Home > Community > Blogs > PCB Design > what s good about allegro pcb editor associative dimensioning check out 16 5
Login with a Cadence account.
Not a member yet?
Create a permanent login account to make interactions with Cadence more convenient.

Register | Membership benefits
Get email delivery of the PCB Design blog (individual posts).


* Required Fields

Recipients email * (separate multiple addresses with commas)

Your name *

Your email *

Message *

Contact Us

* Required Fields
First Name *

Last Name *

Email *

Company / Institution *

Comments: *

What's Good About Allegro PCB Editor Associative Dimensioning? Check Out 16.5!

Comments(18)Filed under: PCB Layout and routing, PCB design, Allegro PCB Editor, Allegro, PCB Editor, PCB, layout, "PCB design", routing, SPB16.5, Allegro 16.5

With the Allegro PCB Editor SPB16.5 release we've enhanced the existing Allegro drafting dimensioning capabilities, so that when a dimension is created involving one or more design database objects the dimension will subsequently remain internally ‘associated’ with those objects as well. Subsequent editing operations such as the moving of an object can then appropriately and automatically update as required any dimensions that are associated with that object.

Read on for more details …

There's a great movie showing all the details that you can find on Cadence Online Support HERE !

The Allegro PCB Editor dimension environment is entered by selecting Manufacturing — Dimension Environment. While in the dimension environment you have access to the following commands which are available in the RMB pulldown.

Parameters               Invokes the Global parameters form
Show dimensions     Displays information on the dimension including if it is an associated dimension.
Align dimensions      Aligns dimension text. Select the master and then window select remaining text to align with the master.
Lock dimensions       Locks the location of the dimension text.
Unlock dimensions    Unlocks the location of the dimension text.
Z-Move dimensions   Allows you to move the dimension to an alternate Class/Subclass combination.
     Allowable class/subclasses
     Board Geometry/Dimension
     Board Geometry/Assembly Notes
     Board Geometry/Any User Defined subclasses
     Drawing Format/ Any User Defined subclasses
     Manufacturing/ Any User Defined subclasses
Delete dimensions   Deletes existing dimension text.
Move text                 Moves dimension text.
Change text             Allows you to change text strings.
Edit Leaders            Allows you to edit leader lines such as adding a vertex.


Instance based parameters

Along with the normal global parameters that you can set you can also set instance based parameters. Just as with instance based shape parameters, the text that is highlighted in blue allows for an instance to have a different parameter than the global setting.

In the image below the connectors were dimensioned with the global parameters and then an instance based parameter for the tolerance of +/- .01 IN was applied to the connector on the right.


In this example an instance based dimension that used dual dimension was applied with the secondary dimension being below the primary.


Migration from older releases

When upreving a design the dimensions will remain in a non-associated manner. In order to get the associative behavior, all dimensions, leaders etc. will have to be deleted and added back into the design.

Downreving a design to a previous release

All dimension elements will remain in the design however the association will be removed.

Frequently Asked Questions (FAQ):

How do I delete associative dimensioning?
You must use the “delete dimensions” command associated with the dimension edit environment.

What happens if I delete the object the dimension is attached to?
The dimension would be deleted as a result.

How do I move dimension leader lines and text?
Use the “move text” or “edit leaders” commands associated with the dimension edit environment.

After moving a component in the y-direction, the dimension text does not maintain its former y position. What can be done to maintain the former y location?
Consider using the “Lock dimensions” command to lock the text in place prior to moving the component.

What does the color blue represent in the parameter forms?
Parameter form changes apply to future dimensions that are added. They do not apply to existing dimensions.
Instance Parameter form – changes apply only to the dimension you select in the canvas.


Please share your experiences using this new 16.5 capability.

Jerry "GenPart" Grzenia


By Hardi on June 25, 2011
Hi,i am new user for PCB design.Is It possible that I have some tutorial on cadence 16.5??Or i can get any free webinar??Moreover,If any resources for I can download free version of 16.5 for my laptop use.
Thank you.

By Jerry GenPart on June 27, 2011
Hi Hardi,
Welcome to the Allegro solutions! There are tutorials, videos, new feature information, etc. all available to customers. As for webinars you can contact your Cadence Account Manager and they can direct you to scheduling a webinar.
Here are a few web sites that will help you obtain more details about Allegro PCB Editor:

By mario on January 17, 2012

but now i cannot mirror the dimension text anymore. It was possible in 16.3.

If I have to mirror the drawing upside down to see the bottom side for proper printing all dimension text is mirrored of course. To avoid this I was mirroring the dimension text in my actual drawing. Like I said, this is not possible anymore. Please, can you tell me how to do this now in 16.5??

