NX10: Sweep not updating as it should (or is it?). Unsure about functionality.

[Nougatti]

Hi there
I'm making a quick overview model of a penstock for a power plant and I'm constructing one of the bends with parametric modelling.
The bend is a 135 degree bend (path deviates to 45 degrees from horizontal) comprised from several straight pipe sections angle-cut and welded together.

With parameters and geometry I can define the small pipe sections from this info:

-Inner and outer diameter (profile/section of my sweep)
-Bend radius (R=4200 mm)
-Bend angle from horizontal (45 degrees)
-Number of sections (for example 5)

Each section will make up alpha = (45/5) degrees of the final bend and will be 2*R*sin(alpha/2) mm long.

I make bend by first sketching up the theoretical "perfect bend" with an arc and the correct measurements:

I then start a new sketch which I will put my first section onto:
Its start is at origin and its end is somewhere along the arc. p10 defines its length (from the parameter above).

I perform a curve pattern with n repetitions and a (45/5) degree spacing around the center point of the arc. The end result is five connected lines which are perfect for a sweep:
I make sure to pick the curves as Feature Curves so that Sweep knows that it should pick whatever lines it finds in the two sketches and not any specific ones:

Gorgeous, quick and easy

But as soon as I change the n (number of sections) the Sweep refuses to update and trying to open the feature and update it manually by rechoosing the sketch gives me the error message:
"Alerts: Smooth guide objects required for inner hole profile objects"

I need to delete the sweep feature and create a brand new one based on the same sketches in order to not get the error message.

What does this mean? I know sweep doesn't require smooth guides, and after all it works perfectly fine unless I update either of my parameters (even if I just change the radius). WHY?

Cheers

Daniel

---------------------------
I am Norwegian.
I design mechanicals for hydroelectric powerplants.
I use NX 10.0.3.5 and ANSYS 16

 

[Nougatti]

I am aware of other solutions to perform the same task. My current solution is to sweep the outer perimeter first and then the inner perimeter along the same path with a boolean subtraction against the first.
This updates just fine with whatever parameter changes I throw at it.

I'm just confused as to how my first approach would work in the first place and then not work at all when a value changed.

---------------------------
I am Norwegian.
I design mechanicals for hydroelectric powerplants.
I use NX 10.0.3.5 and ANSYS 16

 

[Toost]

I wonder if this isn't an old situation which have been forgotten by the developer ...
The functionality has been enhanced when creating the feature but not on updating.
Call GTAC.

Regards,
Tomas

 

[JohnRBaker]

Rather than using the 'Feature Curves' for your Curve Rule, I would try using 'Connected Curves'. It might prove to be a bit more reliable in terms of getting the correct order of the curves selected, particularity after an update where the number of curves may have changed.

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

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