diving dimensions in drafting sketch 1

[SiW979]

Dimensions in a sketch are behaving erratically. I want to position a sketch to the edge of the model as a location to stamp a part number, however, when i select the sketch and the edege when applying the dimension, it says that some objects cannot be used to create driving dimensions, however it was working fin last week. Can any body help please?

Best regards

Simon NX7.5.2 - TC 8

http://www.jcb.com

 

[JohnRBaker]

Simon, could you provide us with at least an image, if not the actual file, showing what it is that you're attempting to do, preferably captured while you're in the sketcher clearly showing the objects which you're attempting to use to create the driving dimension?

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

http://www.siemens.com/plm

http://www.plmworld.com/museum/

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

 

[jerry1423]

Have you added features to the model since the last time it worked ? (last week)
Some of the edges may get renamed as new features are added ~ also make that sketch the "current feature" and work with it from there, it may be easier to see what is going wrong

 

[SiW979]

Ive captured a few screen shots in and bunged them on a pptx.

Best regards

Simon NX7.5.2 - TC 8 www.jcb.com

 

[JohnRBaker]

OK, The issue is that when creating a Sketch in the context of a Drawing, and you're working in the Master Model mode, that you are not allowed to create associative relationships, which a 'Driving' dimension does, between objects in the Drawing (the sketch curves) and objects in another part file (the edges of your model) which is actually a component in the Drawing file. Note that this is a limitation of the Sketcher and would be there even if you were attempting to create a Sketch in Modeling while working in the context of an Assembly and you tried to create Driving Dimension with some edge on one of the Assembly Components.

However, there is something which you can do which will give you exactly what you're looking for. Select the view you wish to create your sketch in (this can be done before or after the sketch has actually been created), press MB3, select 'Style'. Now while in the General tab, set the 'Extracted Edges' option to 'Associative' and hit OK. You can now go ahead and add Driving Dimensions between any of the Sketch objects and the edges of the model as seen in that view. And since the 'Extracted Edges' are associative, any changes in the model will be reflected in the Drawing and the Sketch will update accordingly.

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

http://www.siemens.com/plm

http://www.plmworld.com/museum/

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

 

[SiW979]

John

I tried that with the extracted edges and it didn't work, it still gives me the same problem of no option to create a driving dimension.

Best regards

Simon NX7.5.2 - TC 8

http://www.jcb.com

 

[JohnRBaker]

Make sure that you're actually selecting Curves and NOT 'Snap Points'.

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

http://www.siemens.com/plm

http://www.plmworld.com/museum/

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

 

[moudy1]

Also make sure you are selecting the view prior to changing the style or creating the view after setting it in preferences.