Hi, I would like to conduct a mesh convergence study with a h-method. Which comparative parameter can you use to evaluate the different elemten-sizes? Deformation, eigenfrequency?
Mesh Convergence Study -Parameter
- 141 Views
- Last Post 4 weeks ago
- Topic Is Solved
That is entirely up to you. Deformation will converge more quickly than stress in a Static Structural model. Deformation is irrelevant in a Modal analysis but that is where frequency is relevant.
what values do you take for the deformations ? min, max or average?
i have performed a mesh congenence study using the h method. i refine the mesh with a global element size (10 mm to 1 mm) and see when my 1st eigenfrequency convenges by modal and max. Deformation by Static Structural convenges . The results show me that:
but that doesn't look like convengence or ? because the values are quite far apart.
It is easier to see what is going on if you plot the data rather than provide a table. I can't plot it myself because the table is an image not text.
Please reply with an image of the mesh and say what global element size is shown in the image.
Hello, here's the plot from the table.
i find at the end the 1st eigenfrequency still rises and does not converge.
i vary the global element size and everything else is default. what mesh do you want to see?
The table was of element sizes from 20 down to 4 mm. If you plot that, then you can see how the curve might extrapolate to a zero element size. When you plot number of nodes, it's difficult to extrapolate to infinity.
The table didn't have a zero frequency. Don't plot 0,0.
I wanted to see how big the model is compared with 20 mm.
Hello, if I calculate an element size smaller than 3, the simulation does not calculate at all. I thought if I made the element size finer with my mesh, my eigenfrequency would converge, but from the digram the curve rises even further. Which mesh do you want see to compare ? 20 mm and ?
It looks like it will converge on an 870 Hz frequency at a zero element size.
yes, but as you can see, the gradient at the end is even bigger. I thought that the gradient would become lower when the mesh was fine-tuned.
The results from the very large elements, 10 mm and larger were not in the Asymptotic Range of Convergence. Read what that means in this link to a mathematical formulation for a grid independent solution.
What happens with the element size is set to 3 mm? The solver fails? Is that due to a lack of memory or disk space?
I mean, the gradient from 6 mm to 4 mm is getting larger. I thought that the gradient between the frequencies would be lower if I refined the mesh. yes the solver fails, when i set the element size under 3 mm i think, it is that due to a lack of memory or disk space. How can i fix it ?
The two points at 4 and 6 mm define a gradient. The point at 8 mm lies almost exactly on that line. The gradient isn't getting larger. If the result at 3 mm lies on that line, that is confirmation that we are in the asymptotic range of convergence.
If you show the error, that would help understand what is needed to allow the 3 mm mesh to solve.
If you Clear Generated Data on the Model, that will delete the mesh. Save the file then use File > Archive... to save a .wbpz file. Attach that file after you post your reply and I will run the solver at 3 mm. My computer has a lot of memory and storage. Say in your reply what Release of ANSYS you are using.
i mean the frequency difference between 6 to 4 mm is bigger than from 8 to 6 mm. I have thought with increasing mesh frequency difference decreases.
i use R2
You are not thinking about this correctly. I urge you to read this paper. Here is simple way to describe the asymptotic range of convergence in a mesh refinement study. If the mathematical model of the FEA has a linear convergence with element size on the exact solution, then a straight line plot is exactly what you expect to see. Plotting the data for a 3 mm element size might convince you of this fact.
Do you want me to run the 3 mm element size so you can plot the next point on the graph? If so, Clear Generated Data on the Model, that will delete the mesh. Save the file then use File > Archive... to save a .wbpz file. Attach that file after you post your reply.
i get an error message when uploading. is there an alternative method to upload it ?
The file size limit for attaching a file to a post is 120 MB. Did you Clear Generated Data on the Model/Mesh before you saved the file? What is the file size of the .wbpz file?
If you have a Google email, then you have a Google Drive which means if you attach that file to an email and the file is > 25 MB, it will automatically upload it to your Google Drive and provide you with a link to the file. You can copy and paste that link into your reply.
Microsoft has a similar feature with OneDrive.
here it is.
thx you for the run.
i would like to know up to which mesh size i should refine my model, so that i have a compromise between exactness and processing time.
When you see the table, the p value decreases with a small net size.
grid 4 and 2 = 0,96854 - 0,96178 = 0,00676
grid 2 and 1 = 0.9705 - 0.96854 = 0.00196
and with my model i have also thought, if the mesh size decreases the frequency deviation decreases
I don't like that the element size is changing where the contact is defined. I created what I call a Baseline model where the contact element size is always 2.5 mm while the global element size varies. Here is the result:
Global Element size = 8.4 mm. First natural frequency = 1111 Hz. Baseline.
Global Element size = 2.5 mm. First natural frequency = 1113 Hz. Change from baseline = 1.8%
There are much larger sources of error in the model than the element size. The following models are all computed with a global element size of 8.4 mm.
