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Sketch revolve Dimension??

Experimenter
Experimenter

I'm try to create a diameter dimension in a sketch that I will use for a revolve extrude.  I can't seem to find away to do this I know I can create a dimension and use expressions but would like not to do that.  I attached a pic to clarify what my intent is.

 

Thanks 

8 REPLIES

Re: Sketch revolve Dimension??

Legend
Legend

Hi @ryan2333,

it's not possible. Open an ER.

I can suggest a workaround, create a mirror line, but it's stupid to create a line for this scope.

Thank you...

Using NX 11 / RuleDesigner PDM

Re: Sketch revolve Dimension??

Phenom
Phenom

Following is what I found in NX way of doing it.

  1. Add a point at the LHS of the centre line

  2. Click the command “Make Symmetric”

  3. For objects click the point (@#1) and a vertex at RHS. Click the Centreline thereafter.

  4. Reconfigure the Radius dimension to diameter dimension (=Delete and recreate)
Michael Fernando


Die Designer
NX 11.0.2.7 + PDW

Re: Sketch revolve Dimension??

Siemens Phenom Siemens Phenom
Siemens Phenom

If you're trying to use the Cylindrical Dimension type, the first object needs to be a centerline.  Since you can't create a centerline in a sketch the cylindrical dimension will not be doubled in value (true diameter), but will only show the radius.

 

Regards, Ben

Re: Sketch revolve Dimension??

Phenom
Phenom

NX Sketch limitations.

Michael Fernando


Die Designer
NX 11.0.2.7 + PDW

Re: Sketch revolve Dimension??

Phenom
Phenom

Other method; check the attched part.

Michael Fernando


Die Designer
NX 11.0.2.7 + PDW

Re: Sketch revolve Dimension??

Legend
Legend

Hi @BenBroad,

your solution can be used in drafting mode and when you use detail view where only a part of diameter is visible.

Using your solution put the whole dimension value in half sketch. Can create confusion during the interpretation.

If you import dimension on view via 'Feature Parameter', NX imports half dimension.

There are workaround that doesn't give a real advantage.

Thank you...

Using NX 11 / RuleDesigner PDM

Re: Sketch revolve Dimension??

Siemens Phenom Siemens Phenom
Siemens Phenom
Based on the image that was uploaded it looked to me like the cylindrical dimension type was being used. I simply pointed out that it cannot be used to create a true diameter dimension in the sketcher and that it shows the radius. I wasn't suggesting that this option be used - I was simply pointing out that it wont produce the desired result as it can in Drafting.

Re: Sketch revolve Dimension??

Legend
Legend

@BenBroadyou have right.

 

Thank you...

Using NX 11 / RuleDesigner PDM