Linear to GD&T Dimensioning 2

[Worker7]

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?

 

[3DDave]

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.

 

[dgallup]

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.

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[looslib]

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.


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Ben Loosli

 

[Worker7]

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?

 

[3DDave]

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.

 

[dgallup]

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.

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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.

 

[Worker7]

Thanks to all of you for your help.

 

[Korichnevijgigant]

@Worker7
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

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