May 3, 2018 at 2:29 amRashiSubscriber
I'm trying to simulate interference fit between three tubular bodies. All three components are under interference fit and three components have three different alloy materials.
Please see the below image below for the component description.
Component 1 is fixed from both ends. No other forces are included for the simulation. All the contact surfaces are in "Frictional Contact" with 0.1 c.f. All the contact surfaces have matching mesh density. 20 node hexagonal elements are used with sweep meshing. Mesh biasing is used to have more mesh density near the contact surfaces.
Below are the diameters of the three components.
Component 1 = 20 mm
Component 2 = 20.1 mm
Component 3 = 19.9 mm
In the component 2 Maximum stress occurs in the outer two edges where the three components meet. (blue lines shown in the below image)
To see if the result is independent of the mesh, I did a mesh convergence study. Issue is when the mesh density is increased to have more element neat the the contact surfaces, the maximum stress kept increasing. So there were no convergence reached when the mesh density is increased.
I even tried changing the contact detection method, contact formulation method and tried increasing the contact stiffness. But non solved the issue.
Any help to resolve this issue is highly appreciated.
Thanks in advance.
May 3, 2018 at 11:37 ampeteroznewmanSubscriber
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.
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.
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!
May 14, 2018 at 12:50 pmRashiSubscriber
Thank you very much for your reply. I was very busy with solving the issue with interference fit.Still I was not able to come up with proper conclusion. I'll add a full post on my findings later.
However I have one more question. How do you apply forces for asymmetric simulations? Such as Pre-bolt tension? Do we have to modify the magnitude of the force?
May 14, 2018 at 12:59 pmpeteroznewmanSubscriber
In an axisymmetric model, if you wanted to apply an axial force to an end face, which is physically an annular ring, but in the model is a horizontal line, you apply the total force to the line. ANSYS understands that this is applied to the area of the annular ring. No modifications of the force are required.
May 19, 2018 at 11:33 amRashiSubscriber
Thank you for your reply I applied the bolt pretension as you suggested. But I ended up in another problem. This assembly is bit different to the assembly shown above.
In this assembly there's stress singularity near a fillet (please check results at 1st load step, which is included in the simulation file). I have attached the file below. But I didn't include all the mesh convergence steps due to increase of file size.
How to come up with a proper results for this kind of situation?
Also why this kind of stress occurs when there is no sharp corner in the component.
May 19, 2018 at 11:45 amRashiSubscriber
It's 18.2 Peter.
May 19, 2018 at 1:07 pmpeteroznewmanSubscriber
Shaft has been sliced into 3 pieces so that the nut can be bonded to one part, the bolt pretension can be applied to another part, and the frictional contact can be applied to top part. In this way, the location where the Bolt Pretension occurs is well controlled.
You thought you had a stress singularity because the stress went up when the element size went down from 0.025 to 0.0125. If you have a true singularity, the stress might double when the element size is cut in half. Your example did go up by a significant amount, but it was not close to doubling. You just needed to go smaller and smaller to see that the stress does indeed converge on an exact value. I created a Parameter Set with Edge Size as the input variable and Maximum von Mises Stress as the output variable. Here is the result.
There is no stress singularity between the nut and the disk. There is the expected subsurface Hertz contact stress. Look at Figure 3.8 in this reference.
However, with a 0.0125 mm element size, it looks like this:
A more efficient mesh uses a Sphere of Influence mesh control that only puts small elements where they are needed,
at the Hertz contact stress location. That archive is also attached.
Attached is an ANSYS 18.2 archive.
May 19, 2018 at 2:27 pmRashiSubscriber
Thank you very much for your quick reply and taking the time to do the mesh convergence study. I should have reduced the mesh size more as you have mentioned.
I have three questions.
1. When you add the bolt pretension on the split body the force actually applies on the middle of the body right? But to properly simulate the effect of the bolt pretension shouldn't the pretension force be applied on the middle of the body which is clamped by the bolt and the nut? (in the middle of the disk as for this example)
2. Is there a particular reason for applying the bolt pretension to the body similar to what you have done here?
3. I have tried to do simulation with design points but I failed because when the number of elements changed in each iteration. It will remove the remote point which I have attached to a mesh node, since when the number of elements change in the edge ANSYS redo all the mesh to continue the simulation. How did you stop that from happening? Hope you understand my question.
