Stent Crimping 1

[jayfea13]

Hi,

I'm trying to crimp a stent (tubular medical device) on Workbench 14.0, external diameter of the stent being 2mm and thickness being 0.081mm.

I have assembled the stent and a thin-surface (diameter 3mm) around it on SolidWorks. Using 'Transient Structural', I have applied a 'Cylindrical Support' to the surface after defining a 'Cylindrical Coordinate System'. I have placed a displacement radially (inwards), which I did by selecting the inner surface of the surface-body and placing a 'Displacement' (as i said radially) of '-1mm'; so as to reach a target external diameter of 1mm of the stent (so 3mm surface moves 1mm inwards in all directions).

I am having troubles reaching a solution (loads of errors!); presumably because I haven't defined my contacts properly (I select the 'inner surface' of the surface body to be contacted with the outer surface of the stent, FRICTIONLESS)

A fellow engineer says I could get around this by simulating a thin-surface (using surface elements to mesh); since currently I have to add a small thickness of 0.001mm to my surface-body. I do not know how to create a ylindrical surface AND then mesh it appropriately. Any suggestions?

Thanks in advance!

 

[cvan42]

Hi Jay,
Our group has been working on this type of problem for the last year or so. We are compressing down to crimp dia, then expanding to design diameter. There is a lot that goes into this study. We use all solids and found surface cylinders with the most hyperelastic properties would fail in strain after about 200-300% Of course if you're just doing compression from 3mm to 2mm you might get away with it, but expanding from 2mm to 10mm won't work.

Another issue w/ surfaces is you're forced to use asymmetric contact pairs, and if you wanted to flip contact pairs you can't. We use solids, none are rigid bodies, in order take advantage of symmetric contact.

Once you leave surfaces you need a multitude of solid bodies with prescribed displacements to each one, so if you want to change a radius you have to manually update all the XY displacements of the bodies. Not fun.

Then if your group is interested in residual strains and both compression and expansion behavior you need to take advantage of the contact kill/alive scripting and insert a resting timestep between each move. Then there is the stent self contact pair whcih needs to be added, plus accurate NL material model of the stent.

The typical contact settings we use for bodies to stent are:

Body/Surf or Body/Body (Try Surf/Surf first run, but if "losing contact" chattering problems switch)

Frictionless
Pure Penalty
Nodal normal to target
0.1 FKN
Offset, ramped effects
Each iteration, agressive
Pinball Radius (critical) 0.02" (this value is the body sizing of the non stent bodies)

Stent to Stent:
Surf/Surf and/or Line/Body
La Grange
1.0 FKN
Offset, ramped effects
Each iteration, agressive
Pinball Radius (critical) 0.003" (this value is the body sizing of the stent)
Warning: always check contact w/ status tool, if the pinball is to large there will be initial interference/sticking which never goes away during the study and usually causes it to crash.

You can add friction but it slows down the study
If Surf/Surf gives trouble then switch to Body/Body
If Hex meshed parts and having covergence issues, switch to Tet. Hex/Hex contact can be more difficult than Tet/Tet

 

[jayfea13]

I was defining the wrong material models all this while! Haha thanks for that man.

Okay, even more problems (I'm an FEA newbie, forgive me!)

HAve a look at this pdf I am attaching. THanks!

 

[cvan42]

Jay,
Looks good man, it looks like you are applying radial displacements to the inner and outer surfaces. This might be ok if the struts are the same width/thickness. For reference, our design has two different widths of struts around the circumference, so they are going to move differently tangentially as they are compressed and expanded. Just be aware that by forcing radial displacements on the nodes of ID/OD, you might be introducing strains where the geometry would otherwise naturally move tangentailly/circumferentially to avoid those strains.

I'd like to add some of our screenshots, but it is fairly proprietary (stent geometry is really competitive and highly covered already in patents)- but, I can explain our approach that allows the stent to wiggle/shift as is pleases circumferentially. We do use 3 cells across and full 360 model.

