Hi there peter, How would I be able to do a mesh convergence study on this model? Can I just vary the body sizing for the coating and substrate and keep the body sizing for the indenter the same? Then compare with different body sizing and look at the maximum principal stresses for example?
Mesh Convergence Study
- 2.2K Views
- Last Post 06 March 2018
Hi libin, I moved your new question to a new discussion topic since the other thread got too long to scroll to be bottom!
Here is my post on Mesh Convergence Study when using linear elastic materials.
Did your final model include plasticity? I haven't studied how plasticity will affect the mesh convergence study. I am usually looking at Total Strain as the quantity of interest in a plasticity model. You could try that.
I haven't considered plasticity in my final model, just the young's modulus and v.I don't really understand how I can use the stress for the indentation model. Would I just be able to keep the indenter body size constant and then vary my body sizing for substrate and coating, then solve for equivalent stress and plot the max stress against body size used??
I have also tried to create a path but I'm not sure how I would be able to make sure that the path lies on the surface of where I want to measure the stresses?
You originally asked about a Mesh Convergence Study. That means a study on how the mesh, specifically the element size affects the results. When you are doing a Mesh Convergence Study, you don't change any geometry. You only change the element size. If you are not doing that, then maybe the title of this thread should be renamed.
The path will find the nodes and elements that are touching on the mesh before the deformation occurs and report on those after the deformation occurs.
Yeah, sorry about that. So if I just keep all the geometry the same and change the body sizing on mesh controls i.e. the element sizes and solve for the equivalent stress, would this be the correct way for doing a mesh convergence study?
I have tried to do a study by using the force reaction. I have kept the element sizing fir the indenter constant at 0.09 mm and I varied the element sizing of the coating and substrate. I have found that the reaction is nearly the same from 0.1 mm. From this, can I say that it converges at a value of 0.1 mm?
Is this a correct method to use?
One rule for mesh convergence study is that the ratio of element sizes has to be a minimum value of 1.3 but I often use 1.5.
You can't go from increments of 0.1 to increments of 0.01 and say that you have converged because if you go to an increment of 0.001, the answer won't change much. That is why you have to use a constant ratio of element sizes.
If you use Body Size, you will get small elements over the whole body that will slow down the solution. It's best of you have a face and edge Mesh Size control to keep the number of extra elements to a minimum, but you also need good element shapes or you won't get convergence, so you may have to use Body Size.
This was extremely helpful, I did end up having to use body sizing which takes a long time. Thank you!
Hi there, I was wondering why I'm getting a tensile stress at the bottom of the indenter tip, it should be a max compressive stress at the bottom and then a tensile stress along the path of the edge.
Maximum compressive stress is the most negative value of the Minimum Principal Stress.
Maximum tensile stress is the most positive value of the Maximum Principal Stress.
Stress is a tensor not a scalar value. You should review tutorials on Mohr's circle.
If you plot the Minimum Principal Stress, you may find the most negative value (minimum) is at the tip of the indenter.
This is causing problems for me as I am not getting the correct position of maximum tensile stress. The maximum tensile and compressive stresses both line on the tip of the indenter by this model. This is not correct though as the maximum compressive should be on the tip and the maximum tensile should lie on some distance along the edge.
This picture is from that article, it shows maximum principal stress. It shows that it is maximum (tensile) along the path of the indenter. Could this be because they are considering plastic properties of the material?
That plot of maximum principal stress shows the maximum tensile stress in red where the MX is shown and is on the face of the sample, away from the indenter. What does your model show?
This is different form my model as the maximum tensile stress in my model apparently occurs at the tip of the model.
I think I have found the problem finally! The coating does not get displaced the same amount as the indenter. Is this due to the meshing??
The contact may have some penetration. A different contact formulation may help. A different symmetry slice may help. I recommended slicing on the indenter edges, you chose to slice on the indenter faces.
I have used a frictionless contact. I have also used the symmetry slice along the edges in the archive i have sent in this post. Even if i decrease the displacement of the indenter to 0.05 m, it does not get down that far in the coating. I have asked an expert that i know and they said that gradually decreasing the hex mesh like you did for the initial model you made for the elastic material would be the best way. However, I cannot get that simulation to work on my computer, I have tried several times to do so.
In the frictionless contact menu, there is options for contact detection, is this what you mean? Some other people have also told me to play around with this, but I'm not sure what it does. Please have a look, I'm really really struggling and I need help.
Yes, the best way to reduce penetration is to have smaller elements, and as you say, I already showed you that. By default, the contact is applied at points within the face and not at the nodes, so when you have smaller faces, you have contact points closer to the tip. There is a detection method that uses the nodes instead of points within the face. That will be best, and models I have sent you already included that.
You say your model is not working, by which you mean solving to the full displacement. That is because you don't have a hex mesh that can handle the distortion. In your file, make two slices in the corner so you can create a nice hex mesh in the corner so you can bias the elements to be very small in the corner. Then the outer piece can have a tet mesh to apply pressure to the model.
I downloaded the archive file attached above, but it is corrupt and cannot be opened. Please attach a new copy for me to look at.
Can you try this one? I'm really sorry for bothering you.
With Edge Sizing mesh control, the bottom of the Details window has Bias options.
I'm opening your recent model now.
I'm trying to do a model as well. I've used some bias here as well.
Does this make sense? I have maximum tensile stress along the edge of the indenter, near the corner and the maximum compressive stress at the tip of the indenter. This does not go in fully to the coating, but it gets to 0.82 mm when I put a displacement of 0.1 mm.
The coating does not get displaced the same amount as the indenter.
Let's be more accurate. The coating does not get displaced the same amount as the surface of the indenter where the displacement was applied.
Have you looked at the surface of the indenter where it pushes on the coating? If you do, you will find the tip of that surface has displaced 0.077 mm while the top of the indenter has displaced 0.1 mm. The indenter is flexible and the contact pressure is compressing the indenter by 0.023 mm so naturally the coating cannot be displaced any more than 0.077 mm.
The other effect is contact penetration, which is set to Program Controlled. Penetration further reduces the coating displacement. If you enter an allowable penetration of 0.001 mm, then the solution will take longer to compute, but you will reduce the loss of displacement due to contact penetration to less than 1% of the applied displacement.
The edge bias you show on the top of the coating needs to be reversed. You have the small elements opposite the corner where the indenter is. However, you can probably get a solution without the edge bias on the top. You have proper edge bias direction on the centerline, through the thickness of the coating.
You have to show two separate plots to show max compressive stress (Min Principal) and max tensile stress (Max Principal). You have only shown me one plot for max tensile. The minimum value of the Max Principal Stress does not equal the maximum compressive stress.
- All Categories
- Community Rules, Guidelines, and Tips
- News & Announcements
- Student Products
- Pre and Post Processing
- Physics Simulation
- Tutorials, Articles and Textbooks
- Installation and Licensing
- Student Competition Teams
- eMasters Degree from UPM
- Site Feedback
This Weeks High Earners
- 1 Product and CAD Configuration Manager - No Products Displayed
- 2 student v 19.2 quits right after loading
- 3 Mass flow inlet in Eulerian VOF model
- 4 How to define Boundary Conditions for my complex model (and how to unite the similar geometries)
- 5 SpaceClaim - The geometry editor was closed abnormally.