ABAQUS Dynamic Explicit: Stent Crimping

[suz_02]

Hello,

I am having trouble with crimping a stent using the Dynamic/Explicit Step ( 2 steps in the model: (1) initial and (2) Dynamic/Explicit). It is aborting or stops running completely, without crimping the stent at all.

I am trying to apply an inward, radial displacement (smooth step 0->1) to the centre of 12 rigid plates (reference point at the centre of the plates), that are ordered in a cylindrical manner.
I am using the general contact method with the following interaction properties: Tangential -> Penalty -> Friction Factor =0.1 and Normal -> Hard. I have also used tie contacts between the cylindrical coordinate centre (RP1) and at some point from the geometry (RP2), where RP2 has an encastre BC.

I have used semi-automatic mass-scaling and have applied mass-scaling to poor-mesh-elements using the minimum time increment specified for the free tetrahedral mesh (seed size 0.1 and element type 3D element).

I have set used the point mass/inertia for the rigid plates: mass of the rigid body to be 1 and the rotational inertia (no diagonal terms) to be 1 also. The reference point is at the centre of the rigid body.

I keep getting the following warnings:

(1) TYPE=BELOW MIN mass scaling will be ignored for mass elements.
(2) TYPE=BELOW MIN mass scaling will be ignored for Rotational elements.
(3) OP=NEW on *CONTACT is ignored when the general contact definition is specified as model data.
(4) The option *boundary type = displacement has been used; check status file between steps for warnings on any jumps prescribed across the steps in displacement values of translational dof. For rotational dof make sure that there are no such jumps. All jumps in displacements across steps are ignored

Any solutions to these warnings would be greatly appreciated!

 

[FEA way]

I keep getting the following errors:

Those are all warnings, not errors so they don't prevent the analysis from running. Aren't there any actual error messages when it fails ?

 

[suz_02]

sorry I meant to write warnings, I did not get any errors however, I ran this for 4 days and it was stuck at one time step and not continuing.

These warnings kept appearing every time I ran the simulation and I had thought that they were the cause for it not continuing.

 

[IceBreakerSours]

Have you run explicit analyses before? Do you know if your stent is sufficiently constrained? Not sure why you have multiple rigid plates; usually, these sims have a cylinder with BCs specified in a radial coordinate system.

Take a big step back and ensure: 1) BCs are applied as you expect in a test copy of this model. In that test copy, you could remove the stent altogether. If the crimping tool moves as per the BCs, great. 2) In another test copy, get rid of the crimping and apply a simple point load somewhere on the stent. Do you see stresses in that point load location or does the stent fly away? If the animation shows the stent flying away, your stent isn't constrained appropriately.

 

[suz_02]

Have you run explicit analyses before? Do you know if your stent is sufficiently constrained? Not sure why you have multiple rigid plates; usually, these sims have a cylinder with BCs specified in a radial coordinate system.

Take a big step back and ensure: 1) BCs are applied as you expect in a test copy of this model. In that test copy, you could remove the stent altogether. If the crimping tool moves as per the BCs, great. 2) In another test copy, get rid of the crimping and apply a simple point load somewhere on the stent. Do you see stresses in that point load location or does the stent fly away? If the animation shows the stent flying away, your stent isn't constrained appropriately.

This is my first time running explicit analysis. I have tried using a cylinder to crimp the stent in a previous model using surface-surface contacts however this is difficult to use for stents that have too many small surfaces. Also, when using analytical rigid parts, it will not radial displace unlike when you use a deformable part. In recent literature I have found that many have had better success in using rigid plates in this manner to crimp the stent, and so I am trying to replicate this.

I will do the tests that you have mentioned and get back to you on this. Just to clarify in all of the test models I should keep everything the same except for the changes you mentioned?

 

[suz_02]

Have you run explicit analyses before? Do you know if your stent is sufficiently constrained? Not sure why you have multiple rigid plates; usually, these sims have a cylinder with BCs specified in a radial coordinate system.

Take a big step back and ensure: 1) BCs are applied as you expect in a test copy of this model. In that test copy, you could remove the stent altogether. If the crimping tool moves as per the BCs, great. 2) In another test copy, get rid of the crimping and apply a simple point load somewhere on the stent. Do you see stresses in that point load location or does the stent fly away? If the animation shows the stent flying away, your stent isn't constrained appropriately.

I tried the first test you mentioned and that worked fine, but when i was trying to apply a force to a point on the stent it aborted and i got these messages. I am not sure why I am getting these errors.

 

[FEA way]

I tried the first test you mentioned and that worked fine, but when i was trying to apply a force to a point on the stent it aborted and i got these messages. I am not sure why I am getting these errors.

