Mesh Convergence Study -Parameter

  • 194 Views
  • Last Post 4 weeks ago
  • Topic Is Solved
Johnsoldo posted this 05 September 2019

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? 

Order By: Standard | Newest | Votes
Johnsoldo posted this 4 weeks ago

i do. Can you look in ? 

Attached Files

peteroznewman posted this 4 weeks ago

My description of long and short clamps is only true if the cross-section for both clamps is equal.  The long clamp must be thicker so ends up being stiffer than the short clamp and generates a higher reaction forces for the same displacement. 

Do a mesh refinement study to determine if the small clamp has a singularity.

Johnsoldo posted this 4 weeks ago

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.

I checked the reaction force at the displacement and the reaction force at the long clamp is higher. Does the stress then not have to be higher ? Is it possible that a small clamp has a singularity ? 

peteroznewman posted this 26 September 2019

You have a force of 1.3 kN which is very low. The tension force in a fastener could easily be 14 kN which is more than 10 times larger.

  • Liked by
  • Johnsoldo
Johnsoldo posted this 24 September 2019

I think I understand what you mean. can you recommend literature to me to really understand that?

but I can't yet estimate why the stress and deformation are so low at a force of 1360 N or is the normal ?

peteroznewman posted this 23 September 2019

Deformation is defined as the distance moved from the initial position to the final position.

Consider a 100 mm long beam that starts out horizontal.  The left end of the beam undergoes some local deformation on the order of 1 mm, and that deformation causes the beam to rotate 6 degrees about the left end. That means the right end of the beam moved 100*sin(6) = 10 mm.  The middle of the beam moved 5 mm from its original location.  So you see the part of the body the furthest distance from the axis of rotation shows the biggest deformation.  

Contrast that with strain, which is local deformation.  The maximum strain is at the left end where the local deformation was large. The strain at the middle and right end of the beam is zero because there is no local deformation.

Johnsoldo posted this 23 September 2019

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 ?

 

peteroznewman posted this 22 September 2019

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.

Johnsoldo posted this 22 September 2019

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. 

gfd

peteroznewman posted this 21 September 2019

I think the clamps have the wrong face selected for a boundary condition as described in item #1 above

Johnsoldo posted this 21 September 2019

ok thx for informations. i will think about this. 

 

can you take a look at the static analysis?. 

Are the total deformations and stresses so correct? 

peteroznewman posted this 21 September 2019

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.

Johnsoldo posted this 20 September 2019

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? 

 

peteroznewman posted this 17 September 2019

Johnsoldo,

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.

Johnsoldo posted this 17 September 2019

baseline model:

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 ?

peteroznewman posted this 16 September 2019

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.

Johnsoldo posted this 16 September 2019

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 )? 

 

 

peteroznewman posted this 15 September 2019

I can clarify any point I made if you can't reproduce it yourself.

Johnsoldo posted this 15 September 2019

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

thx

peteroznewman posted this 14 September 2019

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.

  • Liked by
  • Johnsoldo
Johnsoldo posted this 14 September 2019

here it is. 

https://drive.google.com/open?id=13EIvYDucS-vmicHqzrwOKHPZGDZWpsUo

 thx you for the run.

Goal is: 

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 

peteroznewman posted this 14 September 2019

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.

Johnsoldo posted this 13 September 2019

i get an error message when uploading. is there an alternative method to upload it ?

peteroznewman posted this 13 September 2019

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.

Johnsoldo posted this 13 September 2019

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 

peteroznewman posted this 11 September 2019

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.

Johnsoldo posted this 11 September 2019

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 ?

peteroznewman posted this 10 September 2019

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?

Johnsoldo posted this 10 September 2019

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.

peteroznewman posted this 08 September 2019

It looks like it will converge on an 870 Hz frequency at a zero element size.

Show More Posts
Close