Sketches in Drafting - Hiding Dimensions

[OS80RNE]

Hi,
The sketcher in Drafting has only just become suitable for the type of tasks I need to perform, but one problem remains; can I turn off the dimensions once I have finished the sketch, such that they are still driving the sketch but are not visible on the drawing sheet?
Thanks,
Mark

NX8.5.3.3

 

[JohnRBaker]

You can always simply 'Hide' them.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
Cypress, CA
Siemens PLM:
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To an Engineer, the glass is twice as big as it needs to be.

 

[Crocostimpy]

Speaking of which, is there a trick to making the sketch dimensions driving when sketching in a drawing? I usually want them driving but rarely does it happen. I think they're blue when they're driving and yellow when driven. Mine almost always end up yellow.

Mike

 

[JohnRBaker]

I get Expressions for each Drawing Sketch Constraint dimension created and editing those expressions will update the sketch, just like it does in Modeling.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[Crocostimpy]

I'll have to try that next time, but I'm skeptical. I thought the point of Driven dimensions is that they report a measurement but cannot be changed by themselves. Something else needs to change for them to update.

Do I have the terms correct? Driving dimensions can have their value modified to affect a change in geometry, while driven dimensions can't.

Mike

 

[cowski]

Crocostimpy,

In drafting, there are three types of dimensions that you can use:
[ul]
[li]drafting dimension (driven by geometry)[/li]
[li]sketch dimension (driving an expression which drives geometry)[/li]
[li]sketch reference dimension (driven by an expression which drives geometry)[/li]
[/ul]

If you are in a drafting sketch, select the objects you want to dimension but before placing the dim, make sure the 'driving' option is turned on.

If the 'driving' option is turned off while placing the dimension, you will end up with a normal drafting dimension object. After you place a sketch dimension you can convert it to a sketch reference dim (or vice-versa), but I know of no way to convert a drafting dim to a sketch dim (or vice-versa).

www.nxjournaling.com

 

[Crocostimpy]

I have never seen that Inferred Dimension menu before. That would certainly help! I'm going to look for it right now.

Thanks!


Mike

 

[cowski]

Crocostimpy,

What version of NX are you running? I was answering your question in reference to NX 8.5, but now I realize that is the OP's version, not necessarily your version...

The dimension 'toolbar' pops up when placing dimensions in the drafting application. It is also in NX 7.5, but I'm not sure about earlier versions. In NX 9 the 'toolbar' is gone, you'll have to change the 'driving' option in the dimension dialog.

www.nxjournaling.com

 

[Crocostimpy]

I'm in NX9 so I guess it's not there. I've seen the option in the dialog but most of the time it's greyed out. That's why I asked if there was a trick or something. Or maybe I was selecting wrong.

Mike