Variational Sweep doesn't follow curve

[ilovedividends]

NX 9

I attached a quick example of how my variation sweep doesn't follow the curve. Any help is appreciated so I can try this function. Last time I used it I believe it worked but I cannot find my older file.

Also, can 'swept' do the same as the variation by just using multiple datum planes and defining your sketch as you go along a path?

nx 9

 

[NutAce]

What would be the intention of the Variational Sweep? In this particular example it would be easier to use the normal swept instead...
Or even a normal extrusion would do the trick already.

Ronald van den Broek
Senior Application Engineer
Winterthur Gas & Diesel Ltd
NX9 / TC10.1.2
HPZ420 Intel(R) Xeon(R) CPU E5-1620 0 @ 3.60GHz, 32 Gb Win7 64B
Nvidea Quadro4000 2048MB DDR5

HP Zbook15
Intel(R) Core(TM) i7-4800MQ
CPU @ 2.70 GHz Win7 64b
Nvidia K1100M 2048 MB DDR5

 

[ilovedividends]

I'm looking to finally toy with how var sweep differs from creating multiple datums and just using swept. I really don't understand why my simple var sweep isn't following the curve?

nx 9

 

[cowski]

Have you looked up the variational sweep in the help files? After you read up on it, I think you will have a better understanding of what it is and what it can do.

www.nxjournaling.com

 

[Xwheelguy]

For what you have defined in regards to the section geometry, Variational Sweep isn't the logical choice. I think you'd be wise to follow cowski's advice to learn the usage intent for Variational Sweep and the previous 2 responses in regards to what is shown in your NX part file. What you are attempting to do can essentially be done with Extrude. If you're insistent upon a Sweep type of feature, then use Swept for this.

I feel Variational Sweep is intended for instances where you want to define more than one section AND have the ability to add more along the guide while defining those sections via Sketches. Maybe think of it as a more controlled and defined Sweep.

Tim Flater
NX Designer
NX 9.0.3.4 Win7 Pro x64 SP1
Intel Xeon 2.53 GHz 6GB RAM
NVIDIA Quadro 4000 2GB

 

[ilovedividends]

I'm aware of what the var sweep does, I'm aware I could extrude or use swept or use other sweeps. I would like to ask kindly why the section profile isn't attached/following the curve.

nx 9

 

[t300master]

Hello

you`ve constrained the start point ot the line to the CSYS point. If you constrain it to the intersection point which ist created at the intersection between the path curve and the sketch plane of the var sweep it will work as expected.

best regards

Meinolf

 

[SiW979]

I've had this problem with V Sweep in the past, it can help if during creation of the sketch select the path on the body of the rail then drag it towards the end (0%) it's quite easy to get a bad result with a V sweep by just selecting the end point of a line/edge. See the attached video.

Cheers

Si



Best regards

Simon

NX7.5 NX8.5 NX9 NX10
NX Consultant
www.team-eng.com

 

[ilovedividends]

Thanks fellas, that was seriously driving me crazy, much appreciated. I almost threw my computer out the window and checked into a rubber room.

nx 9

 

[GrLoki]

Hi,
that was good joke and way how somebody bring to mad
But there is easy solution. Sketch was wrong constrained. By using Variational Sweeep is good all constrains keep only inside in sketch. In this case was line constrained to guide line but had to be to intersecting point, by this case to point of sketch basis.

Best regards