! in sketch constraint 1

[BOPdesigner]

I know what the ! means when it is in the file name header in you NX window, but I now have a case where I have a ! in a sketch constraint in the sketcher. How can this happen? Without deleting and reapplying the constraint(s), is there a way to fix it? In the current state, the constraint is not working properly. NX 6.

 

[JohnRBaker]

OK, what this means is that some object (generally an edge or a face) which you referenced when you constrained your Sketch has since either been deleted or is no longer reference-able by the Sketch. Note that the constraint has not been deleted, it has just been made ineffective or 'out-of-date' (which will be noted in the Part navigator). This can happen to both geometric constraints as well as dimensional constraints.

To see what I mean, open the attached simple example and note that at the moment everything is OK. Now enter the Sketcher editor (be sure to use Edit-With-Rollback) and you will note that there is both a Collinear Constraint and a Dimension with references edges which were blended AFTER the sketch was created, which is not a problem since those edges are there when the sketch updates in timestamp order.

Now leave the Sketch task and go to the Part Navigator and reorder the blends by dragging them so that they appear BEFORE the Sketch in the timestamp ordered list of features. Now note that the sketch will be flagged as out-of-date and if you now go to the sketch editor you will see that the one dimension and the one collinear constraint are flagged as being out-of-date, because the edges are no longer there during the timestamp ordered update of the model.

Now the system didn't delete anything, it just created some temporary 'reference' geometry so as to maintain the integrity of the sketch, but these two constraints will be ignored if the model is edited, for example if you were to change the X and Y values of the block size from 100mm to say 200mm. However, even if you did edit the block in this manner, if you then went back to the Part Navigator and reordered the two Blends so that they were once again shown as having been created AFTER the Sketch, the model will update properly. So the Sketch doesn't ever 'forget' what your original design intent was, just that at the moment it can't honor it because of some other operation which was performed which affected some object(s) which had been referenced by the Sketch.

Anyway, look at my attached example and manipulate it as I've described above and perhaps this will help show you what may have happened to your model.

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.org/museum/

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

 

[BOPdesigner]

That is exactly what had happened. Thanks for the detailed reply.