Problem with convergence in mesh independence

  • Last Post 3 days ago
Hassaan posted this 6 days ago

Hello there I have created an assembly of knee joint by 3d scanning of knee joint parts. Imported these parts into creo and assembled them. Then transferred these parts to ansys 18.1. Now the problem is that during mesh independence study, my results are not converging. I gave fixed joint constraint to the knee joint between tibia and femur and also between femur and patella. Then I started reducing the mesh size at the joints. But the trend of values is very bad when a graph is drawn. Any ideas related to it? I attached the assembly picture in the file.

Attached Files

Order By: Standard | Newest | Votes
peteroznewman posted this 6 days ago

Please describe what you are trying to simulate with this assembly of the knee.

Where are you holding these parts fixed to ground?

Where are you applying a load (force or displacement) and in which direction?

What value are you measuring that is not converging?

When you use a Joint to connect two parts, some geometry is selected for each side of the joint (Reference and Mobile). Did you pick an area on each part to connect the Joint? 

Did you set the Behavior of the Joint to Rigid or Flexible?

Are the bones solid or hollow?

What material properties are you using for the bones?

If you are trying to represent the ligaments that hold bones to each other, I would not use a Fixed Joint, it is too rigid. A very simple improvement is to use a Bushing, which has 6 springs on 6 degrees of freedom. A more accurate model would have geometry and material properties for the ligaments themselves.

If you Clear Generated Data on your mesh and create an Archive, it may be small enough to Attach the .wbpz file to your post.

  • Liked by
  • Hassaan
Hassaan posted this 4 days ago

Thank you for your reply peteroznewman.

Actually, My project is to make a stress analysis of knee joint for different daily activities. I have taken all the forces from some papers as well as angles for the joint when these forces are applied. I have to calculate peak stresses acting on this joint during these activities and suggest a material which could bear these stresses.

I have applied a fixed support to the upper part of the femur bone and another support at the lower part of tibia.

One of the forces I am applying is at femur towars tibia. That I am applying through components which were received from a paper. 

Another force is being applied from femur towards patella. I only have resultant force acting from femur to patella. So I converted it to components approximately and applied at this joint.

The values that I am measuring are deformation (total and directional for each bone separately which is converging) + Normal stresses ( for each bone separately) + shear stresses (for each bone separately) + Equivalent von-mises stresses + principal stresses (for each bone separately). Only deformations are converging and error is reduced to less than 2%. But none of the stresses are converging and their data is not giving an error less than 2%.

For joints, I created fixed joint between tibia(reference) and femur(mobile). Also another fixed joint between femur(reference) and patella(mobile).

The bones are solid

Material properties being used are that of a healthy person. These are shown in the following table.


Bones properties

I am also attaching the file with my post. Kindly review it. Thanking you in advance.

peteroznewman posted this 4 days ago

I should have mentioned that there is a 120 MB file size limit on uploads. I got your email and can see your model. I will reply on the convergence question later.

I attach a CT image of a slice through a knee joint. You can see that the bone is very compact (shows as white) for only a small thickness near the surface and is very spongy (shows as darker) in the center.  The table of bone properties shows that the Young's modulus for compact bone is 17,600 while it is only 500 MPa for spongy bone. If your model of the bone is solid throughout using the compact bone properties, the deformation and therefore the stress will be different in that model compared with a model that has a thin wall of compact bone and a center of spongy bone. You could make some simple geometry and test the effect of a compact bone surface thickness with a spongy interior (or even leave it hollow).

  • Liked by
  • Hassaan
Hassaan posted this 4 days ago

Okay. Yes its a good suggestion. I will work on this. Can I give different material properties to one bone in ansys? As in the case described above. I will be very thankful for your reply.


peteroznewman posted this 4 days ago

Mesh Convergence Study
First let me say that I am glad to see you doing a mesh convergence study. Everyone should do this, few actually do. I wrote about this topic in this post. However, I will challenge the 2% you mentioned. There are far larger approximations in your model, maybe even over 100%, which makes reducing the change in stress to < 2% due to mesh size an unnecessary restriction; 10% would be sufficent. 

I will say that 2% can easily be achieved. If you have one mesh that has an element size of 1.00 mm and another mesh that has an element size of 1.01 mm, the stress will change by < 2% so the metric is flawed because it doesn't account for the magnitude of the element size change.  In the plot below, the element size changes by at least a factor of 1.5, which is the other constraint needed in a mesh convergence study.

What you really what to know at the end of a mesh convergence study is what is a good estimate for the exact stress, which is at a zero element sizeYou can do that by plotting the stress vs. element size data and showing that it is converging and extrapolate to zero element size. In the example plot, the exact stress estimate is 1540 MPa based on a linear fit through the last three points. The last two points are 1447 and 1478 MPa. The difference is 2.1% so you could say you had converged. The exact stress estimate is 1540 MPa which is 4.2% higher than 1478 MPa. Isn't that a better estimate?

What I see in your model
Looking at the two forces in your model, they are both applied to the Femur, which also has a Fixed Support at the cut end.

Your model show a tension force on the Femur in the direction of the Tibia, but the Femur experiences a compression force from contact with the cartilage on the Tibia, so I think you have your force in the opposite direction. The force on the Femur from the Patella also looks wrong, the Patella pushes on the Femur, it doesn't pull on it. After you fix the directions of force, you could suppress all the other bones in your model, and just perform an analysis on this one bone. I don't think this is a good way to calculate the stresses in a knee joint.

If you want to calculate the stress in a knee joint, which consists of bones that push against each other through cartilage, you should use contact between the Femur and Tibia and Patella.  Fixed Joints prevent contact from carrying the load properly.

Model Improvement Suggestions
I recommend you draw a free body diagram of the knee to help you understand how the forces pass through the knee joint.


Delete the Mechanical Fixed Joints and use contact with the cartilage and the Femur and the Tibia and contact between the Patella and the Femur. I will warn you that getting models with contact to solve can be challenging.

If you are going to model contact, you must adjust the initial positions of the bones and cartilage so they are just touching. Your geometry has excessive overlap.

A good arrangement is to make the ligament from the Tibia to the Patella be a spring, then you can apply a force to pull the Patella upward.

One Bone Two Materials
You can create one bone with two materials, say compact and spongy, by creating a component in Spaceclaim with two bodies using the Fill command on a hollow solid such as Wall 1. I projected a shape onto the wall to apply a force or connect a ligament or a spring to represent the ligament. This is the model I ran the mesh convergence study on, but I suppressed the interior of the bone to reduce the computation time. I have attached the ANSYS 18.2 archive below.

I hope you find these suggestions helpful.

Kind regards,


Attached Files

peteroznewman posted this 3 days ago


I'm wondering if you should be so focused on the stress in the bones. Most of the wear and tear from daily living on a knee joint is to the cartilage, not the bones. A low impact event like a fall might tear a ligament. It is only a high impact event like being hit by a car or a bullet that will break a bone.

If you want to calculate the stress in the cartilage or Patella ligament, you could treat the bones as rigid bodies. That would save a tremendous amount of computational effort.

Kind regards,