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modify nominal dims - Is there an equivalent to "OUT OF SCALE" in NX? 1

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ingallspw

Mechanical
Mar 17, 2009
178
Is there an equivalent to "OUT OF SCALE" in NX?

In I-deas there is a check box that is labeled "OUT OF SCALE". If you check it you can now modify the nominal of the dimension that I-deas is actually measuring.

For instance if you have a thin curved piece of plastic that deforms after it is molded and the model no longer is exactly what the actual finished part is and all you care about is that the finished part is with in tolerance, how do you change that nominal dimension to call out the actual real life measurements?

Thanks!

Keegan
 
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You can edit dimension text, and there is an "out of scale" symbol that can be used.

To edit text, Edit -> Annotation
and to add "out of scale", Annotation Style -> Dimensions -> last selection in dimension tol type pulldown

"Good to know you got shoes to wear when you find the floor." - [small]Robert Hunter[/small]
 
Manually entering text for a dimension value is highly discouraged for a number of good reasons, but if you decide to live with the possible consequences here is how to do it:

The menu entry location depends on which version of NX you are using, on older versions it was 'Edit' -> 'Text'; on newer versions it is 'Edit' -> 'Annotation' -> 'Text'. Activate the command then choose the dimension you wish to change, enter your desired text. When you change the value you will get a warning about losing the dimension associativity, think one last time about what you are doing and choose accordingly.
 
There is no explicit function to do this in NX (I guess the theory was to not make this TOO easy) however the procedure to do this is as follows. With your drawing displayed, go to...

Edit -> Annotation -> Text...

...and select the actual dimension you wish to edit and you will see the value of the dimension in the 'Text Input' box. Now just make your changes, being aware that you WILL be warned that you're converting the true dimension into a manual dimension (we warn you because this process can NOT be reversed, that is you can't convert a 'manual' dimension back to being a true dimension, you'll have to delete and recreate if that is needed).

Now once this is done, you may wish to assign an 'out of scale' designation to the dimension, generally an underline. To do that select the dimension, press MB3, select 'Style', go to the 'Dimension' tab, and in the 'Precision and Tolerance' section, set the dimension format to 'Not to Scale' (the last option on the list) and hit OK.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

To an Engineer, the glass is twice as big as it needs to be.
 
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