Variational sweep 1

[ds4378]

I´m trying to understand how the Variational sweep works, but I fail.

The first surface I have made a simple section that I want to follow the guide. The sweep does not follow the guide instead it creates a surface with a strange shape. Why?

The second surface on layer 2 I have a simple section that I want so follow the same guide but I have added a section "Through point" at midpoint of the guide. The resultant surface does not pass that point. Why?

And finally how can I make the section follow two guides? I´ve seen examples of the possibility but again I fail to create that.

 

[Toost]

I opened your part in 7.5.
I cannot reply to all your questions, but i would make a 90% guess that the strange results you see all depend on the guide curve.
It seems to be both torsionally twisted and it contains a C1 knot.
( Non- smooth)
Try editing the guide and set it degree 4, then try again to create the variational sweep. ( degree 4 should force the knot be C2)
Only increasing the degree did not update the sweep for me.

You can constrain the sketch to multiple guides IF you in the sketch create Insert - curve from curves - intersection point and ( and set constraints to that point(s))

 

[JohnRBaker]

When asking specific questions about functionality PLEASE INDICATE WHAT VERSION OF NX THAT YOU'RE RUNNING!!!!!!

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.

 

[ds4378]

Thank´s Toost for your answer. I have tried to do as you recommended. It became better when I made the guide smoother but the section still looked strange. So I have made a new guide in one plane, a simple 3 degree spline just to get it to work. Then I made the two variational sweep as in the earlier attempt. The result is not what I would like to have. The section does not follow the guide.

My attempt with two guides failed again. I got an alert as the attached picture and I didn´t manage to orient it to create a surface.

I have run the CAST training successfully so there must be something I miss about the options.

By the way I run NX6.

 

[capnhook]

Info > Part > Part History is your friend.

This part was built with NX 6.0.3.6

Proud Member of the Reality-Based Community..

 

[ds4378]

The NX file is attached here.

 

[JohnRBaker]

I KNOW what version it was created on, I was just trying to make the point that we can avoid a complete 'cycle' in providing help IF WE KNOW WHERE WE NEED TO START LOOKING!

BTW, may I suggest that you also update your modeling templates as that NX 6.0 part file is based on one which is over 5 years old and was originally created using UG V18.0 and the part history indicates that nothing of significance was done to that part file for over 500 iterations, which indicates that all that you've been doing with it is opening it and resaving it. Please try starting with fresh templates with every new version of NX that you install.

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.

 

[cowski]

ds4378,
In the 'Variational_sweep_2.prt' you posted, if all you want is the line to follow the guides, you would be better served by deleting the sketch and using 'Through Curves' on the line and spline (your guides).

Using a single line as the section will not leverage the power of the variational sweep command; it is better to use it with a 2D section.

Using variational sweep allows you to constrain what you need, but must let something vary along the path. In the attached file (very similar to the help file example) I extruded a line and spline to create 2 sheet bodies to use the edges as rails. I next created a sketch at the 50% arclength along the spline, intersected the sheet bodies with the sketch plane, and added a 'dome' between the 2 lines. In the sketch I added a dimension constraint to the height of the dome, try deleting this dimension and adding a dimension to one of the side legs instead to see how it affects the variational sweep feature.

 

[ds4378]

Thanks a lot for your input. I think I know how to manoeuvre the Variational sweep now.
It seems that you can´t use a guide that varies along a vertical axis. The guide/-s must be in one plane. As soon as I tried to use a guide that vary along the z-axis I got an unexpected result, and I could not use 2 guides.
When I put the guide/-s in a horizontal plane everything worked as expected. The section followed the guide and there was no problem to use more than one guide.

Have I drawn the right conclusion?

 

[Toost]

No. Guides can be full 3D.
I think that you have missed a few important issues that makes you draw this conclusion.
1) When defining the section sketch, you also have to think carefully on how the section plane should orient as the sweep moves along, the orientation of this plane controls the orientation of the section , -during the sweep. ( drag the plane back and forth along the guide to see how it will orient the sweep.)
2) the constraints in the sketch is controlling how the section behaves related to the guides.
In the supplied part, there might be mistakes made that has produced unexpected sweeps.
As an example, in your part , feature(13)"Vertical 1 guide": The section sketch is orientated "Parallel to vector" which forces "all sections" to be parallel,nothing wrong as long as it is intended.
The reason the sweep is not following the guide is that there are no constraints that dictates that, the arc is constrained to be point on curve, -to the ABS datum csys, and they are static.(not constrained to the datums of the sketch.) Edit that Sketch, delete the arc then HIDE the abs datum csys such that no mistakes can be done. Recreate a similar arc, - snap it "coincident" to the point ("Vertex").
In the attached part, i have done the above and thereby updated that feature. ( i then deleted the previous sweeps) and finally created a copy of the spline guide that you had created.
= Spline (11) and later are mine. Note that both spline guides are full 3D. Note how the Sketch(13) is constrained. Try do re-attach the section sketch and drag the placement plane to see how it orients.
Regards,
Tomas

 

[ds4378]

Thank you Toost.
I have followed your recommendations and everything works in 3D. It is obvious when you pointed it out that the sketch must be constrained so it can "be dynamical".
Thanks again.