How to apply symmetry in stent simulation

[tgbabu]

I am a relatively new user. I am trying to use ANSYS for analyzing the crimping and expansion of stents. I started with elementary shapes like a simple 'u' shaped hair-pin, and then a full sinusoidal wave shaped rod/pin. I was able to successfully 'squeeze' such shapes by applying suitable forces/pressures and view the deformations etc. Now, I have moved on to the next stage of a 'wavy ring like structure' shown in the attached files. A stent would comprise of assembling many such rings with some structs connecting them at various points.

The difficulty that I have run into is that, I am unable to simulate a uniform, radial compression/expansion in all directions (perpendicular to the cylindrical axis of course). I have been able to apply a fixed support at one radial location; the rest of the stent/ring squeezes towards this 'fixed' point. But, that is not realistic. In reality, I should be able to apply a pressure on the outer surface and the entire geometry should shrink radially inwards 'uniformly' in all 'theta' directions.

I have tried applying symmetry but not successfully. Can someone give me some pointers, or give me some clues?
I have attached a report file from ANSYS, as well as another one that tries to illustrate more clearly the problem that I am facing.

Thank You. -Babu

 

[tgbabu]

I have attached the report file mentioned in my earlier post / original question.

-Babu

 

[Dave442]

Hi tgbabu,

If your stent geometry is symettric about its mid-point you only need to model half the stent length. If the stent is also symmetric about its circumference, you only need to model one repeating circumferential cell (i.e. if the stent has eight repeating circumferential cells you need only model 1/8 or 45 degrees of its circumference). To constrain the stent you can then constrain the nodes located on both the longitudinal and circumferential symmetry planes from moving normal to the respective symmetry plane.

To simulate the crimping/expansion of the stent you also want to use a rigid cylindrical surface. If I remember correctly, applying a pressure load directly to the inner/outer surface of the stent does not provide realistic results. To model a rigid cylindrical surface you can just mesh a cylindrical surface with shell elements and give it linear elastic properties with an extremely high elastic modulus. To simulate the crimping/expansion of the stent you then need to set up contact between the outer/inner surface of the stent and the rigid surface. I believe I used the penalty method to good effect in the past. Once you have your contact surfaces and conditions set up properly you can model the crimping/expansion of the stent by applying an appropriate radial displacement to each node located on the rigid surface. When the rigid surface makes contact with the stent it will then force it to crimp/expand as required.

If the stent does not feature longitudinal or circumferential symmetry you need to model its entire geometry. To constrain the stent in this scenario you can constrain a small number of nodes located at its mid-point in both the longitudinal and local circumferential directions. The rest of the procedure is then the same.

Sorry, I wasn't able to check your report files as I no longer have access to ANSYS.

Good luck!
Dave