Somebody now how i can draw an axis along a hose , wich is step file

[manuel_alexandru]

here is how it's look the hose .I was thinking about to make a formula to a line wich will follow the contur of the hose , but i'm not shore how to do that ,if somebody can help me ,i will remain indebted

 

[MrCATIA]

Here's one way to get the centerline (axis) if the hose is split down the middle like in your picture:

1. change to the Generative Shape Design workbench
2. Extract both curves on the split edges of the hose (use Tangent propagation)
3. add a Line between the end points
4. add a Point in the middle of the line
5. draw a Sweep surface along the extracted curves (Profile Type: LINE, Subtype: 2 LIMITS, guides = extract curves, & verify Lengths = 0)
6. add an Isoparametric curve on the sweep surface at the middle point. This is the centerline of the hose.

 

[MrCATIA]

Here's a similar method to get the centerline, if the hose is 3D:

1. change to Generative Shape Design workbench
2. Extract outside surface of hose
3. Hide the Part Body, so only the surface is shown
4. working on one end, add a Point in the center of the hose
5. add a Point on the edge of the hose (Nearest Extremity, or anywhere on the edge)
6. add a Line between the last two points
7. add an Isoparametric curve on the extracted surface at the point on the edge
8. make a Sweep surface:
-- profile type: EXPLICIT
-- subtype: WITH REFERENCE SURFACE
-- profile: pt-pt line
-- guide curve: isoparametric curve
-- surface: extract surface
-- angle: 0° (if orange arrow is not pointing toward center, click NEXT)
9. add a Boundary curve at the inside edge of the sweep surface (this is the centerline of the hose)