Learning Forum

[Suresh Varma]

Hello there I am using a thin glass plate to bend it onto the substructure.

Here I am using a double-curved substructure but i cannot have a converged solution i have metioned the details below

I have used shells since both are thin bodies.

i have interface treatment to adjust to touch and here are the analysis settings

For the remote displacement I have set the x direction to 0 and for remote displacement 2 I have the z direction to 0.

with a pressure of 0.25 MPa.

the direction of the top body is to move y direction to take the shape of the substructre but i am having a exceeding limit at uy and these errors popup 

here are the point nodes where this error shows

Thank you

suresh varma. 

[peteroznewman]

Please show the Analysis Settings.  Do you have Large Deflection turned On? That is required. You should turn on Automatic Time Stepping and set the Initial Substeps to 100 or larger.

You also change from Frictionless to Frictional contact and use a small coefficient of friction. This will help the solver to converge because you don't have enough constraints to prevent rigid body motion with a Frictionless contact.

[Suresh Varma]

Hello sir,

I had turned on large deflection and my initial analysis was initial substeps 30 but now I have changed it to 100 and changed the contact to frictional contact and used 0.1 as the coefficient of friction. but still the converged solution is being generated. for your reference, i will attach a link to the file which is in Ansys 2023 R2.

https://drive.google.com/file/d/1q3JTz90Tz4tPZ7Cp4vGo_hyWLY_4HHNb/view?usp=drive_link

 

[peteroznewman]

Unfortunately, the link to the file in your Google Drive only works for email addresses that you have authorized. You should create a link to the file that anyone can use to download the Ansys archive.

[Suresh Varma]

hello sir,

Sorry for the initial link. Now I have adjusted it to work for everyone.

https://drive.google.com/file/d/1rjsMCLaPw5GALe6OpG-p7LSAo-lP4fUo/view?usp=drive_link

Thank you 

Suresh Varma. 

[Suresh Varma]

hello sir,

did you find any mistakes in the file or any rework that needed to be done in the setup with respective to contact or analysis settings?

Thank you for the help 

Suresh Varma.

[peteroznewman]

I found settings that allow the solution to converge. The changes I made were:

1. change contact to Rough, which means no sliding
2. change the contact Normal Stiffness back to the default value of 1
3. turn on Weak Springs to resolve the rigid body motion issue
4. suppress Remote Displacements
5. reduce the pressure to 1e-5 MPa

https://jmp.sh/LDVt41l6

This pressure will not push the corners down, so make the analysis a 2-step solution where a higher pressure can be applied in step 2.

[Suresh Varma]

hello sir,

I understood the first four changes but for the fifth one, you are suggesting me to initial step apply a low pressure of 1e-5 Mpa and in the second step applying a high pressure of 0.25 Mpa.

I will add this step and let you know the results sir

Thank you for the help 

Suresh Varma.

 

[Suresh Varma]

Hello sir,

I have performed the analysis using a two-step pressure where the initial pressure was 1e-5 Mpa and the second step 0.25 Mpa but the solution only converged till the initial low pressure and unconverged for the second load step.

So I tried a three-step process as well with an increment pressure but still the same problem exists. Can you have a look into this once

https://drive.google.com/file/d/1rm1wFVo9qOdHEMeT2r6alliEcdjnLdZ1/view?usp=drive_link

Thank you for the help

Suresh Varma.

[peteroznewman]

Hello Suresh,

The applied pressure in my model was 1E-5 MPa and that took 185 iterations to converge.

You want a pressure of 0.25 MPa which is 25,000 times larger. I haven’t looked at your model, but did you try just doubling the pressure to 2E-5 MPa in step 2?  I expect that will converge in less than 185 iterations.  If it does, you can double that again and do 4E-5 MPa in step 3. You only have to keep doubling 15 times to exceed 0.25 MPa.

If you take this approach, you should configure the Analysis Settings, Restart Controls to be able to restart the analysis from the last step and to not delete the files when the analysis is complete. Then you also need to know how to restart from the last step. If you don’t do that, then the solver will start from the beginning each time, which would be a waste of time.

Another way to save time is to increase the element size. You could double the size of the elements without much harm to the quality of the results. That will reduce the size of the model by a factor of 4 with a corresponding reduction in solution time.

The corners are 144 mm above the fixed surface. In my solution, the corners moved 17.8 mm. If the model was linear, you would only need to double the load 3 times to get to 144 mm. The model is nonlinear so it may take more than that, but once the corner has a positive contact pressure, do you need to add any more pressure?

Regards,
Peter

 

[Suresh Varma]

Hello sir,

I will first look into the process you mentioned about restarting from the last step and later if I cannot do that I will look to change the element size as well.

with regrads to pressure I only need it to make the upper thin body to take the shape so once the corners have the contact i dont need to add more pressure is that what you are asking about?

thank you for the help 

Suresh varma.

[peteroznewman]

Yes, double the load three times in 3 steps.

• Step 1 pressure = 1E-5 MPa
• Step 2 pressure = 2E-5 MPa
• Step 3 pressure = 4E-5 MPa

If the corner is not touching, add Step 4 and double the pressure again.

[Suresh Varma]

hello sir,

I will do these steps until the corners touch and I will post the results here soon.

thank you for the help

Suresh varma

[Suresh Varma]

 

 

hello sir,

It took some time for me to do this restart process but I have some results.

in this case, my structure is a bit moved I guess even with weak springs can you just have a look at the figure below.

and the pressure vs. displacement are as follows

Pressure 1	1e-05	1e-05	1e-05	1e-05	1e-05
Pressure 2	1e-05	1e-05	1e-05	1e-05	1e-05
Pressure 3	4e-05	4e-05	4e-05	4e-05	4e-05
Pressure 4	8e-05	20e-05	34e-05	84e-05	164e-05
Respective deformation	86.99	101.24	105.27	106.54	109.56

Thnak you sir 

suresh varma.

 

 

[peteroznewman]

Hello Suresh,

The rigid surface you are wrapping about has a length of 1.438 m across the diagonal plane.

The length of the flat film you are wrapping has a length of 1.414 m on that diagonal plane.

So naturally, the corners of the flat film will not reach the corners of the rigid surface after wrapping.

If you want to know if the film has made contact with the rigid surface out to the corners, you should insert a Contact Tool into your Solution section and request the Contact Status, Contact Pressure and Contact Gap.

[Suresh Varma]

 

hello sir,

Thank you for the explanation I just verified my theory of this study so you are right about the corners. As the initial curved body dimensions are different from the top body dimensions which justify the model.

I have a similar analysis but with the different curved body so I used same process but here I got convergence for low pressure but at higher pressure it tend to fail one reason i knew is that the corner points are higher while the centre surface is a bit lower.

Sir could you have a look into the file and maybe suggest me any methods to converge it. I will attach the file link here.

https://drive.google.com/file/d/13Osu7YgcboEiJmv6i7Li_PgbIDSK-V9S/view?usp=sharing

 

Thank you 

suresh varma.

 

 

[Suresh Varma]

hello sir,

Did you find any error in my model regarding the analysis of this type?

Thank you

with best regards 

Suresh varma.