May 19, 2018 at 2:41 pmpeteroznewmanSubscriber
3) In my archive, the remote point is scoped to a vertex and not a node, so it is persistent after remeshing.
1) The way bolt pretension works is that it splits the body in half and grabs the two new faces created and pulls them together with the force that was specified. In the image below, you can see the Y-deformation of the Bolt Pretension, which creates the appropriate tension forces in the top and bottom parts of the shaft.
2) Controlling where the program splits the body to apply the Bolt Pretension is the reason to split the shaft into 3 pieces.
August 1, 2018 at 10:21 amRashiSubscriber
While using perfectly elastic material model(bi linear kinematic hardening > zero tangent modulas) can the maximum stress even increase higher than the yield stress?
August 1, 2018 at 11:10 amSandeep MedikondaAnsys Employee
Hi Rashiga, I wouldn't expect it to. Can you confirm that you are looking at the von-mises stress or principal stress? A picture of material data vs your simulation result would help as well.
August 1, 2018 at 12:26 pmRashiSubscriber
Thank you for the reply. Actually I was looking at the von mises stress. Is it wrong?
Also I got to know that I have to use "ERESX,NO" APDL snippet in order to preview the results below yield stress. So in in solution I have run that command also.
Below I have attached the material data and simulation result.
August 1, 2018 at 1:24 pmSandeep MedikondaAnsys Employee
It should match up unless you have bigger elements in which case, we are extrapolating the stress values from the integration points to the nodes. Yes please right click and insert a command snippet, put the ERESX, NO command in and evaluate the results, this will copy the integration point results to the nodes. Also, look at the plastic strains and if it is zero, that means that we are just extrapolating the linear part of the stress-strain curve.
August 1, 2018 at 2:51 pmRashiSubscriber
I checked the plastic strain and if was zero in the body which I shared the stress results. Is this why the maximum stress is higher than the yield stress?
August 1, 2018 at 3:19 pmSandeep MedikondaAnsys Employee
Yes, this could be the reason. Now, do you have large deflection turned on in your model?
August 2, 2018 at 1:15 amRashiSubscriber
Yes Sandeep, large deflection is turned on.
August 2, 2018 at 3:14 pmSandeep MedikondaAnsys Employee
So if your plastic strain is zero, that tells me that material hasn't yielded (stress at the integration point) yet and so when you are extrapolating this to the nodes, since you are still inside the elastic region of the stress-strain curve, your stress is just being extrapolated and it could be significantly higher especially if the Young's modulus is high. Now, when you calculate the equivalent stress (von-mises) based on these values, the value could be higher than what the yield is. So the best workaround here is to use the ERESX, NO command.
Hope this clears things a bit.
August 3, 2018 at 12:50 amRashiSubscriber
Thank you for the explanation. I totally understand what you are saying.
But the issue is even with the ERESX, NO command I get higher von mises stress than the yield stress. I want to know if I'm doing something wrong. I have included the command to the solution folder. Is it should be included before the simulation or can it be included after the simulation when I'm post processing the results
August 3, 2018 at 1:04 pmSandeep MedikondaAnsys Employee
Yes, this is a little confusing but it needs to be under the Static Structural branch/folder not the solution. When you put it under the solution, it does give you a warning but it is in the Solver Output:
*** WARNING *** CP = 2.328 TIME= 08:54:29
ERESX is not a recognized POST1 command, abbreviation, or macro.
This command will be ignored.
In the case below, I tested this on a simple cantilever beam with a yield stress specified at 250 MPa and a ramped pressure load applied at 240 MPa, when I don't have the ERESX command in there, I observed a value of around 287 MPa but once I put the ERESX command in, I see a value below the yield as shown:
August 3, 2018 at 2:08 pmRashiSubscriber
Thank you Sandeep. I'll try the method which you have mentioned.
- You must be logged in to reply to this topic.
Simulation World 2022
Earth Rescue – An Ansys Online Series
- How to calculate the residual stress on a coating by Vickers indentation?
- An Unknown error occurred during solution. Check the Solver Output…..
- Saving & sharing of Working project files in .wbpz format
- Solver Pivot Warning in Beam Element Model
- Understanding Force Convergence Solution Output
- Colors and Mesh Display
- whether have the difference between using contact and target bodies
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- What is the difference between bonded contact region and fixed joint
- Massive amount of memory (RAM) required for solve
© 2022 Copyright ANSYS, Inc. All rights reserved.