Manual Text on sketch dimensions

[NXConsultants]

Hi

A number of users that I support are seeing an issue with manual editing of sketch dimensions (non-driving) in NX7.5.3.3

Create a new (empty) view in drafting
Sketch shape in this view and add dimensions
Change dimensions to reference
Edit dimension text... The dimension reverts to the original value.

Any ideas?

The 'simple' solution of drawing everything to scale is not a solution in this case - the parts that I am dealing with are complex aerodynamic profiles that cannot be easily detailed. The views are for reference only to describe the lay-up of a composite laminated component, that need to be turned around in hours rather than weeks.

 

[JohnRBaker]

I've verified this behavior and have opened a PR. I'll report back what I learn.

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

http://www.siemens.com/plm

UG/NX Museum:

http://www.plmworld.org/p/cm/ld/fid=209

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

 

[NXConsultants]

Thanks for the prompt response John.

We're working around the issue with labels and leaders at the moment.

 

[JohnRBaker]

OK, this is a known issue and it will be addressed, however, it will be awhile before it's implemented since it's part of a larger project which we just started working on. However, there is still GOOD NEWS!

There's a workaround which will let you do exactly what you want as long as you do things in a certain order. If you add driving dimensions while creating your Sketch, as you've already discovered, even if you 'convert' them to 'Reference' they will not allow you to edit them.

What you need to do is create them as Non-Driving or 'Reference' from the beginning. So either add your regular sketch dimensions, edit the sketch until you get the size and shape that you wish and then delete those dimensions that you wish to edit, OR never create them in the first place.

Once your sketch is 'done', now add the dimensions, HOWEVER, after you select the first sketch object that you wish to add a dimension to BUT BEFORE you indicate the origin/location of the dimension itself you will notice that an option on the Dimension 'dialog bar' labeled 'Driving' will have become active. Just toggle it OFF and NOW indicate the location for the dimension. Once you've placed all of the 'candidate' dimension, you can go into...

Edit -> Annotation -> Text...

...and edit the numerical value of the dimension(s), thus turning them into 'manual' dimensions.

Note that once you've toggled OFF the 'Driving' option in the dimension 'dialog bar', it will remain toggled OFF until you again toggle it ON during a future dimension creation operation.

Anyway, give it a try. This should work for you until we resolve the issues which currently prevents you from doing this directly.

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

http://www.siemens.com/plm

UG/NX Museum:

http://www.plmworld.org/p/cm/ld/fid=209

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

 

[NXConsultants]

Excellent, that works.

Thanks John.