Hyperelastic Shell

[roger_coxNUKZV]

Nonlinear Static Deformation Analysis

I'm modelling a thin part made from a hyperelastic material.

With Tet elements, it crashes when I reduce the element size or increase the displacement, so I believe that it should be modelled in shell elements.

But, with shell elements, as shown in the figure, it only runs if I change the material to Isotropic. With the Superelastic material I get:

FATAL ERROR T2027: NON-COMPATIBLE MATERIAL

I'm looking at a high strain on a material that gets a lot stiffer at high strains, so an Isotropic material is going to give unrealistic results. Any suggestions please?

[John_Holtz]

Hi @roger_coxNUKZV . Welcome to the Inventor Nastran forum.

The thickness of shell elements does not change in a nonlinear analysis. (This is probably why the hyperelastic material model is not supported.) 

Since the part is not that thin (10 mm thick for a 60 mm "diameter" tube) and a hyperelastic material is required, you should use a solid model for the analysis.

John

[roger_coxNUKZV]

Hi @John_Holtz . Thank you for your reply. With Tet elements, it crashes when I reduce the element size or increase the displacement. Any suggestions please?

Strain 5.8%

[John_Holtz]

Hi @roger_coxNUKZV 

That mesh is very coarse. Try to get 3 elements through the thickness of the spring.

Other questions are:

1. What are the material properties?
2. Where did you get the material properties? (Another customer told me that material properties for hyperelastic materials from manufacturers are rarely suitable for simulation. You need to have the material tested by a lab that specializes in simulation to get properties that will work.)
3. How is the part restrained so that it does not move in X, Y, or Z? (whatever the left-to-right and back and forth directions are). I would not rely on friction to hold the piece in place and be able to converge.
4. What is the contact type?
5. What warnings occurred in the analysis?
6. How many increments are you using? (I suggest a minimum of 20 steps for something like this.)
7. Where's the model? It will answer all the other questions reader have and enable readers to try different settings.

John

[roger_coxNUKZV]

Hi @John_Holtz

Thank you for your questions:

* That mesh is very coarse. Try to get 3 elements through the thickness of the spring.

I have made the mesh finer

* What are the material properties?

Type: Hyperelastic

Sub Type: Polynomial

Simple Tension / Compression

Stretch	Stress
	MPa
1.1	0.2
2	7
3	20.8
4	42

* Where did you get the material properties? (Another customer told me that material properties for hyperelastic materials from manufacturers are rarely suitable for simulation. You need to have the material tested by a lab that specializes in simulation to get properties that will work.)

Supplier data sheet

* How is the part restrained so that it does not move in X, Y, or Z? (whatever the left-to-right and back and forth directions are). I would not rely on friction to hold the piece in place and be able to converge.

Constraint 1 - Top face, fixed. A displacement load is applied to this face, to compress the spring.

Constraint 2 - Bottom face, fixed

Constraint 3 - Bolt hole, fixed

Constraint 4 - Side faces, symmetry

* What is the contact type?

Type: Surface to Surface

Contact Type: Sliding / No Separation

Penetration Type: Symmetric Contact

Stiffness Factor: 1

Penetraition Surface Offset: 0

* What warnings occurred in the analysis?

Warning E5074: No Convergence in maximum number of iterations permitted
Fatal Error E5076: Maximum number of bisections permitted reached

* How many increments are you using? (I suggest a minimum of 20 steps for something like this.)

Thanks, I have changed it to 20

* Where's the model? It will answer all the other questions reader have and enable readers to try different settings.

attached

[John_Holtz]

Hi @roger_coxNUKZV 

I assume the enforced displacement of 1 mm is just to test whether the analysis will run or not. I imagine the real displacement is much larger than 1 mm. (The dimension of the tube is 70 mm between the plates and 80 mm in the horizontal direction.)

