Hi Rashi,

Thank you for a well explained question! I'm always glad to see engineers doing a mesh convergence study. You have found a singularity in your model, which means the true solution is infinite stress. I usually find those at interior corners, but they do exist in other places. The reason for the singularity is the step change in geometry which is being resolved at a point in the tube, not over an area.

**Corner Stresses Matter**

Is the peak stress at those edges of vital interest? If so, the corrective action is to change your geometry and add a small radius to the two corners on component 1 and 2 where they make contact with the inner surface of component 3. Because in reality, there is not a perfectly sharp corner, there is a very small radius. Use enough elements to mesh around the radius and along the tube in the area of radius contact to allow the stress concentration to be spread over several elements. It's good that you biased the mesh to these edges, you just have to take it to the next level.

**Corner Stresses Don't Matter**

Maybe the exact peak stress at the corners is not the central focus of this study and the behavior toward the center is of more interest. There are two approaches for dealing with the results plotting to get a plot that does not include those elements, in effect ignoring the peak stress. There are some FEA best practices for this if you don't want to weigh the mesh down resolving a peak stress that you know about, but don't care about. Here is a post on E-ring groove. You could slice component 2 into three bodies and putting them in a multibody part, the peak stress in component 2 can be plotted by selecting the center body and not including the thin slices at each end, in effect ignoring the singularity. Do the same for the other two components.

**Use Plasticity**

If all your materials are Linear Elastic, another approach is to use plasticity and let the corner element plastically deform to relieve the stress. In Engineering Data, drag and drop the Bilinear Kinematic Hardening material model under the Plasticity category onto the materials for component 1 and 2. Enter in the yield strength for each material and use 0 for the Tangent Modulus. This defines an Elastic Perfectly Plastic material. Then you don't have to change your geometry or your mesh at all!

If you do care about the stress increase at these edges, and you have better information on the strain hardening behavior of materials 1 and 2, then you can enter a non-zero Tangent Modulus or even use a Multilinear Kinematic Hardening material model to capture a more accurate response of the material at the corner. You might even combine this with the geometry modification of adding the radius.

**Use Symmetry**

Your model looks symmetric. If the loads are symmetric, you don't need to model the full length of the components. Add a center plane and cut the model in half, applying a symmetry boundary condition to the center plane and only mesh the solids on one side.

Does your model include only axisymmetric loads? If so I highly recommend you construct an axisymmetric model. That means taking a 2D slice through your components like section A-A and bringing just three rectangular faces into Mechanical to mesh. This will greatly reduce the time taken to mesh, especially if you decide to add the radii. The axis of symmetry must lie along the Y axis and your geometry be on the plus X side of the Y axis. You can also add a center plane and only model one half the length of your components. Now that's a really small model!

Best regards,

Peter