Simple section sweep issues

[opelgt21]

Platform: NX4

I am trying to create a simple sweep from a .18" circle to a .10" circle using a curve between the two center points as a guide. (i.e. I am making a converging duct)

Issue 1: The resulting shape is not linear

The little guide arrows point different directions, which means the shape is being twisted, but I am not sure why this matters but it does.

Would someone please explain the correct way to use the NX4 sweep command. I have gone through several tutorials on the net and am convinced that no one understands how this command works.

Any help would be appreciated.

-Paul

 

[SiW979]

You need to break the circle up into a couple of pieces and ensure that the arrows start at the same quadrant and point in the same direction. (see attached model) alternatively, if it is a round section, draw the cross section and revolve it. It's difficult to understand exactly what you are trying to do without some sort of illustration.

Best regards

Simon (NX4.0.4.2 MP9 - TCEng 9.1.3.6.c)

http://www.jcb.com

Life shouldn't be measured by the number of breaths you take, but by the number of times when it's taken away...

 

[cowski]

Issue 1: The resulting shape is not linear

Set the 'interpolation' option to linear, I think it defaults to cubic.

no one understands how this command works

I think this perception comes from the fact that it is a very powerful command with lots of options to choose from. The tutorials you saw probably all used different options from each other and none were precisely the options you needed for your application. There are multiple ways to get the desired effect within this one command. The classic example is sweeping a shape along a helical path; using 1 guide and the default options will result in the shape 'twisting' along the path. This can be fixed by using multiple guides or using the 'vector direction' alignment method.

Spend some time in the help files while you play with the options and post questions as needed. You will find that swept is a powerful and useful command to have in your bag of tricks.

 

[hudson888]

Yep when sweeping circles best to split them into two halves so that the start and end points are aligned. If on selection the arrows point in opposite vectors there is an arrow to reverse the section direction that will assist you. If you want a linear sweep set the interpolation type to linear, it may have been set to cubic by default.

Using cubic interpolation you may be able to achieve simple tangency with adjacent geometry which supplies a pretty good reason for having the two methods.

Best Regards

Hudson

www.jamb.com.au

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