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Duplicate Reference Dimension

Hey folks

 

Is there a quick way within a sketch to duplicate (but use for real) a reference dimension? I know I can exit the setch, create a distance/angle measure with a pX value and refer to that back in the sketch but that seems convoluted.

 

Attached is an example sketch. The angle highlighted in red is a reference dimension. I would like to assign the same angle between the lines of length 240 and 60. I could probably use some symmetry here but I would like to learn if there is another way to refer to the ref dim as there might not be symmetry in future cases.

 

Thanks!

 

6 REPLIES

Re: Duplicate Reference Dimension

Siemens Phenom Siemens Phenom
Siemens Phenom
You don't need to exit the sketch. Go to expressions and you will see a pxx value for the reference dimension. Apply the anglular dimension between the 240 and 60 lines, and set the value to the pxx value of the reference dimension.

In cases in the future where there is no symmetry, just edit the dimension to be the desired value.

Re: Duplicate Reference Dimension

Gears Esteemed Contributor Gears Esteemed Contributor
Gears Esteemed Contributor

Bear in mind that the expression for the reference dimension does NOT update when the model updates. When you convert a dimension to reference, the expression value is "frozen in time" until you change the dimension back to driving. The value shown by the reference dimension will update in the graphics window (it will act like a measurement), but the expression associated to the reference dimension will not update.

Re: Duplicate Reference Dimension

Gears Esteemed Contributor Gears Esteemed Contributor
Gears Esteemed Contributor

I'm not sure, but I think the angle expression is a feature.

To measure the current value it has to be after the sketch.

But then it would not be available for the sketch to use?

Ken Akerboom Sr CAx Systems Engr, Moog, Inc.
Production: NX10.0.3.5 MP16/TC11.2
I'd rather be e-steamed than e-diseaseled


Re: Duplicate Reference Dimension

Yeah I did look for such an expression but I don't think it creates one which is the problem. I've attached a screenshot of my expression window.

 

Edit: To clarify, the expression would be equal to 170.8 and be between Line 6 and Line 7..

Re: Duplicate Reference Dimension

Gears Esteemed Contributor Gears Esteemed Contributor
Gears Esteemed Contributor

Looking at the PNG you posted.

Down at the bottom is an icon "F(X)"

Just to its right is one with a ruler

If you "drop list" the ruler one (measure distance), you will see a "measure angle" one - pick that & measure the angle between the lines.

But it will probably crceate a feature, which you can't use.

 

Best idea I can think of (if a straight "mirror" of the curves won't work) is

1) Mirror the 2 lines

2) Set them reference

3) create the profile, and make the profile lines parallel (or co-linnear) to the "reference" lines

 

This way the new profile curves can have different lengths, etc. than the originals, but they maintain the angle.

 

Another option is to make the angle a "driving" expression for the sketch.

Or make a 2nd sketch for the "other half" of the profile

Ken Akerboom Sr CAx Systems Engr, Moog, Inc.
Production: NX10.0.3.5 MP16/TC11.2
I'd rather be e-steamed than e-diseaseled


Re: Duplicate Reference Dimension

yeah thanks ken

 

so creating the angle measure exits you from the sketch and also do not update. i guess there is no answer to this it's just not an option in the software. i think switching which are driving dimensions isn't optimal because it may lead to rounding errors if i'm copying the ref dims but yes, now i think about it this is probably always (not matter the geomtry) reproducible by creating some reference lines with geo constraints and referring back to them. just a couple of extra steps.

 

thanks guys