Those are still warnings. No errors again ? There should be some if the analysis was aborted.

 

[suz_02]

Those are still warnings. No errors again ? There should be some if the analysis was aborted.

I believe that there are issues with how i have defined my tie constraints, I did get this warning when running my simulation in regards to this:


I am not sure how I should constrain my stent so that it does not move during the process. I have just applied coupling constraints and it has gotten rid of this error in the data file and in the warnings. I have applied this to my main model, as I have made some adjustments.

However, I still cannot get rid of the warning regarding the displacement, is this something that can be ignored as i have applied a smooth step displacement BC. Also could you please advise me on how to refine my mesh since this warning continuously pops up:

5117 elements are distorted. Either the isoparametric angles are out of the suggested limits or the triangular or tetrahedral quality measure is bad. The elements have been identified in element set WarnElemDistorted.

I have just used free tet mesh on this with 3D elements and growth rate of 1. I am not sure how to resolve this

 

[IceBreakerSours]

Unrelated - It appears that you have imaged a stent and are using the scan (STL) as a starting point for your mesh - Is that correct? If yes, it would be much better to come up with a much more coarse mesh because the elements may be very small which kills the explicit time step. Also, what is the element count in your mesh and the smallest time step (should be reported in the msg/dat/.. file, going by recollection)?

Related -

1) The crimping tool can be very close to the deformable surface. Cylinder should work - it works for everyone.
2) A node on the stent can be fixed in the out-of-image (Z) direction at least until the crimping tool comes into contact with the stent and friction prevents it from slipping away. So, you may consider performing a two-step analysis with the stent fixed in the Z-direction in the first step while the crimping tool starts to come into contact with the stent and then, in the second step, releasing the Z-constraint on the node and continuing with the crimping.

 

[suz_02]

Unrelated - It appears that you have imaged a stent and are using the scan (STL) as a starting point for your mesh - Is that correct? If yes, it would be much better to come up with a much more coarse mesh because the elements may be very small which kills the explicit time step. Also, what is the element count in your mesh and the smallest time step (should be reported in the msg/dat/.. file, going by recollection)?

Related -

1) The crimping tool can be very close to the deformable surface. Cylinder should work - it works for everyone.
2) A node on the stent can be fixed in the out-of-image (Z) direction at least until the crimping tool comes into contact with the stent and friction prevents it from slipping away. So, you may consider performing a two-step analysis with the stent fixed in the Z-direction in the first step while the crimping tool starts to come into contact with the stent and then, in the second step, releasing the Z-constraint on the node and continuing with the crimping.

Unrelated- The STL I have decimated, converted mesh into geometry and then into a solid using FREECAD. Currently I have around 200,000 elements and I believe the minimum time step was around x10^-10

Related- For your point 2) would that mean I would have an initial step where I apply a ZSYM constraint that does not propagate into the second dynamic step. The crimping displacement would be applied to the initial step and propagate into the dynamic?

What I have done so far -I have gotten rid of the tie constraint warning by implementing kinematic coupling constraint between two reference points.

The main warnings I get now are the displacement jumps, OP=Contact and the error with my mesh quality. For the mesh quality I have tried making it coarse but I still get the same error, I’m not sure how much more coarse I should make it or if there is anything else I could do.

 

[IceBreakerSours]

1. 10^-10 is a very small time step. How long (real physical time) are you running the analysis?
2. Once you are past method development and have the analysis running, that time step will still take the job to run to completion. At this early stage when are developing a method, you'll end up waiting a lot which is not good. As an aside, this sort of analysis is solvable with implicit (Abaqus/Standard - Static or Dynamic - Static should work but might take some work). In fact, the analysis should not take more than a few hours on modern hardware.
3. I have seen meshes with 4-6 linear bricks through thickness during early stages. For convergence studies, they can go higher.

I strongly recommend asking your boss/manager/prof/.. for support. Otherwise, you may end up wasting a lot of time.

 

[suz_02]

1. 10^-10 is a very small time step. How long (real physical time) are you running the analysis?
2. Once you are past method development and have the analysis running, that time step will still take the job to run to completion. At this early stage when are developing a method, you'll end up waiting a lot which is not good. As an aside, this sort of analysis is solvable with implicit (Abaqus/Standard - Static or Dynamic - Static should work but might take some work). In fact, the analysis should not take more than a few hours on modern hardware.
3. I have seen meshes with 4-6 linear bricks through thickness during early stages. For convergence studies, they can go higher.

