Modeling suggestions for my problem, please

[cal34]

Hello. I am rather new to ABAQUS FEM and would be very grateful for some input on my model and study design.

My overall goal is to model how the tip of a needle interacts in human tissue. Specifically, I am interested in looking at the stress, strain and strain rate for small needle displacements inside of tissue. To model this interaction, I have created a 3D bevel-tipped needle and a block of tissue with the needle profile removed from the tissue, in Autodesk Inventor. I then import the CAD files into ABAQUS.

In my study, I have the needle inserted into the tissue and in contact with the tissue at the start of the simulation. I then want to add a displacement boundary condition in the 2nd step (after initial step) to displace the back of the needle 0.5 mm into tissue to observe the stress, strain, and strain rate.

However, I am having several issues:
1. Mesh. As you can see in the images below, the needle has fillets around the beveled edges so that it does not "cut" the tissue. Creating a mesh for the needle (and for the negative profile of the needle in tissue), seems to be very difficult. I have tried partitioning the needle, but with no luck. Thus, I have reverted to automatic meshing with a bottom-up scheme and tet elements. I've read that this can be inaccurate for results, is this true? Needle image:

2. Contact. I can specify contact between the flat beveled face and the cylindrical shaft of the needle with their corresponding faces in the tissue block. However, I am having trouble specifying contact between the fillet of the needle edge and the fillets produced in the tissue edges. Since there is friction between the needle and tissue, I feel like I need to establish this contact. When I try to specify contact, I get some sort of error that the bevel face and the fillets overlap, and something about a "tie"? (Sorry, can't remember off the top of my head). Here is the initial state of contact between the needle and tissue:

3. Insertion. When I displace the needle 0.5 mm into the tissue, I am finding that the needle actually moves straight through the tissue elements, as shown below! I am wondering why this is happening, is the tissue too soft (E: 7kPa) relative to the needle (E: 50 GPa)? I can't understand why the needle should go straight through the tissue elements.

Middle cut view of the needle in the tissue at the start of simulation:

Middle cut view of the needle in the tissue at the end of simulation with a 0.5mm displacement. Notice how the needle tip actually penetrates the tissue elements:

Thank you very much for your time!

 

[IceBreakerSours]

1.

I have reverted to automatic meshing with a bottom-up scheme and tet elements. I've read that this can be inaccurate for results, is this true?

First order tet elements are not recommended for modeling contact. Have ABAQUS/CAE generate modified quadratic elements (C3D10M). On the other hand, use the Virtual Topology tool to ignore those bevels, partition the geometry, and mesh it with linear bricks.

2. I did not quite get the problem.

3. Contact interaction is not working. Have you ran a Hertzian contact problem from the manuals? If not, you must play with simple geometries first.

By the way, what kind of soft tissue are you trying to model? What is the Poisson's ratio of the soft tissue?

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[MechIrl]

Like has been said, the Tet mesh isn't ideal. If you post your needle geometry you might get some better ideas for meshing.

 

[burningDiesel]

He might just as well use linear tets, as all other errors and unknowns will be far greater than the 30% stress difference you might get from using linear tets. Other than that, I of course completely agree.

Since u are only displacing the needle, can't you just leave out the needle mesh, and put boundary conditions (or loads) at the 'hole' in the tissue?

 

[cal34]

Thanks everyone for your helpful insights.

So, since it seems that meshing the fillets is tricky, I decided to start with an easier problem. I'm just trying to insert a standard bevel-tipped needle into tissue. The dimensions of the bevel are 0.711mm diameter cylinder, 4.03mm long on the bottom edge, with a 10 degree bevel. The geometry is pictured below (again, no more rounded edges from fillets):

Now, without the rounded edges, I do believe I will run into a singularity at the needle tip (due to the very sharp point). However, even when I try to mesh this geometry, ABAQUS will only allow tets to be used. I've tried partitioning the geometry, but I am not sure how to do it properly.

Could someone give me an idea of how to mesh this geometry? It also seems there is some discussion about the accuracy of using tets for the mesh. Could someone give a quick explanation as to why this is the case? And why Tets are not ideal for contact? With my geometry, it almost seems I am limited to using tets, especially when I plan to round the edges of the needle.

Since u are only displacing the needle, can't you just leave out the needle mesh, and put boundary conditions (or loads) at the 'hole' in the tissue?

My goal is to model different needle materials (with varying Young's moduli and Poisson's ratio), and the effects on the tissue. Thus I think I need to have a needle model. Correct?

By the way, what kind of soft tissue are you trying to model? What is the Poisson's ratio of the soft tissue?

I am modeling brain. E = 7kPa, v = 0.475.

Thanks all for your help.

 

[burningDiesel]

Well, unless you are going to use plastics or other soft material, the metal is about 10000 times as stiff as the brain tissue, u clear cut case where using rigid bodies to represent your metal is perfectly justifiable. Even the softest possible metal will still be at least 1000x as stiff.

If you want to continue with the meshed geometry, mesh with tets but select the C3D10M element as IceBreakerSour suggests.
Are you doing the simulation in Standard? What contact are you using?
Try using the general contact (this will be the easiest) and let ABQ chose contact surfaces and edges.
If that fails, select the contact faces and EDGES yourself, and do an edge to edge contact to avoid the penetration.

 

[IceBreakerSours]

I agree with sdebock. Unless you are interested in computing strains/stresses in the needle (which would be odd, to say the least), there is no need to mesh it.