Many thanks.

By Jerry GenPart on January 17, 2012
Hi Mario,
I asked one of our Allegro PCB Editor Support AE experts about this. He states - "I don't think this is possible with associative dimensioning although I would think that we should be able to add the dimension text as ‘mirrored' so that when the design is mirrored that the text is ‘correct reading’"
Jerry G.

By Bill O. on April 16, 2012
When datum dimensioning all of the text is place in the same direction.  How can I rotate the text  90 degrees so it is in the porper orientation.

By Jerry GenPart on April 16, 2012
Hi Bill,
I received the following details from one of our expert Allegro Support AEs:
I have dimension that I need to rotate. How can I accomplish this?
The ‘Align text with dimension line’ setting, either as a General or Instance parameter, can accomplish what you are asking for.
If you have dimensions already added to the design and wish to rotate these to be aligned with the dimension line select
Manufacture > Dimension Environment
Right mouse button “Instance Parameter”
Select, with the left mouse button, the dimension you want to rotate
In the’ Text’ tab of the Dimension Parameters UI select ‘Align text with dimension line’
Jerry G.

By Prahlad on August 22, 2012
Hi, Dimension is defined for PCB length. Is there any way, dimension update automatically, if PCB length is modifed afterwards?

By Jerry GenPart on August 23, 2012
Hi Prahlad,
Yes, in 16.5 Allegro PCB Editor provides associative dimensioning. This means that once an object is dimensioned, if the object is moved the dimension will update to reflect that change.
Prior to 16.5 you would have to manually update the dimension.
Jerry G.

By Maria on November 14, 2012
Is it possible to delete a single dimension in 16.5 without deleting all other associative dimensions? For example, I put in the datum 0 on x axis but was not happy where it landed.  Instead of stopping dimensioning of all other objects and removing this mess-up first, I finshed  dimensioning the rest of the board.  Now when I try to delete only the messed up dimesnion, all other dimensions disappear as well.

By Jerry GenPart on November 14, 2012
Hi Maria,
I've checked with one of our Allegro Customer Support experts and he indicates that when you delete a dimension it should not delete the others. He asked about the 16.5 HotFix versions you're using. It might be best to file a new Service Request at http://support.cadence.com.
Jerry G.

By Peter Cerbone on March 19, 2013
How do I de-assoicate the dimension from the board outline?   Is there a work around?

By Jerry GenPart on March 21, 2013
Hi Peter,
We don’t have any method of removing dimension association.
If the board outline is on grid you could select grid points that are close to the corners of the board. In this way the dimensions would be correct for the board outline, but would not be associated.
Could you explain why you don’t want to have the dimensions associative?
Jerry G.

By Rz on July 17, 2013
Is there any way to "break" a dimension element into it's native line, shape, and text elements so it can be manipulated outside of the dimensioning environment?

By Jerry GenPart on July 22, 2013
Hi Rz,
Currently, there is no method of breaking or exploding dimensions into native elements.
Jerry G.

By Rz on July 26, 2013
Thanks Jerry - I determined a way to work around "exploding" dimensions by using the "create detail" command.  It's not a perfect solution but it's something...

By Jerry GenPart on July 26, 2013
Hey - thanks Rz for posting the workaround and sharing it with the community!
Jerry G.

By Dhamodharan on July 3, 2014
Hi..  i am new to pcb editor. When i am using the dimension environment , whether i am moving the dimension means can i view the dim text parallely with cursor moving.In OrCAD Layout 16.2, when ever we dimension means, the dimension and text will be mover parallely,but that option is not get enabled in editor.
(Ex:-) If i am select the dimension at particular grid to other grid means, the distance take from particular grid is took  as zero distance and from there, the dimension is get is marked. This is been done in layout. But in editor it is not possible.. Any person provide the solution for this problem.  Thanks & Regards Dhamodharan

By Jerry Grzenia on July 4, 2014
Hi Dhamodharan, You might want to contact your local Cadence Customer Support team at http://support.cadence.com. They can assist you with this question.Jerry G.

Leave a Comment

E-mail (will not be published)
 I have read and agree to the Terms of use and Community Guidelines.
Community Guidelines
The Cadence Design Communities support Cadence users and technologists interacting to exchange ideas, news, technical information, and best practices to solve problems and get the most from Cadence technology. The community is open to everyone, and to provide the most value, we require participants to follow our Community Guidelines that facilitate a quality exchange of ideas and information. By accessing, contributing, using or downloading any materials from the site, you agree to be bound by the full Community Guidelines.