I strongly recommend asking your boss/manager/prof/.. for support. Otherwise, you may end up wasting a lot of time.

When I first ran the explicit model I waited 4 days and it was still running. But I had some warnings that I wanted to get rid of.


Do you suggest that I try doing the same setup but using the dynamic implicit step? I can give that a go if you think it is more feasible. Would the implicit step use less time increments when compared to using the explicit?

I remember using a global seed size of around 5-7 and it gave me 200,000 elements. Do you think it would be better then to increase it above ten so that I have fewer elements which should increase the stable time increment? I’m not sure if it’s because I have decimated the original STL file and that is why the mesh is still too refined.

 

[IceBreakerSours]

For a simulation of this level with explicit, I would want to start seeing data trickling into the output file within minutes and the job finished within a few hours.

Implicit is a different beast altogether - It will take fewer time steps but the time step size can be much larger compared with explicit. However, getting a job to run with implicit tends to take more careful thought than explicit. There is a LOT of material in these forums and elsewhere to guide you. Abaqus documentation is an excellent resource as well.

You are working with an advanced technology that you do not have a grasp of; I strongly recommend asking for help from your boss. Tough pill to swallow, I know.

 

[FEA way]

When I first ran the explicit model I waited 4 days and it was still running. But I had some warnings that I wanted to get rid of.


Do you suggest that I try doing the same setup but using the dynamic implicit step? I can give that a go if you think it is more feasible. Would the implicit step use less time increments when compared to using the explicit?

Quasi-static explicit analyses can indeed take a few days for more complex models. Stent analyses are often performed with Abaqus/Standard (static step with optional stabilization or dynamic implicit quasi-static step to help with instabilities) but crimping might be difficult to solve this way due to complex contact conditions. So Explicit seems to be a good choice for this stage.

 

[suz_02]

Quasi-static explicit analyses can indeed take a few days for more complex models. Stent analyses are often performed with Abaqus/Standard (static step with optional stabilization or dynamic implicit quasi-static step to help with instabilities) but crimping might be difficult to solve this way due to complex contact conditions. So Explicit seems to be a good choice for this stage.

I am currently working on fixing my mesh. I have used virtual topology to create a single face and then trying to create sections so that I can mesh. Since I will be using text elements, do you suggest any specific planes or angles of planes to ensure that the sections will create, nicely shaped set elements? This should help my model to simulate faster so that I may observe if any of the setup needs changing, since the only worrying warning I am getting is that the simulation will take 2M steps.

 

[FEA way]

I can't see the geometry of your model well but it looks like a wire stent with hexagonal cells. Did you consider modeling it with beam elements, at least initially to significantly reduce the size of the model ? The Wrap Mesh plug-in available for Abaqus/CAE will allow you to start with a 2D pattern and then wrap it to create a full cylinder. Tetrahedral elements should be avoided if possible.

 

[suz_02]

I can't see the geometry of your model well but it looks like a wire stent with hexagonal cells. Did you consider modeling it with beam elements, at least initially to significantly reduce the size of the model ? The Wrap Mesh plug-in available for Abaqus/CAE will allow you to start with a 2D pattern and then wrap it to create a full cylinder. Tetrahedral elements should be avoided if possible.

Is this plug-in used to create stent geometries? I remember reading about this. Does this allow you to create different types of wired stents, similar to how we sketch a part in Abaqus? In terms of beam elements do you mean the element assigning in the mesh module. For example I am currently using 3D stress test elements to mesh my model.

 

[FEA way]

Is this plug-in used to create stent geometries? I remember reading about this. Does this allow you to create different types of wired stents, similar to how we sketch a part in Abaqus? In terms of beam elements do you mean the element assigning in the mesh module. For example I am currently using 3D stress test elements to mesh my model.

The Wrap Mesh plug-in is mode general. It’s not meant specifically for stents but can be particularly helpful when modeling them. It just wraps a flat mesh into a cylindrical shape.

When it comes to beam elements, you would have to remodel the stent using wires (lines) first to be able to use them.

 

[suz_02]

The Wrap Mesh plug-in is mode general. It’s not meant specifically for stents but can be particularly helpful when modeling them. It just wraps a flat mesh into a cylindrical shape.

When it comes to beam elements, you would have to remodel the stent using wires (lines) first to be able to use them.

Do you have the plug-in file for the wrap mesh? I cannot seem to find it, or is this done with scripting that requires a separate plug-in. I would like to explore the use of this.

 

[FEA way]

You can download this plug-in from the Dassault Systemes Knowledge Base but you may need a customer account to access it. Alternatively, there's a simple scripting utility to wrap orphan meshes (those without associated geometry).