Sweep along guide is twisting 2

[Trietsch]

Hello,

Anyone know how to keep a sweep along guide from twisting? I have extracted curves (from an imported model) as a guide string with some bridge curves replacing the small non-tangent curves. When I sweep a simple cross section, it twists as it goes along the guide string.

In the attached model, I really want the the sweep to remain parallel with the Z axis. The curves represent a groove for a press in place gasket in which a seal will reside.

Any thoughts?


NX6.0.5.3 globally
NX8.5.0.23 in testing for rollout

 

[cowski]

For the "orientation" option, use "vector direction" and use a vector parallel to your Z axis.

www.nxjournaling.com

 

[Trietsch]

Cowski, that is exaclty what I am after, however I don't see that option. Which sweep feature might I find that in?

 

[SDETERS]

Try using the swept command instead of sweep along guide.

 

[Trietsch]

SDETERS, Thank you, I was just playing iwth this and it does have an orientation option.. hwoever the geometry goes very wrong easily with this feature. did you have any luck with this?

 

[Trietsch]

sorry forgot the link

 

[Trietsch]

I should have read Cowski's repsonse more closely. The 'Vector Direction' is working well for now, (I was using forced direction) but Swept is a bit more picky with tangent curves apparantly.. I'll replace some more with bridges and this may be my solution.

Thanks!

 

[JohnRBaker]

Attached is an example using the method suggested by cowski and SDETERS, however, in order to make it work the profile must be at least tangent continuous and there was a problem in the corner where the red circle is at. I replaced that seires of arcs and bridge curves with a single bridge curve (if that's not OK you'll need to go back and clean-up that area yourself to get a fully tangent segment).

Anyway, take a look (note that I left your old 'Sweep' feature in the model just that it's suppressed, which you can unsuppress to see how it compares to the new 'Swept' feature).

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.

 

[Trietsch]

John,

Thank you for your response, I completely agree and it seems you and I did the same operation in this case. I wish we were able to obtain better parasolid geometry to extract the curves from, however that is proving to be impossible from our customer (that also uses NX so native would have been perfect). I'll work with this method and add the complex geometry cross section and the multiple loops to see how it turns out. Thanks everyone!

 

[SDETERS]

John How did you find the curves that was causing the issue being non tangent continous?

 

[Trietsch]

I found them by selecting the cuves as a single curve until NX gave an error. on occasion if you leave the selection filter to tengent curves NX will put an asterisk on the curve intersection that has a problem.

 

[Xwheelguy]

You can also measure the angles (from where the curves meet) and see if they measure 0° (or 180°).

Tim Flater
NX Designer
NX 8.0.3.4
Win7 Pro x64 SP1
Intel Xeon 2.53 GHz 6GB RAM
NVIDIA Quadro 4000 2GB

 

[JohnRBaker]

The problem is that that's basically what happens now when you don't use the default orientation method, the software tries to maintain the spatial relationship between the profile and the curves defining the path, which it actually does pretty well. The problem is that there is also a 'twist' factor when it comes to complex 3D splines and it's this 'twist' factor that is causing the original 'twisted' result.

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.