Breaking feature dependencies?

[CNSZU]

Hello,

Here's the problem: I'm trying to move a sketch to a location earlier in the part navigator. But when I do that, an extrude feature gets moved as well and placed right before the sketch. That's because the extrude feature somehow is a parent to the sketch, and therefore automatically gets moved together with the sketch. I do not know how the extrude feature became a parent of the sketch. It was never intended to be a parent, or, if it once was an intended parent I now want to break that dependency. So, in order to move the sketch without the extrude feature being moved simultaneously, I need to break the dependency(ies) the sketch has to the extrude feature. Without knowing how it became the parent, it will take a lot of detective work to find the dependencies and delete them. One way to do it is to open the sketch, look at the Show/Remove Constraints dialog and sift through every single constraint in the sketch until I find the offending constraints and delete them.

Is there an easier and faster way to break the dependency between a child and parent? I thought that perhaps you could in the Dependencies panel right click a parent and select "Remove Dependency" but there doesn't seem to be a command like that.

NX9 Win8.1 64bit i7-3770K 16GB Quadro2000

 

[JohnRBaker]

That depends on how you created your Sketch and exactly what aspect of the Extrude feature is being referenced. Now if it was as simple as attaching the Sketch to one the faces of the Extrude then all that you have to do is create a Datum Plane and then reorder it so that it appears AHEAD of where you want the Sketch 'Timestamp' to be. Now edit the Sketch using 'Edit with Rollback' and when the Sketch ribbon appears, select the 'Reattach' icon near the Left side of the ribbon and when asked, select the recently reordered Datum Plane and hit OK. Now close the Sketch task and go back to the Part Navigator and reorder your Sketch.

Now if you referenced any of the faces or edges of the Extrude feature while creating Sketch constraints then it may be a bit trickier as you'll need to create some new objects, Datums and/or Curves, reordering them AHEAD of where you want the Sketch and then edit the Sketch constraints replacing the references faces/edges of the Extrude using the recently created and reordered Datum/Curves.

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

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

 

[CNSZU]

Often when creating a sketch, because Create Inferred Constraints is turned on, a sketch start/end point would inadvertently get "attached" to the edge of a previously created feature without me knowing it. Since in the beginning of creating a part I would sketch "loose and fast", this doesn't matter. It's only when trying to reorder a sketch that this sometimes becomes a problem. Therefore a command to "force break" a relationship between features would be useful. This command would automatically delete all references (constraints and sketch plane) to the specified parent. Or at least, in the Show/Remove Constraints dialog to include an option for "External" which would only list the constraints to external features. This would really help me weed out the constraints I don't want.

NX9 Win8.1 64bit i7-3770K 16GB Quadro2000

 

[JohnRBaker]

Unfortunately those relationships are actually part of the definition of the Sketch. That's why you have to 'edit' the Sketch to change those references. What I'm saying is that the Sketch can't really exist without REPLACING the original relationships with new ones.

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

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

 

[TheeCircle]

I would also check out a software called Spaceclaim for modifying solids/ surfaces. Many mold shops are using it as it is simple to modify/ repair models.

 

[JohnRBaker]

The approach used by 'Spaceclaim' to modify Solid/Suface models is what's known as 'Synchronous Modeling' in NX, which is based on technology that has been available, free-of-charge (with each Feature Modeling license), in UG/NX since 2000 with the release of Unigraphics V17.0.

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

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

 

[TheeCircle]

Hi John,

I am aware of that feature but will it work with non native solid or surface files?

 

[JohnRBaker]

Of course it will! That's one the primary reasons that we initially developed this technology nearly 14 years ago.

For more information about 'Synchronous Technology' and how it can be used to support multi-CAD workflows, go to:

http://www.plm.automation.siemens.c...oductivity-tools/synchronous-technology.shtml

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

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

 

[TheeCircle]

Thanks John!

 

[jerry1423]

Actually some of the features that are within Syncronous Modeling have been with Unigraphics (NX) for something like 23 years, and were part of the Edit Face commands (I think since UGv7). They became more robust with Syncronous Modeling.