Spline To Curve

[rc0213]

I have a situation where I imported a DXF into UG NX 9.0. And, there are splines which I need to convert to basic circles. The method I use is create 3 points on the spline. Then, I create the circle through the 3 points. Is there a quick way to convert these splines?

 

[cowski]

You can use the "simplify curve" command, but it may break the spline into hundreds of small segments...

www.nxjournaling.com

 

[rc0213]

The issue with "Simplify Curve", for me, is that the center of the arc is hard to locate. You can have a dozen arcs, and each arc has a center that is slightly different than the others. Thanks for that suggestion. Worst case, I can use "Simplify Curve just to create the curve and then, try to find the center.

 

[JohnRBaker]

If you increase (make larger) the Distance Tolerance (Modeling Preferences) you can control, to a certain extent, the number of arcs needed to replace the original spline. In the end, even using a very LARGE tolerance (like from 1.0 to 10.0 mm) will give you results as good or better than what you're going to get doing a simple 'eye-ball' placement of three points at a time for each arc segment created.

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

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

 

[Toost]

There is a Fit Curve Feature, which can fit circles to points. ( These points can be "on curve snaps" .)

But, have you tried to set the import option import polylines as : Splines OR arcs / lines in the dxf import ?

Regards, Tomas

 

[rc0213]

Thanks for the suggestions. Changing the option to arcs/lines while importing the DXF helped a lot. And, I tried the Model tolerance to simplify, it helped some.