In any case, no matter what you do, make sure the needle is the master surface. Also, have the soft tissue mesh to be *much* finer (than the needle mesh). Do not forget to verify the mesh quality is high. By the way, C3D10M elements converge slowly and one needs a fine mesh to get accurate results. You may also need to create a thin layer of membrane elements on the soft tissue and assign comparable stiffness to them, if you really need accurate contact stresses.

By the way, are you trying to model how the "cut" in the tissue progresses as the needle is pushed deeper? Technically speaking, are you trying to model crack propagation?

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[cal34]

Well, unless you are going to use plastics or other soft material

That's the goal of the project, to model different needle geometries as well as materials (including plastics) to view the effects of strain, strain rate and stress on tissue.

Are you doing the simulation in Standard? What contact are you using?

I am trying to model in Standard, yes. The inputs to the simulation are a 0.1 mm "push" on the back of the needle into the tissue. I am working with the General contact method now. However, if I want to model different velocities of needle insertion over this 0.1 mm distance, I will need to use a dynamic solver, correct?

The goal is to also measure the tissue stresses/strains during small needle rotations, but I haven't gotten to that point yet.

Unless you are interested in computing strains/stresses in the needle (which would be odd, to say the least), there is no need to mesh it.

Well, I actually am interested in the downward displacement of the needle tip as it is pushed forward. With softer needle materials, the tissue causes more displacement. The needles are essentially flexible.

are you trying to model crack propagation?

No, not for this simulation. Maybe down the line. Right now I just want to model a small "push" of the needle into the tissue.

 

[IceBreakerSours]

downward displacement of the needle tip

Even if you want the displacement of the tip, it still is not an argument for meshing it. Why? Think about it.

However, if you are interested in testing softer needles, then yes, meshing makes sense. But, in that case, why do you need to mesh the entire solid? Why not just create a surface mesh? Heck, why not create a 2D problem, for that matter! (I am sure you have your reasons.)

if I want to model different velocities of needle insertion over this 0.1 mm distance, I will need to use a dynamic solver, correct?

Yes, you should use the implicit dynamic solver.

However, to me, it is the soft tissue material model that is critical in this application. And soft tissues, in particular, are NOT isotropic linear elastic materials. They are anisotropic hyperelastic and, at least, linear viscoelastic, if you are not worried about damage inducing deformation. I *guess* fluid inside the brain soft tissue does not resist much load, so you may not have to worry about poroelastic effects, but I do not know.

Anyway, do NOT take this road until you (and your boss!) are sure about the goals (and underlying assumptions) of the project.

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[corus]

Relatively the needle is much stiffer than the tissue, hence you could use a discrete rigid region for the needle and only mesh the tissue. The discrete rigid region is only meshed on the surface. The rigid region is the master surface in the analysis of course. For meshing, it's best to firstly use symmetry along the mid section of the needle (YZ plane). Partition the rest of the tissue by extending the planes of the needle. If you can't get structured or swept regions then use C3D10M elements.

 

[cal34]

Great points from everyone! It's really helping me flush out my project.

What I'm modeling are flexible needles. When inserted into tissue, the tissue places a transverse force on the face of the bevel, causing the needle to curve downward. I am interested in modeling this downward curvature of needles while also looking at tissue stress.

A 2D model would be very useful (and make my life much easier), but we ALSO want to model the needle being rotated in tissue, as it is being inserted. Unless there are techniques that I'm not thinking about, it seems I have to have a 3D model for this.

Even if you want the displacement of the tip, it still is not an argument for meshing it. Why? Think about it.

The downward displacement of the needle should be due to needle bending, which is why I believe I need to mesh the needle (and cannot model it as a rigid body). No?

NOT isotropic linear elastic materials

Absolutely correct. Other papers in my field, however, have modeled tissue as linear elastic. It's a big assumption, but for a first approximation to my model it is OK. As I refine my model, I will look toward implementing a hyperelastic model (Mooney-Rivlin), as others have done.

So, the BIG reason for modeling the needle as deformable is to observe needle curvature.

until you (and your boss!) are sure about the goals (and underlying assumptions) of the project.

Well, no one here does FEA. My boss just told me to start modeling this problem, though he has no experience with FEA. Which is why I came here and am very grateful for all of your input.

 

[burningDiesel]

For this problem, maybe you can use an Eularian approach (Coupled Eulerian Lagrangian or CEL in Abaqus), where you treat the 'brain' more as a fluid (but not totally, read the manual for more info). For instance, look at these examples from abaqus.
One of them is a pile of concrete driving into soil (pretty much the same problem but bigger ).
Personally, I'd use this approach to get a good estimate of what is really happening. The results can still be half or double of the real value, but qualitatively, I'm pretty sure the results will make sense! As much sense as with this meshed method anyway.
+ you won't have the contact problems.

I think CEL is possible from abaqus 6.9, so you should be able to give it a try.

 

[IceBreakerSours]

The downward displacement of the needle should be due to needle bending, which is why I believe I need to mesh the needle (and cannot model it as a rigid body). No?

Since flexible needle bending is of interest to you, you are correct; you need to mesh it. However, I still think you can get away with a relatively coarse (in comparison with soft tissue) surface mesh.

It's a big assumption, but for a first approximation to my model it is OK. As I refine my model, I will look toward implementing a hyperelastic model (Mooney-Rivlin), as others have done.

It is a good first step.

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083