MODEL CHANGES AT CONSTANT MESH SIZE
1. Changing Face. The boundary condition on the clamps does not represent reality. The clamps have a displacement BC on the large (red) face of the clamp that is 0, 0, 0.001 mm. This is a source of error because the real clamp is not pressed down over the whole face, but instead by a nut or washer on the small annular (green) face. Moving the displacement from the top face to the annular face has a large effect on the natural frequency by adding more flexibility to the model.
First natural frequency = 886 Hz, Change from baseline = 20 % reduction
2. Rough contact. The contact between the clamp and the hook is defined as Frictional with a coefficient of friction of 0.2. If the contact was changed from frictional to rough, then no slipping is allowed.
First natural frequency = 1209 Hz, Change from baseline = 8.8% increase
3. Static Structural Pre-Stress analysis vs. No Pre-Stress analysis. When you do not have a Static Structural Pre-Stress, ANSYS converts the Frictional Contact to Bonded Contact and uses the Initial Contact Status and any nodes that are closed become bonded. To do this, I used Fixed Support to replace the Displacements on the red face of the clamps. Eliminating the Static Structural Pre-Stress has a large effect on the results.
First natural frequency = 1337 Hz, Change from baseline = 20% increase
4. Bonded Contact with No Pre-Stress. The Frictional contact was replaced with Bonded Contact and there is no Static Structural Pre-Stress.
First natural frequency = 1356 Hz, Change from baseline = 22% increase
MESH CONVERGENCE STUDY
Back to the question of mesh convergence, here is a plot of a Modal parameter sweep of element size using model #4. Bonded Contact. Look at how the four points with the smallest element size lie on a straight line. This is a good result for a mesh refinement study. There is only a 2.5% change from the 8.4 mm element size to the 2.5 mm element size and an even smaller change to the zero element size.
3) with my settings of my model, this is equivalent to the Static Structural Pre-Stress? i thought with the displacement boundary condition i can perform a static structural pre-stress
can you send or upload your file ?
so i can look in and understand your meaning better
I can clarify any point I made if you can't reproduce it yourself.
which boundary conditions you have configured for the baseline model.?
did you still calculate the element size 3 and 11 mm for my model (First natural frequency )?
I didn't change any boundary conditions for the Baseline. I used 2.5 mm for the four mesh contact sizings, while setting 8.4 mm for the global mesh size. I then looked at only one other point, the global element size was set to 2.5 mm.
can you perform the MESH CONVERGENCE STUDY for element size 2 and 1 mm and tell me the results for the first eigenfrequency and the Elapped Time ?
Why do you want to know information about element size 2 and 1 mm?
I showed you the first two points and that it is a straight line. I can extrapolate to zero size.
Size = 8.4 mm, Freq = 1111 Hz
Size = 2.5 mm, Freq = 1113 Hz
Size = 0.0 mm, Freq = 1113.8 Hz
The numbers you are looking for are somewhere between 1113 and 1113.8 Hz. Why do you care about such a small change of 0.08 % when I am telling you about changes in the model that create a 20% change?
Please pick one of my posts and click the Is Solution link to mark that as the best answer to your original question. If you particularly liked any of my posts, you can click the like button.
so how does the frequency deviation strongly depend on the contacts? Which contacts do you recommend to me?
can you take a look at the static analysis?.
Are the total deformations and stresses correct?
Validation is when you take a measurement on a physical sample and compare it with a model result. Model tuning is when you adjust some aspect of the model to change the model result to make it agree more closely with the physical measurement. Can you take a measurement of the natural frequency of the hook in the clamps? There are non-contact displacement sensors that can be used to measure the vibration of the hook when excited by a Modal hammer strike. Alternatively, you could place a lightweight accelerometer on the hook. Do you have access to any of these kinds of instruments? If not you can rent them.
What do you need to know the natural frequency for?
To what accuracy do you need to know the natural frequency?
It is a good practice to report a range for the key response, frequency in this case, to show the uncertainty in the model. That is what I was doing above, showing how different contact conditions can move the frequency around. If you can do validation, then you can tune the model instead of reporting on the uncertainty.
I've adjusted the boundary condition like #1. It seems to me that the stress and deformation is very low.
I got the following values:
max. deformation: 0,00246 mm
max. voltage: 20,481 Mpa
force reaction: 1360 N
Is there any way to explain why the values are so low?
Is there any sense why you place my max. deformation there, see photo. I have thought that the location of the max. deformation is near my clamp, because there the forces act.
There is a long clamp and a short clamp. The long clamp is more flexible than the short clamp. When both clamps have the same displacement on the annular face, the long clamp will generate less force and less stress, while the short clamp will generate more force and more stress. If you apply a large force instead of a displacement, then the forces on both clamps can be larger and the stresses will be similar in magnitude.
When the hook deforms, there is some rotation of the body. The part of the body at the furthest distance from the axis of rotation shows the biggest deformation.
but is it normal that the stress and deformation are so low?
"When the hook deforms, there is some rotation of the body. The part of the body at the furthest distance from the axis of rotation shows the biggest deformation."
I don't understand why the part of the body furthest distance from the axis of rotation shows the biggest deformation. do you have any literature you can recommend to me ?
- 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