Sweep and keep sections normal to guide

[NXMold]

I have a simple sweep that I used to do in ProE all the time, but can't figure out how to accomplish it in NX.

I am making a cashew gate, I have created a centerline arc and a diameter arc at each end (sizes are adjusted to create a proper draft angle) normal to the centerline.

When I sweep these two sections, they remain in thier current orientation relative to the WCS, when I need them to remain normal to the guide curve. How can I do this?

See attached image for the 'collapsing' cone I get.

NX 6.0.2.8 MoldWizard

 

[Berserk]

Hello,

Problem could be the direction of section one and section two. It looks like they point in the opposite direction.

What I do is rotate one of the circles to match.

UGNX5.0.4.1 MP6 \ WinXP-SP3
Productive Design Services

http://www.productivedesign.com

 

[JohnRBaker]

You don't have to actually "rotate one of the circles to match", just select the 'Reverse Direction' option below the 'Select Curve' item in the dialog.

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.

 

[NXMold]

Ah, yes I didn't notice that. The problem not the direction, though, as much as it is the start point is in the wrong quadrant.

The fix is not obvious, because when you draw an arc/circle from center you do not get direct control of the start point. I am using 'radius' as the through point and referencing an expression.

I found that you have indirect control of the start point by inferring the second point and clicking in the general vacinity you want, then change back to the associative radius.

So, problem solved. Thanks.

NX 6.0.2.8 MoldWizard

 

[cowski]

Actually, I think you do have direct control of the start point, though it is less obvious than showing up as a prompt in a dialog box. The start point will lie in the direction of your horizontal reference. For non-sketch curves, the horizontal reference is the WCS X axis at the time the curve was created. So if you imagine the WCS at the center of your circle and its X axis parallel to your horizontal reference, the start point will lie on that X axis.