1. Within the stent ID we have 12 tubes all on top of each other. In solidworks you extrude one tube and make 11 copies without displacement/rotations.

2. Just outside of the stent OD we have 12 plates. Make them fairly thin relative to the width, and make sure they are wide enough to be effective at the various diameters.

3. Create a contact pair for each tube and plate, insert a cid and tid script to define the contact/target pairs. Yes, there will be 24 contact pairs so far. We've had trouble grouping all the plates or tubes into single contact pairs.

4. In excel, create the moves of each plate and tube with trig. Under static structural, create a displacement and type in the X and Y coordinates of each move.

5. We use the kill/alive scripting at each timestep to compress and expand the stent. It takes awhile to coordinate all the moves, as sometimes the plates move while the contact is killed to get ready for the next timestep.

The moves are as follows:

TS1: Plates compress the stent to the crimp diameter, here the tube OD is just under the stent ID.

TS2: Plate contact pairs are killed so the stent can spring outward to relieve residual stresses.

TS3: Tubes start expanding outward to the expanded diameter while the plates are also moved while the contact is still killed.

TS4: The tubes are killed along with the plates to once again allow the relieveing of residual stresses after being fully expanded.

TS5+: The plates are again activated and move a bit inward to check fatigue issues.

It takes a whole bunch of setup time, but this is the only way we could get the stent to move in the range we're designing for.

 

[jayfea13]

thanks for that cvan!

i do believe that while your crimping/expansion analysis does infact represent the actual process quite realistically (crimpers do actually used multiple surfaces/plates!), the analysis i've performed suffices for the relatively simple model that i am looking at.

i would like to now perform a longitudinal deformation test on ansys (static this time too), and i would like to, in the same analysis, apply a 'fixed support' AFTER the third time-step; i.e. after the expansion process. so, i would like to select the same edges as i showed earlier, and apply a fixed support to those, but after the third step. Is this possible on ANSYS?

If not, how can i retrieve these results (deformed geometry with stresses) and insert them into another static analysis??

Any help with this would be highly appreciated!!

Thanks

 

[cvan42]

Jay,
If I read it correctly it sounds like you are compressing to crimp diameter, expanding to design diameter, then pulling axially a certain amount. If you cannot constrain one side of the stent to always be restricted axially, there is another way without having to write scripts. Need to solve it twice though.

1. Run through with a deformation result tied to the lines/surfaces. At the end of the timestep before you want to freeze it, write down the displacement.

2. Insert a displacement or relative displacment scoped to this line/surface. have all DOF of no interest free, and the others create a table.

3. In this table have all the displacments at 0. At the timestep (last one) in which you want to start freezing, type in the displacement value you got from above. On all the other timesteps go to the farthest left column, right click, and select "Activate/Deactivate at this step!". All the zeros should be greyed out, your displacement still white

4. Rerun the study, and you should see the stent move axially as it pleases until the timestep you want to freeze it. Then it should deform axially as you pull on it.

Everytime you change any parameter in the study, you need to rerun to get the displacement of step 1. Otherwise the geometry will drift back to the original number when you don't want it to move.

You can map results of a surface and have them applied to the same surface in another study, but this is usually done for thermal/mechanical or CFD/mechanical coupling. To export the deformed geometry is a huge ordeal. You need to have a setting in DM to export the results as an .STL (or point cloud), then you have to import to SolidWorks and start recreating the geometry with splines ans surfaces as .STL does not convert to any solid model format.

 

[flash3780]

I think you may want to have another look at your boundary conditions. Imposing a displacement is almost certainly over-constraining your stent. I think that the contact behavior between the crimping/expanding tools are important to your problem. I'd recommend modeling the tools as (second order) shell elements and apply radial displacements to them to simulate contracting or expanding. You'll want to set up surface-to-surface contact between your tools and your stent to properly capture the behavior of your stent.

