How do I wrap a helix around an existing tube?
I have inherited a system, of which one component is an arbitrarily shaped tube. I have no idea how this tube was created, and I don't want to modify this tube. However, I want to wrap a piece of spiral wrap around this tube as sacrificial protection. Because we use TeamCenter's DMU as the controlling document, I must create a reasonably representative model in CAD, which happens to be Catia V5 at our company.
In SolidWorks I would have created a helix, swept the rectangular sketch, then bent the final solid using the "Flex" operation. But what would be the method to use in Catia?
Thanks in advance
If I understand what you're trying to do, i would create the helix and sweep the rectangular profile using the helix curve as a guide. I have no idea what the Solidworks Flex command does or why you need to use it.
If the tube is straight and circular, then just make a regular Helix curve.
(I will post a second answer for a curved tube)
If the tube is an irregular shape (not a cylinder or cone), such as a bent centerline, or non-circular cross-section, here's a little helix trick I learned on GrabCAD many years ago (but I forgot the author to give proper credit to):
1 Extract the tube surface from your inherited model
2. draw a point on the surface where the helix will start
3. draw a Line starting at the point
a. line type = angle
b. length = 1000 (or any big number)
c. support = tube surface
d. angle = guess at what you think the helix angle is
e. when you OK, the "line" will actually be a curve on the surface.
4. edit the Line and adjust the length and angle to get the helix you want
Now that you have the helix, sweep the profile to represent the wrap.
Here's a video showing another way to draw a helix if you have the center line of the tube: https://grabcad.com/tutorials/tutorial-how-to-get-a-helix-on-a-spline-curve-polyline-in-catia-v5