sketching bug?

[opetrenko1]

is it a bug or a "feature" :
sketching dimension set to be equal to reference dimension is allowed but does not drive the sketch.
In the attachment I set p5=p4, but it does not do anything (NX9).

 

[cowski]

When a dimension is created in the sketcher it is tied to an expression; if/when the dimension is converted to reference, the association between the dimension and expression value is suppressed - the expression no longer updates when changes are made to the sketch. If/when the dimension is converted to driving, the association will be restored.

That said, I don't know if I'd call it a "feature" or a "bug"; more like an operation that is allowed, but is not useful.

For the situation in your attached file, I'd suggest creating a line between the endpoints then making the vertical line "equal length" to the new line. This will work even if you convert the new line to reference.

www.nxjournaling.com

 

[JohnRBaker]

No, this is working exactly as intended.

When you convert a 'Driving' dimension to 'Reference', the expression that was originally used to control this dimension, in your example that would be 'p4', is NOT deleted since it might still be of importance to your design, just that it's now a bit of an orphan. Granted, if you go to the Expression editor you will see that while 'p4' still appears to be linked to the now 'Referenced' dimension, you will also see that it's value is actually what it was at the time that the dimension was changed to 'Reference', not it's current value since by definition, the 'Reference' dimension is no longer driving anything. And in this state, you can see that 'p4' actually IS driving the value of 'p5'.

Now the reason that NX still seems to be linked to that now 'Referenced' dimension is that if later on you decided to convert the 'Reference' dimension back to a 'Driving' dimension, it will be reassigned the original 'p4' expression (give it a try and you'll see what I mean). That way the original 'Design Intent' is never lost. What this allows users to do is to temporarily set one or more dimensions to 'Reference' as a way to help mange some other dimension/constraint actions, giving the user a chance to utilize a sort of 'Trial & Error' workflow to help flesh out the final dimension/constraint scheme.

Anyway, after awhile I think you'll see that this can be a very useful feature.

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

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

 

[opetrenko1]

Thank you for confirming, gentlemen.

Still I disagree.
1) it's not an orphan, it has parents it depends on. It is driving dimensions that are usually orphans. Reference dims. are put to measure what's established by driving dims.
2) all dependency graphs start with orphan nodes and end with children.
3) John, design intent actually gets broken. I switch driving dim. to ref. either to a)measure or b)to drag lines around, so I see how geometry behaves. So if I had design intent say, height = 2* width, I'd like to see that intent being maintained when I turn width to reference and drag it back and forth. But in this case height gets frozen unless I turn it to reference too. So, I'm not sure how prohibiting ref. dims to have kids in both of the cases: a) letting a measurement drive geometry b) maintaining design intent while relaxing a dimension and moving lines around. But my experience with sketcher is limited, so I'm sure I'm missing something.

by the way, earlier NX6 allowed me to change driving dimension by dragging a slidebar. Somehow, I can't find it...

Thank you

 

[phillpd]

To get to the slider, from within the Sketch, go to Menu->Edit->Sketch Parameters

NX 9.0.3.4
NX 10.0.3.5 (Testing)
Windows 7 64 (Windows 8.1 Tablet)

 

[JohnRBaker]

If a 'Driver' dimension could be controlled by the value of a 'Reference' dimension, this could potentially lead to a circular reference. which cannot be tolerated. For example, what if it were either the expressions 'p2' or 'p3' in your sample sketch which were using 'p4' in their formulas and it was possible that 'p4' did update when the sketch was updated? How would you expect NX to behave?

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

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

 

[opetrenko1]

John,
circular references could happen with driving dimensions as well.
Try to set p1=p2 and p2=p1 and NX9 will just ignore last entry without warning.

I understand that driving dims. dependencies are written explicitly, and it's trivial to catch circular refs. on the explicit dependency graph.

So the true reason is inability of the sketcher's engine to catch implicit circular references. (I wonder if other CADs can do this)

Thank you for clarifying

 

[MFDO]

@opetrenko1,
I can confirm that in my previous Software,I always used this parametric capability to drive many functions, timing and to automate the design process.

Michael Fernando (CSWE)

http://www.solidCADworks.com

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