of the lower check boxes. I only wanted to tund off Check to solder mask pads on vias and not Check to solder mask shapes, this is a must as we have had to change the Valor efr files to remove the silkscreen errors on the vias and when this happens we don't get the check on other solder mask shapes.

Cheers, Roger
Dave Elder
Moderator
Posts: 150
Online: User is Offline
9/11/2007 12:56 PM  
Hi Roger, Try the attached code. Obviously it needs to be renamed to autosilkUtils.il. Cheers, Dave

Attachment: autosilkUtils.il.RogerGreen.il
Dave Elder
Tait Electronics
roger.green@alspcb
Posts: 8
Online: User is Offline
9/12/2007 1:00 AM  
Dave

Magic thanks a lot for that, as I said before this is a fantactic bit of skill

Roger Green
Advance Layout Solutions
eswar
Posts: 0
Online: User is Offline
9/25/2007 10:47 PM  
Hi Dave

I am using allegro Ver 15.5 in which i am getting the following error.

E- *Error* axlGRPDrwInit: argument #1 should be any user-defined (other) type (type template = "otg") - nil

Can u help me out.
Dave Elder
Moderator
Posts: 150
Online: User is Offline
9/26/2007 1:47 PM  
Hi, That message indicates that the main form was not created successfully. A possible reason is that your form path is not set as expected. Check that "." is the first entry. (User Preferences/Ui_paths/formpath) Let me know if this helps CHeers, Dave
Dave Elder
Tait Electronics
leonlee
Posts: 81
Online: User is Offline
11/06/2007 1:01 AM  
Hi, Dave,

I have tried the routine you offered. It's useful to my problem. Thanks.

And I found a problem about the routine:
It runs successfully in PCB Design Expert , but there are some error in PCB design 220(PCB studio)

When I click the [b]DRC list[/b] in [b]DRC Browse Form[/b], the function cann't zoom to the target and tell me an error information:

E- *Error* setq/set: Variable is protected and cannot be assigned to - layerInfo

Could you help to check it?
Leon Lee
Schneider-Electric
Dave Elder
Moderator
Posts: 150
Online: User is Offline
11/06/2007 2:23 PM  
Hi Leon, I don't see that behaviour in 16.0. It possibly arises because the layerInfo variable is protected by another Skill function that you use in your environment. What version of Cadence are you using? Cheers, Dave
Dave Elder
Tait Electronics
leonlee
Posts: 81
Online: User is Offline
11/06/2007 5:07 PM  
My Cadence's version is still 15.5.1 s065(v15-5.1-43CF).
Leon Lee
Schneider-Electric
Dave Elder
Moderator
Posts: 150
Online: User is Offline
11/06/2007 7:01 PM  
Hi Leon, I have,'t got a copy of that release handy. Try loading the attached file. I have changed the variable name. Cheers, Dave

Attachment: autosilkUtils.il
Dave Elder
Tait Electronics
leonlee
Posts: 81
Online: User is Offline
11/06/2007 7:48 PM  
It's OK now, Yeah~~
Leon Lee
Schneider-Electric
BillZ_EMA
Posts: 51
Online: User is Offline
11/07/2007 5:58 AM  
Just a comment. I did a quick check and this skill routine launches and appears to work in version 16.0
I didn't do any extensive testing but didn't encounter any run errors.

Regards,
BillZ
EMA Design Automation
Posting to forums is available to community members only.
Login or Register
Forums > Silicon-package-board > Shared code - SKILL > How to check the mistaken Reference Text location


ActiveForums 3.6
     
Copyright 2006 Cadence Design Systems, Inc.