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: NC Legend
Posting to forums is available to community members only.
Login or Register
Rate this topic:
   
Author Messages
roger.green@alspcb
Posts: 8
Online: User is Offline
7/13/2007 7:52 AM  
Hi All Does anyone know how to change the tolerance '+0.00/-0.00' to text 'SEE BELOW' or something, if the tolerance is 0 in the pad and only display the tolerance if set. Cheers.
KenM
Posts: 18
Online: User is Offline
7/16/2007 7:01 AM  
you can change it in MANUFACTURE > NC > DRILL CUSTOMIZATION.
roger.green@alspcb
Posts: 8
Online: User is Offline
7/16/2007 8:34 AM  
Thanks for your reply, it's not quite what I was after. What I was trying to say, but I don't think that I explained it very well, is if you are using the tolerance in the .dlt file but is comes out with +0/-0 then I would like it to say something other than +0/-0 i.e. See Below.
mcatramb91
Posts: 141
Online: User is Offline
7/16/2007 9:30 AM  
I sort of see what you are trying to do but as far as I can tell there is no mechanism to do what you are asking.

You can make the tolerance field a USER Defined field, which would force you to specify the tolerance for ever hole size used on the design inside of the default-mil.dlt file, I would not recommend this but it was worth mentioning.

The first suggestion to use MANUFACTURE > NC > DRILL CUSTOMIZATION is the easiest and best way to go and you can change all the tolerances that are +0/-0 to your default tolerance. The other added benefit in using the Drill Customization is the tolerances defined in the database will be added to the NCdrill files generated out of Allegro so there is no confusion or conflicting information between the NCdrill data and the NCdrill Legend on your documentation.

I guess a good enhancement request would be "Any Padstack with a tolerance defined as +0/-0 should be replaced with a default tolerance specified in the Allegro .brd database" or "The ability to globally replace all the hole sizes with a tolerance of +0/-0 inside of NC Drill Customization with a default tolerance" - Currently the Drill Customization global change applies an updated tolerance across all hole sizes regardless of what they are defined in the library.

Hope this helps,
Mike Catrambone
UTStarcom, Inc.
oscar@oqo.com
Posts: 18
Online: User is Offline
12/05/2007 11:22 AM  

create a custom padstack. for specific holes with "see text below" create another copy of a 10mil drill and rename it using a 10.01mil drill.

Modify your drill table file. Located in your share folder. cadence folder\share\pcb\text\nclegend\default-*.dlt. When you generate nclegend the gui points to this file.


open default-mil if your using mils using notepad, make your mods and save in the same folder. create a backup zip just incase it breaks.

heres my example:

(make__ncTemplate_struct
?Name "custom DRILL CHART by Oscar Miguelino"
?Title "DRILL CHART"
?Units "mils"
?TitleHeight 250
?TitleTextBlock 9
?ColumnTitleTextBlock 8
?DataTextBlock 8
?PlatingOrder "PlatedFirst"
?ColumnDefinitions '(
("Figure" "FIGURE" 7)
("User" "SIZE" 13)
("User" "TOLERANCE" 14)
("PlateStatus" "PLATED" 10)
("Quantity" "QTY" 6))

?CustomData '(
( 10.01 "PLATED" "0.010" "+0.0/-0.0 SEE TEXT BELOW" PLATED) ( 10 "NON-PLATED" "0.010" "+/-.003" )
( 11.01 "PLATED" "0.011" "+0.0/-0.0 SEE TEXT BELOW" PLATED) ( 11 "NON-PLATED" "0.011" "+/-.003" )
))
Posting to forums is available to community members only.
Login or Register


ActiveForums 3.6
     
Copyright 2006 Cadence Design Systems, Inc.