• If the motion of the plates is small, like 1 mm, then I would use an isotropic material. You know the modulus of elasticity for strains up to 10% is 2 MPa.
• If the motion of the plates is large, then I suggest these changes:
  • Use a contact type of separation. As the tube is compressed, more area will come into contact. That will not happen when using any other type of contact.
  • A simple tension test is not sufficient to describe the complete behavior of a hyperelastic material. You need other test data also. (See How to enter hyperelastic (rubber) materials in Nastran for more details.) Instead, use an isotropic material, set the Poisson's ratio to 0.48, and enter the tension data from the supplier under the "Nonlinear > Nonlinear Elastic". (The theoretical Poisson's ratio if 0.5 which is not a valid number for numerical simulation.)
  • With those two changes, this is the result (with 1 mm motion on the top plate). Note how the tube is not remaining in contact with the plates over the entire area, so separation is the proper contact type.

Let us know if you have any questions.

John

[roger_coxNUKZV]

Hi @John_Holtz

Thank you for your advice:

* Number of Incriments: 20

* Contact Type: Separation

* Penetration Type: Symmetric Contact

* Stiffness Factor: 1

* Coefficient of friction: 0

* Penetration Surface Offset: 0

* Poisson's ratio: 0.48

* E: 0.0001 (I assume this is overruled by..)

* Nonlinear Material Data Type: Nonlinear Elastic (Stress & Strain input)

I tried following it but I am still getting the same error E5076.

[John_Holtz]

Thanks for the updated model. Sorry, but it looks like I made more changes to the setup than what I had mentioned. I made the changes to your new model (using Inventor 2024, the same as you). See the attached file.

I made all these changes at once, so not sure which ones are necessary or if all are necessary.

1. Separation contact as mentioned before. I also entered a Maximum Activation Distance of 2.5 mm to make sure this distance was large enough. (See Tip 18 in the PDF document attached to my forum post Suggested Reading - Tips and Tricks on the Inventor Nastran forum.) As you make the enforced motion larger and points with a larger initial separation will come into contact, you will need to increase the Max Activation Distance to account for the initial gap. I also added the round surfaces on the spring to the contact selection since the tendency is for the contact to occur between other surfaces, especially if you increase the enforced motion.
2. I changed the modulus of elasticity of the steel to 300 MPa. I assume the steel is just meant to be rigid and is not of interest in the analysis. A value of 100 to 1000 times the stiffness of the hyperelastic should be "rigid enough" without being too strong. If too strong, the convergence becomes difficult. (The fully fixed constraints on the steel parts also contribute to the rigidity of those plates.)
3. I agree with your assumption that the modulus of the hyperelastic spring should not matter, but that assumes that Nastran uses the value calculated from the stress-strain curve at all steps in the analysis. That assumption may not be true. Just to be safe, I entered the modulus as 2 MPa. (2 MPa = 0.2 MPa/0.1 strain)
4. I used a larger mesh size (3.5 mm) to reduce the number of nodes and elements in order to get the results more quickly.  Feel free to use a finer mesh if needed once you review the results.

Let us know if you have any questions.

John

[roger_coxNUKZV]

Hi @John_Holtz

Thank you for your further advice. I followed it and repeated your result.

However, when I increase the enforced displacement to 20mm or 5mm, I still get the same error E5076.

Any suggestions please?

[John_Holtz · Accepted solution]

Hi,

You need to look at the results that are calculated, guess why the analysis fails at X% load, and make changes.

• The model converges with 5 mm motion. You may need to increase the maximum activation distance to account for contact occurring between points that are more distant. See the attached.
• The model gets to 75% load with 20 mm motion. See the attached. I could not see an obvious reason for the convergence. The spring does not appear to be buckling, the force is not dropping to zero, the stress and strain are moderate. The question is this: is the convergence problem due to the material or contact. Maybe run the analysis with loads and constraints on just the spring to see if it can be compressed. (Of course the constraints are hard to set to mimic the contact, so it is just an approximation.) If the spring can be compressed, that implies the contact is causing a problem. If the spring cannot be compressed, that implies a problem with compressing the material, such as an element becoming distorted. A different mesh could help with both situations.

John

[roger_coxNUKZV]

It's now working with enforced displacement of 20mm. I just needed to make sure that the maximum activation distance for contact was greater than the maximum displacement.

Thank you so much for your support @John_Holtz!