Hi Mohamad.
In order for the results to be symmetric, the following need to be true:
- Geometry is symmetric. (true in your case)
- Loads are symmetric. (true in your case)
- Material is symmetric. (true in your case)
- Constraints are symmetric. (not true in your case. I will explain below.)
Can you provide more details about what you are seeing? For example,
- What is not symmetric in the results? Or what are you expecting to see different?
- The model did not include a nonlinear analysis with shrink fit. Where is that model?
For the symmetry of the results, your results look symmetric left to right and certainly have some symmetry top to bottom (Z direction). Since the cylindrical "shell" is only held in place by separation contact, and because the "shell" has a larger coefficient of thermal expansion than the solid, the "shell" contracts more than the solid. Are you expecting the "shell" to be floating in the middle so that the top-to-bottom displacement is 100% symmetric, like this?
Photoshopped image. Deformed shape exaggerated. The deformed shape is symmetric about the two centerlines shown. This is not going to happen in the analysis.
A more important question is this: why did the analysis give results when the model is statically unstable? It should have given an error because there is nothing holding the cylindrical "shell" in place! (At the very least, the "shell" is free to rotate about the Z axis.) Because of the shrinkage, the shell is also free to move in Z. The model is not statically stable.
The answer to this question is the analysis made an arbitrary decision about how to stabilize the model. In your analysis, the "shell" remained at the top of the solid. (I am assuming the Z axis is up in your image. The mini-axis is missing.) In my analysis, the shell remained attached at the bottom of the solid. The deformation or strain is symmetric; the displacement magnitude is not symmetric because the arbitrary constraint added by the solver is not symmetric. The results of your analysis and my analysis are both correct even though the displacements are completely different!
In my opinion, it is better to setup the analysis properly so that you get the results you want instead of letting the solver change the setup and give results that it wants to give! For example,
- bond the face on the top (or bottom) between the I.D. of the "shell" and solid so that the shell is statically stable. (This simulates that when the "shell" contracts more than the solid, the friction holds the "shell" in contact with the solid. This is an approximation but hopefully better than unexpected results.)
- split the outer face of the "shell" along the horizontal plane of symmetry. Apply a constraint so that the "shell" cannot move in the Z direction. Also apply constraints somewhere on the "shell" so that it cannot rotate about the Z. (This requires other splits so that nodes can be fixed in the appropriate direction while still leaving the "shell" free to contract.)
About shrink fit, I did not find a tutorial or video. Perhaps someone else knows of an example that I could not find. Otherwise, please attach the model with the shrink fit setup. Someone will look at the model and explain why it was taking longer than 20 minutes to start analyzing, and if the shrink fit setup is proper or not. Note that this article describes the basic steps to setup a shrink fit analysis. See How to perform a press-fit analysis in Inventor Nastran and Nastran In-CAD.
John
Hi,
Thank you for the explanations.
The simulation involving shrink fit was deleted. The results of my current simulation resemble those in the second picture you provided, although the numbers are different.
I tried two options: the first yielded similar results to before, while the second still lacks accuracy. The images of the total assembly in the xz and yz planes are below. I am unsure why the displacement contours are not continuous.
I have attached the model with the new constraints for your review to identify any missing elements.
If this method does not yield accurate results, I will consider using the shrink fit approach.
In this model, I pressed ''kill Nastran'', because I wanted to change a constraint and then I faced crash again and the window was closed. Although we installed the graphics driver and I am using Inventor 25, the crash happened. Do you think we should buy a graphics card for the PC to resolve this problem?
Best regards,
Mohamad
Hi Mohamad.
You made the model 8 times more complicated. Instead of splitting the shield into 8 separate bodies, you should have split the outside face into 8 section. This would have left the shield as a single body.
- With 8 bodies, you need to use bonded contact to keep the pieces together. Bonded contact is an approximation at best and should only be used when there is no other option.
- When you try to create a section view exactly on the plane where the body is split, in theory the section plane does not cut any elements. That is why there are elements "missing" in the display. You get a partial section view of the shield just because of round off accuracy. Move the section plane 0.1 mm in either direction to see what you were expecting.
Here are other problems with the new model:
- The mesh was created with Continuous Meshing checked on. You do not want the parts to be continuous because you are using separation contact between pieces. The continuous meshing is why the shield is "stuck" to the other part at two locations. (Continuous meshing is not designed for solids, so you should only use Continuous Meshing with shell elements. It is only random chance that nodes on separate pieces get merged together.)
- Not a big problem in this analysis because the results are symmetric, but you do not need the X, Y, Z symmetry constraints on the entire face through the thickness of the shield. Because these constraints are artificial, you should place them on the least amount of geometry possible. I was thinking about the edge on the outside face of the shield. Now that I see the model with the splits, you only need to put the constraints at the 4 "corners" where the symmetry planes intersect. (Z constraint at 4 points or vertices, Y constraint at 2 points, X constraint at 2 points.)
Speaking of symmetry, the model has 3 planes of symmetry. You could cut away 7/8 of the model and make a 1/8 symmetry model. The symmetry constraints would then provide all the stability needed in the analysis. (Also, a smaller model would run faster even if using a smaller mesh.)
1/8 symmetry model with the 3 symmetry planes highlighted (red, green, blue).
John
Hi,
Thank you for your guidance. Initially, I attempted to split the surface along the z-axis in Inventor, but it did not work, although splitting in other directions was successful.
I created a new section of the entire geometry (1/8 symmetry model) as you suggested. The results appear to be satisfactory, with the exception of an issue with the mesh. As shown in the images, the mesh was not generated continuously. I experimented with different mesh qualities and sizes, but certain areas still lack elements. What could be causing this problem?
Mesh
displacement in z direction
Total displacement of the assembly
Could you please check if the analysis or geometry have problems?
Thanks
BR,
Mohamad
