# REVISITED: How to model this stent?

#### CatiaMod

##### New member
I was modeling a Stent and was successful in completing the first part of the design. A stent is a cylindrical structure and right now I have a rectangular structure/area. I wanted to know if it was possible to convert it into a cylinder. (something like the toroidal bend in solidworks) Is it possible to do that in Catia?

This is the point till which I have completed :

View attachment 1464

This is what the final model should look like :

View attachment 1465

PLEASE DO HELP! IT IS A PART OF MY PROJECT!
ANY SORT OF HELP WOULD BE APPRECIATED!

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#### MrCATIA

##### Super Moderator
I try to avoid doing school projects for students, but this modeling problem has bugged me for several months. I think I found an easy way to model this stent, using the PART DESIGN and GENERATIVE SHAPE DESIGN workbenches along with the DEVELOPED SHAPES license.

I will list the steps of my method in a series of posts within this thread.

Before we start, we need to do a few calculations based on CatiaMod's attached picture of what the final model should look like:

** number of similar sections in the stent: 10

** number of U-shaped segments in a section: 21

** number of centerlines in a section: 2 X 21 = 42

** OD of stent: unknown, so I'll use Ø25 mm

** line spacing (pitch): 25 X PI / 42 = 1.870 mm

** width of each U-shape leg: 1.870 x .80 = 1.496

** length of each section: unknown, so I'll use 15 mm

(continued in next post)

#### MrCATIA

##### Super Moderator
POST II

1. Start with a new part file, and switch to the Generative Shape Design Workbench

2. add a Sketch of an arc with a diameter of Ø25mm

3. Extrude the arc, making a surface that is longer than one section (20mm)

4. add a Plane outside of the extruded surface

5. Project the corner of the extruded surface onto the plane

(continued in next post)

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#### MrCATIA

##### Super Moderator
POST III

6. draw a Sketch of the centerline profile of the U-shaped segments using the parameters we calculated earlier. (I've sketched two S-shapes, although one is all we need)

7. switch to the Part Design workbench

8. insert a new Body

9. add a Pad from the S-shaped sketch using the THICK option. Length doesn't matter, but use the calculated width for the Neutral Fiber Thickness

10. switch back to the Generative Shape Design workbench

11. Extract (no propagation) the flat face of the S-shaped pad

13. Extract an edge (point propagation) to get the the entire s-shaped profile curve

14. Hide the extracted face, but show the extracted profile curve

(creating the profile like this allows us to go back and make adjustments to the sketch and/or pad that will update the profile)

(continued in next post)

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#### MrCATIA

##### Super Moderator
POST IV

15. Make sure the DEVELOPED SHAPES (DL1) license is active

16. Find the DEVELOPED SHAPES toolbar (in the Generative Shape Design workbench)

17. Use the UNFOLD tool (left icon) to flatten the extruded surface (step #3). Make sure the the S-shaped profile is totally inside the unfolded surface.

18. Double-click on the unfolded surface to edit it. Click the MORE> button and set the Surface Type to ALL.
(click NO if a message pops up about a ruled surface)

19. Project the the extracted curve onto the unfolded surface. Hide the extracted curve

20. Use the TRANSFER tool (middle icon in the Developed Shapes toolbar) to transform the flat profile onto the surface:

SURFACE TO UNFOLD: extruded surface
UNFOLDED SURFACE: unfolded surface
TRANSFER ELEMENTS: projected curve
TRANSFORMATION: FOLD

21. Hide the projected curve, unfolded surface, and projected point

22. add a FILL surface inside the folded curve, using the extruded surface for support

23. Hide everything except the Fill surface and the Axis

(continued in next post)

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#### MrCATIA

##### Super Moderator
POST V

24. switch to the Part Design workbench. And make the Part Body the current work object (underlined)

25. use THICK SURFACE to add 3mm thickness to the fill surface. Make sure the direction arrow is pointing in, and not out

26. Ooops - I made a mistake! my double-S shape cannot be used to make 21 segments. Sorry!

Edit the sketch that was used to make the first pad. Change the bottom lines and circles to construction, so the sketch only has one 'S' in the profile.

The updated surfaces and solid should look like this after the edit:

26. Hide the Geometric Set. Verify the ThickSurface is the current work object (underlined)

27. add a Circular Pattern of 21 instances about the center axis

28. add a Rectangular Pattern of 10 instances, spaced 18mm apart

That should complete the stent model! Some of the values could be parametrized to make it easy to modify.

I imagine the flat solid (included in the original post) could have been used in a similar fashion.

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