Large strain

[HTTPS]

Users, I need an advice!
I'm modeling a coronary stent with Ansys WB 9.0, this stent undergoes a radial strain and has plasticity, in this process, it has a contact with the arterial wall. I have built the solid model and I have apply all constraints. My problem is: why the stent undergo a rigid body motion in addition to the radial strain?
This problem doesn't appear if I impose a little radial strain (in this case, the stent has an enlargment and it contact with the arterial wall).
I can't constrain along z (the assial coordinate) my stent because Ansys can't rich a convergent solution... help me please!

Thanks

 

[Stringmaker]

Have you tried specifying "rough" contact along the entire surface? What about frictional contact between the nodes on the outer diameter on one end of the stent with the arterial wall? Be sure to set the coefficient of friction just high enough that rigid body motion in the z-direction is eliminated. This should be relatively easy to obtain convergence on. In most cases like this there is typically other ways to constrain things besides displacements. Sorry I'm an Ansys user and my experience with WB is limited or I'd probably have a more precise answer.

Good luck,
-Brian

 

[HTTPS]

Stringmaker,
thanks for your advice, I'll try to introduce a frictional contact, I think it could solve my problem, even if the stent shows the rigid motion during the expansion and not when it reach the arterial wall.

Thank you

 

[MArcOGtheBOY]

I think... you need to add some tie to your model.
I don't know your geometry but I think you can add a spring or a link, with low Young modulus, in z direction, or add a bond, in z direction, upon the areas that limit your volume, for stabilize your body.
I don't know why the solution doesn't not converge but, if you put your constraints well, you can not have mistakes.
You can add the frictional contact but, if the problem is during the enlargment, I think the contact can't change your result.

Good luck

 

[Stringmaker]

Marcogtheboy is right about needing some sort of weak springs during the swell process until contact with the arterial wall is established. I initially misunderstood that contact had not been established in the first load step. Have you tried turning weak springs on under the Solution -> Options -> Weak Springs to prevent rigid body motion?

 

[HTTPS]

Stringmaker, I work in batch, in which way could I insert the spring? I don't know the command.

Thanks

 

[Stringmaker]

What exactly are you doing in batch? Constructing the model? Solving? Weak springs would be specified before you solve via Solution in WB. I've never known anyone who ran WB in batch mode that's why I ask. The Ansys documentation did not list any sort of command for week springs so it must be an option solely for WB (which makes sense).

 

[HTTPS]

I work in batch from the analysi's start (import solid geometry, define materials, real constant, element type, mesh) to the end (solve).
I run WB in batch because for me is quite simple and I can modify parameters, if necessary, without restart from the beginning, I never work with the GUI.
For me, is impossible the documentation doesn't list any command for put a spring, probably I can run my model in GUI and after apply the spring and see, after, the command in the .log file.

 

[Stringmaker]

Yes the log file should show it. You may want to play around with the spring values or atleast ensure that they are small values and will not adversely affect results. I'm not exactly certain how stiff stents typically are. In the WB help do a search for "weak spring" and it will give you a good insight of the options you have for tailoring this value to your needs.

 

[HTTPS]

Thank you Stringmaker!

 

[cbrn]

Hi,
also consider that you can insert APDL commands just like you would do with Ansys "classical". So, in order to apply weak springs, you can also create a COMBIN14 element type with RC,,... and so on. This works for every APDL command, except those which relate to graphical interaction in POST1.

Regards

 

[HTTPS]

Hi cbrn, can I add this type of element if I have a 3D geometry?

 

[cbrn]

Hi,
sure you can! The spring/dampener 14 is a COMBINation element, it works with any other structural element type. But my suggestion wasn't to create the springs with APDL when you can use the Workbench option "Use weak Springs -> ON": it would be more difficult for nothing! It was only an example of how you can use APDL in order to "cheat" with operations that Workbench SEEMS not to be able to do (and, instead, he does...).

Regards