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extruding imported dxf curves

extruding imported dxf curves

extruding imported dxf curves

Dear all
i need help regarding extruding imported dxf file.The problem is when i try to extrude those curve(no of curves) directly the nx stop responding. is is there any proper way to extrude them? like converting those curve in something simple to actual ? i have attached the image below

RE: extruding imported dxf curves

Most probably, this happens a lot with imported dxf curves, there are a lot of tiny elements in there.
There are most probably even gaps.
You need to check the geometry first and solve these issues. For this you can use "Examine Geometry"
Have a look at the splines as well. If they are not "real" splines they might be build up out of tiny curves. This might cause an issue as well.
The spline issue you can repair by using "Join" from the "Derived Curve" features.

Ronald van den Broek
Senior Application Engineer
Winterthur Gas & Diesel Ltd
NX9 / TC10.1.2

Building new PLM environment from Scratch using NX12 / TC11

RE: extruding imported dxf curves

Like NutAce says, the DXF export probably created thousands of little curves. The sheer number of curves may be giving NX problems, especially if some are not planar or gaps/overlaps exist. The good news is that it is easy to clean up or recreate in NX. Focus on one horizontal element of the pattern; clean it up as you see fit (I'd suggest using the existing geometry as a guide to create 2 new splines). Extrude the resulting shape.

Create a circular array with this element (count = 3, angle = 360/6)

Use the linear array command to fill out the pattern (X count = number desired, X pitch = length of horizontal element, Y count = number desired, Y pitch = X pitch * cos(30)). Use the stagger option in the X direction.

Use datum planes or other means to trim the edges of the pattern as desired. Future edits to the pattern element will propagate to the entire pattern making updates easy.


RE: extruding imported dxf curves

A side note on the "NX stop responding".
If i guess it is as Ronald and Cowski says, "millions of tiny ( bad) curves", and, NX probably did not stop responding but rather is processing the input curves, which might take loo-oong time.
DXF is originally an Autocad file format but very frequently used for file transfer between many systems,
What system produced these curves that you have imported ? - Illustrator ?

Try see if that system can write a Step or Iges file, you might get better results .


RE: extruding imported dxf curves

Thank you all for your suggestion. :) 1) i have checked the curves which is spline an not curves through examine geometric .
@toost yes it was actually processing those curves but takes toooo long may be i need a better pc ? all though it get extrude after taking too long but i wanted to know is there any better way to do so it wont get lag an i got my things work well ?

RE: extruding imported dxf curves

I see this a lot. Try Simplify Curve? (Menu-Insert-Derived Curve-Simplify Curve). You can also reference or project into a sketch and the recreate using constrained geometry as you wish.

NX 1847
TC 11.5

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