Off the bat, there are a few basic modeling suggestions to consider:
1. You should be able to utilize symmetry in this analysis: take advantage of that.
2. Your mesh is not sufficient to accurately report the stresses in your part. This will affect the accuracy of your results, esp. since you have an elastic/plastic model.

Here is an example of a stent analysis from the folks at Simula/ABAQUS. Note that they are expanding a cylinder to expand the stent; ANSYS can perform the same operation.

It's worth noting that you should be able to produce pictures of a full stent even if you only model a portion and take advantage of symmetry in your problem. Symmetry will allow your model to solve/debug your model more quickly with a finer mesh.

Finally, keep in mind that there are some more advanced modeling techniques which may be more difficult in ANSYS/Workbench. There are some complexities to this problem... If you run into trouble in Workbench, you may consider flipping over to ANSYS/APDL once you've completed your geometry creation, manipulation and meshing.

 

[yomi213]

Hi Jay,
I am working on stent analysis. The stress values are not between tensile strength ad yield strength values.
I am trying to apply a pressure of 1 - 20 atm pressure to deploy the stent and the stress values are very high.
I don't understand the problem. Any suggestions??
I am using Ansys Workbench.
Thanks in advance.

 

[jayfea13]

Thank you cvan and flash; I will work with these methods and get back to you over time.

Yomi; are you sure you are defining a non-linear material model for the case? This was what I was doing wrongly for some time initially; I used a bi-linear stress-strain curve eventually; (Bi-linear Isotropic definition on ANSYS Workbench 14.0). What material are you using; I can probably provide you with the material properties for your stent material.

Try this and let me know!

 

[yomi213]

I have to test the stents using Magnesium alloys.
I have all the information about materials.
The stresses are high and the stent moves in Y direction.
I am not understanding how to constraint the stent and get the expansion and crimping effect.
And also I am applying pressure (0.1 - 2.03 MPa).
I have lot of questions.
Which direction did you apply the force?
How to apply pressure in 360 degrees form for a balloon expandable stent?

Thank you in advance.

 

[yomi213]

I have to perform expansion analysis on a crimped 180 degrees symmetry stent structure.
I have to test the stent using Satinles steel316 L, Co-Cr and magnesium alloys.
Boundary conditions:
Fixed supports: fix the ends
Pressure: 1- 2.03
I have applied displacements x- free, y=0, z= free. Still the values are high.
Analyse the stress, strain and total deformation.
The stress values are high.
I am using non-linear materials.
Could you please help me to get stress values below yield strength?
Are there any boundary conditions that has to be applied?
Does the tangent modulus value change with the type of alloy/ material?

 

[jayfea13]

TM will definitely change for different materials.

You can calculate the Tangent Modulus of the material using:

TM = ('Ultimate Tensile Strength'-'Yield Strength')/('Elongation at UTS'-'Elongation at YS').

Elongation at YS = (Yield Stress)/(Young's Modulus).

For Elongation at UTS; you'll need to have some papers which indicate the empirical/experimental values for this (I don't know any other method!).

Hope this helps.

Also, I had a quick look at your pictures; looks like you're working on a half-stent (not too clear)? If you're constraining the stent by allowing only planar motion of the half-stent, you may still be under constraining the model (it'll still move around on the plane!). Re-consider the BC's.

 

[yomi213]

Hi Jay,
Thank you for the information.
The following paper mentions the material properties.
Are you talking about the % elongation (i.e., Elongation at UTS)in Table 1 of the paper?
Please suggest me.

Thanks

 

[yomi213]

Here is the paper

 

[yomi213]

Hi Jay,

The stresses are much better after applying the boundary conditions.
But still they are not between yield strength and tensile strength.
The design is not solved whenever I apply contacts.
And if contacts are deleted it solves (stress, strain and total deformation) but the stresses are high.
Could you please tell me the material that you have worked with?

 

[yomi213]

The solver takes almost an hour to solve each time.
Could you please suggest me to get the solution in short time.