CENTERLINE FROM A TUBE BODY 3

[CAD2015]

Hi,

I was trying to create a centerline from a tube body.
I got the error message in the second picture.
My main task is to measure the centerline of this tube body.
I use NX 2212.
How could I fix this matter?

Thank you!

 

[cowski]

Is this an imported body (STEP or similar)? If so, try using "optimize face" on the geometry before using it for anything else.

 

[CAD2015]

Cowski,
Thanks for your prompt message.
I am trying to get back on NX track, after more than 10 years of "exile" in other CAD systems.
I did follow your directions, but it doesn't work.
Attached is a copy of all my tentative:

1. Optimize Face
2. Extract Virtual Curve
3. Extract Geometry

The optimize face doesn't work.
I used "Extract Geometry" and got a curve (Composite Curve), close to what I need, but it is not a centerline.

What else should be done?

Thanks,

 

[CAD2015]

What files are we allowed to attach to a thread?...................

 

[cowski]

Siemens Digital Industries Software Community

The thread above (Siemens community forum) has a method that was used before the addition of the extract center line command. Perhaps it will work for you.

 

[CAD2015]

I will try that.
Thanks again!

 

[CAD2015]

Hi,
The tube in the picture is a Sheet Body.
How could I get its centerline?
Or/and how could I convert it to a solid body?

Thank you,

 

[mmauldin]

Does the edge that runs lengthwise on the tube have a diametrically opposed counterpart? If it does, it might be worth a shot to create a ruled surface between them then create an isoparametric curve on that surface to determine the centerline.

 

[cowski]

The tube in the picture is a Sheet Body.

Or/and how could I convert it to a solid body?

If it is a single sheet body, use the "make solid" command to convert it to a solid.

If it is a collection of sheet bodies, use the "sew" command (use the solid body output option).

 

[CAD2015]

Thank you, Cowski.
I have done everything mentioned in this thread.
No way to make Extract Virtual Curve (centerline).
There is an issue with this body.
I tried to send a step file for you, but Eng-tips doesn't accept this extension......

 

[Jon]

I've just added stp and step as allowed extensions. Please try uploading again ...or you can upload as .zip

 

[CAD2015]

I've just added stp and step as allowed extensions. Please try uploading again ...or you can upload

Thanks to the Administrator approval, I am able to bring the file of the tube that can't be used for the "Extract Virtual Curves" command (centerline curve).
I can't wait to see how you can figure out this issue!..........
Thanks in advance!

 

[mmauldin]

Tried to open the file but found no geometry. 2.2KB is pretty small for a STEP file.

 

[mmauldin]

I downloaded a STEP file of a spring and used the ruled surface/isoparametric curve approach to recreate the centerline. I used the isoparametric curve to recreate the tube and it seems to work.

I tried to create a Tube Centerline using both faces of the tube but it failed. Tube Centerline does work if I select only one face of the tube.

 

[CAD2015]

Tried to open the file but found no geometry. 2.2KB is pretty small for a STEP file.

mmauldin (and anybody else):

Here's the file I was inquire about.
Can you get its centerline?

Regards,

 

[CAD2015]

 

[cowski]

mmauldin's advice about creating a ruled surface and isoparametric curves should work well in this instance.

Does the edge that runs lengthwise on the tube have a diametrically opposed counterpart? If it does, it might be worth a shot to create a ruled surface between them then create an isoparametric curve on that surface to determine the centerline.

 

[mmauldin]

I used the edges to create a ruled sheet body but isoparametric curves didn't work. Instead, I used Offset in Face to offset one edge of the ruled body half the face width, then created a tube that essentially matches your original. Part file also attached.

 

[mmauldin]

Actually, Isoparametric does work, I just forgot to set it for U and V.

 

[CAD2015]

mmauldin,​

Perfect!...........
Good lesson!



Thank you!