Sweep with changing cross section

[DLH81]

I'm having an issue creating a sweep.

The attached prt file should show the issue I'm having. When trying to accompish the sweep in 1 step, the section flattens out around the bend as shown by Swept (8). If doing in 2 steps (Swept (9) and Swept (10)), it comes out correct but wondering if there is a way to do it in only 1 step?

 

[PSI-CAD]

Hi

You must change the start of the first Section


Regards
Didier Psaltopoulos

http://www.psi-cad.com

 

[PSI-CAD]

Hi,

The best the way is:

1°) Edit the sketch then Reverse Direction of the sketch orientation
2°) Edit the swept then Reverse Direction of the first section


Regards
Didier Psaltopoulos

http://www.psi-cad.com

 

[cowski]

Similar, but slightly different solution (no need to reverse direction of sketch):
Reverse the direction of the first section in the swept command and use the alignment option 'By Points' to remove the twist.

http://files.engineering.com/getfil...0b63a4&file=Circle_Sweep_Example_byPoints.prt

www.nxjournaling.com

 

[PSI-CAD]

Hi cowski,

I have tried the same solution first, but alignment by points was not easy to explain


Regards
Didier Psaltopoulos

http://www.psi-cad.com

 

[JohnRBaker]

The easiest and most direct approach, for a situation like this, is to just add additional cross sections, as I've done in the attached model.

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

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

 

[JohnRBaker]

I should have seen that in the beginning. There is NO need for the extra cross sections and there is NO need to use 'align by points' either, as long as you get the circles oriented in a consistent manner, which can be done by simply editing 'Sketch_002' and selecting...

Tools -> Reattach...

...and when the dialog comes up go to section of the dialog labeled 'Sketch Orientation' and simply hit the 'Reverse Direction' icon. After you 'Finish' the sketch, you may still need to reverse the direction of the cross section when you edit the sweep but it should work OK, as seen in the attached model.

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

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

 

[DLH81]

Thanks all for the replies.

John - Thanks, that worked beautifully!

 

[JohnRBaker]

Actually DidierPSICAD hit onto it sooner than I did, I just provided mode details on exactly how to accomplish what he suggested.

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

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

 

[vrishraj]

Hi Cowski,
How you manage to align points on circles, facing so much problem to drag those points. some time it snap to the adjacent point then it is difficult to drag after that. Is there an easier technique? thanks.

Raj
NX 8.5

 

[SvenBom]

If you want to work with Swept command, then my advise to you is to use Arcs instead of Circles.
Arc has start and end point, where circle doesn't have any. So, when aligning arcs, there will be no problem for NX, because NX will align those start points with no problem.
Well, if you use circles and Align by Points, it can work. But it is quite hard to define the correct alignment points.

So, if you check my examples, you will see one with Swept command. There are 3 new sketches; all circles are defined with 2 arcs. There was no problem in creating such swept body.

And if you want to complicate a little bit, you can write down the equation for the change of the radii along the curve. Then, when you have defined such equation, you can use Insert->MeshSurface->Sections->SectionCircle command.
If you check my other part, you will see the use of this command. In Tools->Expressions, you can see my equations:
length...this is associative measurement of your guide curve
t........this is just a parameter for NX equations (law curves, etc.). It will go from 0 to 1
x........additional variable for my ft function
ft.......the lenght of the curve, where you have a change of radii from 1.25in to 0.75in is 6in. So, if x is equal or less then 6in, then the radius is changing according to this equation:1.25-0.5/6*length*t. And, if radius is greater than 6in, the radius will be 0.75in
Then, when selecting SectionCircle command, you have to select your guide curve first. The spine curve is the same one. In section Control, select ByEquation and use the t and ft parameters.
That way, you will get nice transition from one circle to another with creating only the guide curve and no section curve.

Hope, that those two examples will help.

 

[PSI-CAD]

Hi John

Thanks for those clarifications


Regards
Didier Psaltopoulos

http://www.psi-cad.com