Contact US

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Linear to GD&T Dimensioning

Linear to GD&T Dimensioning

Linear to GD&T Dimensioning

In Creo 4.0 if you know that you want your finished model to be parametric and to have holes located as basic dimensions coming from particular datums, do you have to create the model as such initially, or can you just locate the holes in the model using the linear dimensions coming from the default edges of the part and then afterwords create GD&T basic dimensioning from different datums and then delete the original linear dimensions from the model?

RE: Linear to GD&T Dimensioning

People who dimension the model to behave one way and show an entirely different scheme on the drawing are just causing a huge problem. Sure, it can be easy for them, but when it comes time to make any changes? 10X the work that was "saved."

Obviously you can redimension the model at any time and use those dimensions on the drawings; the best choice is "Replace" in the sketch or reroute existing features.

RE: Linear to GD&T Dimensioning

I agree with 3DDave. One of the strengths of Pro/E is the ability to use the sketch driving dimensions on the finished drawing. Every time you create anything in Pro/E you are creating relationships between the references and the object. It's best to put a little thought in up front and do it right. It can be a nightmare working on a model where the driving dimensions are completely different than the drawing and changing one part dimension changes 6 things in the drawing that you might not notice.

There are those (usually saladworks users) who completely ignore this and just dimension the drawing with created dimensions. I hate them.


The Help for this program was created in Windows Help format, which depends on a feature that isn't included in this version of Windows.

RE: Linear to GD&T Dimensioning

Or you have designers who have been using Creo since the days of Pro/E 18 and all they do is use created dimensions because 'that is how they did it on the board'!

I will admit most of our parts are one off unique, but the designers give very little thought to utilizing the parametric aspect of the software. I have seen many parts where the drawing dimensions from one end but the positioning in the model is from the other end of the part.

"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

RE: Linear to GD&T Dimensioning

When it is time to create the drawing, I plan to bring in the dimensions from the model. I want the model and the drawing to be parametric. I was just wondering if you could locate holes in the model from the default edges that CREO dimensions from and then later while you are still working in the model, go back and while leaving the holes where they are on the part, redimension their location from different datums and delete the original location dimensions. Can this be done?

RE: Linear to GD&T Dimensioning

Either redefine the feature and change the sketch or reroute the feature references. If you use Replace in the sketch the new dimension takes the place of the old one; no need to delete the original dimension, it will be removed by the Replace process. If the feature references are rerouted the dimension references are changed and again, no need to delete the related dimension(s). If there is a sketch you can add reference dimensions to ensure the feature doesn't change in undesired ways.

If you are using hole features, the reference markers can be dragged to new references.

RE: Linear to GD&T Dimensioning

Yes, the replace functionality in section redefine will automatically remove the old and place the new dimensions in the drawing. Very slick. It's even better to do it right the first time.


The Help for this program was created in Windows Help format, which depends on a feature that isn't included in this version of Windows.

RE: Linear to GD&T Dimensioning

Thanks to all of you for your help.

RE: Linear to GD&T Dimensioning

generally speaking, the first thing I do is create my control frame before modeling (usually its just renaming the top, right and front datums)

whenever I am teaching people ProE I always tell them this is the foundation to your model, use it


Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members! Already a Member? Login


Low-Volume Rapid Injection Molding With 3D Printed Molds
Learn methods and guidelines for using stereolithography (SLA) 3D printed molds in the injection molding process to lower costs and lead time. Discover how this hybrid manufacturing process enables on-demand mold fabrication to quickly produce small batches of thermoplastic parts. Download Now
Design for Additive Manufacturing (DfAM)
Examine how the principles of DfAM upend many of the long-standing rules around manufacturability - allowing engineers and designers to place a part’s function at the center of their design considerations. Download Now
Taking Control of Engineering Documents
This ebook covers tips for creating and managing workflows, security best practices and protection of intellectual property, Cloud vs. on-premise software solutions, CAD file management, compliance, and more. Download Now

Close Box

Join Eng-Tips® Today!

Join your peers on the Internet's largest technical engineering professional community.
It's easy to join and it's free.

Here's Why Members Love Eng-Tips Forums:

Register now while it's still free!

Already a member? Close this window and log in.

Join Us             Close