Nonlinear Simulation Error 5075 - Maximum number of bisections permitted reached

[kurtoglu_33]

Hi there,

I have a project about nonlinear simulation. I would like to tell you some information about the simulation study and occuring error. 

- Material Type -> Hyperelastic, Mooney Rivlin custom material. Thermoplastic PolyUrethane

- Load -> Pressure (Approximately, 0.06 MPa) (To inner all surfaces) <This material and design should resist 0.5 MPa but I can't load over 0.0.6MPa because of Error 5076 >

- Mesh Settings( Model-base Size 10%) // When I change to 5%,1% or absolute size 5mm, Fusion gives me Error 5076.

- Nonlinear Simulation ( Number of Steps : 600)

There are 5 different types of studies;

 -E600_Mesh-10%_0.06MPa - Succeed

 -E600_Mesh-5%_0.06MPa - Solver Error

 -E600_Mesh-5mm_0.06MPa - Solver Error

 -E60_Mesh-5mm_0.01MPa - Succeed

 -E600_Mesh-5mm_0.07MPa - Solver Error

Could you help me about this Error 5075, please?

E600_Mesh10%_0.06MPa

[Anonymous]

Can you share a link to the file?

[kurtoglu_33]

Sure, here you are. Thank you for quick response.

Link ; https://drive.google.com/open?id=1G_aY_Yt3IVgQmht5Yx8vsEC6JXNuNvOV

[Anonymous]

I took a look at the model and I noticed a few things:

1. That geometry is going to be a challenge because of the thin wall sections and sharp right angles throughout. But a 10% mesh will be very inaccurate for any setup. 
2. I can't access the material properties because they didn't transfer with the file. Can you detail the properties of the mooney rivlin material you've chosen? I'll also add that I have always had difficulty with the mooney Rivlin model on any solver (ANSYS, Solidworks and F360) because of sensitivities to deformation and biaxial loading. What I typically do to ensure it's an issue with the model and setup is to use an approximate modulus with a linear or non-linear material. 
3. Regardless of material model, the simulation needs to be non-linear because of large displacements. 
4. 600 steps is quite a few. I'm not sure why you would need that many.
5. The Mooney-Rivlin model can be unstable depending on your material coefficients, load case and total range of deformation. I believe it may be good up to 200% but can still become unstable under your load condition.

I would try to run the same simulation with a ~3% mesh size, a linear material and maybe just 10-20 steps. It's possible this simulation will not solve on F360 because of limitations with the Mooney-Rivlin model. 

What are you trying to learn from this simulation?

[kurtoglu_33]

Thank you for your response, I'll answer all things and I am sharing Physical Material Properties with you.

1. That geometry is going to be a challenge because of the thin wall sections and sharp right angles throughout. But a 10% mesh will be very inaccurate for any setup. In this project, I am researching optimum design that most bend with inner pressure (Like as pressure type of pneumatic system)
2. I can't access the material properties because they didn't transfer with the file. Can you detail the properties of the mooney rivlin material you've chosen? I'll also add that I have always had difficulty with the mooney Rivlin model on any solver (ANSYS, Solidworks and F360) because of sensitivities to deformation and biaxial loading. What I typically do to ensure it's an issue with the model and setup is to use an approximate modulus with a linear or non-linear material. I'm sharing a link with you about material properties basic and advanced screenshots and an excel document to create new custom material for simulation. The material I used Hyperelastic material and its called Thermoplastic Polyurethane(TPU), I couldn't find in Fusion 360 Library, so I created a custom TPU for simulation.
3. Regardless of material model, the simulation needs to be non-linear because of large displacements. Yes, you're right. There is a large displacement on model but I need so much more displacement(Bending) 
4. 600 steps is quite a few. I'm not sure why you would need that many.Yes, it is. When I simulate in 20 steps, Max displacement is being approximately 30mm, But when I simulate in 600 steps, max displacement is being approximately 65 mm. So in this reason I chose 600 steps, but it's very time wasting.
5. The Mooney-Rivlin model can be unstable depending on your material coefficients, load case and total range of deformation. I believe it may be good up to 200% but can still become unstable under your load condition.Not this model but close design simulated with MSC Software Adams and Simulation solved successfully. In this project, my aims are obtain more pressure loading and more bending without error. The link shows you an example which I would like to reach.

[kurtoglu_33]

Hi there,

I couldn't reached any solution yet. Could you help me on my problem? Thank you!

[Cotral.RD2]

I just had a look at your simulation setup. I consider that your coefficients are verified and correct for MR model.

I reduced the number of iterations to 20 and noticed that your model suffers from self collision. I am not sure if Fusion 360 has this capacity to detect self collision during the simulations. I personally dont think but i may be wrong. This may explain why the simulations work on other dedicated CAE softwares. 

A solution might be to cut the model into differnt repetetive bits and create them as different components. Then apply initial contact surfaces. I see your fins are spaced at around 1.7mm so either create the contacts manually or apply an auto method. I would also refine the mesh at highly strained areas.

I cannot test this hypthesis as it costs me valuable credits 😛

Let me know if this works. and if it does do not forget to accept hte solution or like it 🙂

[Anonymous]

Sorry for the delayed response, I have been incredibly busy with my "day job" lately.

@Cotral.RD2 is correct in that this type of simulation doesnt allow for self contact. Event simulations do, but that probably wont be an optimum solver. I think his recommendation may be a good idea as far as making this an assembly, but I've never tried to fake a self contact that way so I cant tell you.

If you can get it to work in MSC, why not use that? This is a very Niche simulation that may be pushing what is reasonable in F360.

[kurtoglu_33]

Hello again,

I am still stuck in same error.  Now, I simplified my simulation problem. Could anyone help me about this " Max Number of Bisections permitted reached ERROR". 

I have 6 Simulation Studies which I want to explain my basic problem. I would like to solve Nonlinear Simulation using Custom Material(Thermoplastic Polyurethane). It's same with my previous problem. And I have a simply question about that? Why Fusion 360 could not solve my Same Study while I am changing Mesh size?

I attached the F3d file, you could solve again to answer my problem. 

Thanks for Helping!

[kurtoglu_33]

Hello,

As you said, it's not preffered solution type Event Simulation. Now, I simplfy mt problem, I wrote a comment for you. Could you check up on? Thank you so much your help!

Now, we could not use MSC and I have to initially solve the problem with F360.

[kurtoglu_33]

Hello again,

I still have a problem, could anyone help me ? Thank you!

[John_Holtz]

Hi @kurtoglu_33

You asked "Why Fusion 360 could not solve my Same Study while I am changing Mesh size?" Unfortunately, that is how math works. Each element approximates the behavior of the real world. The accuracy of the approximation depends on the shape of the element, and the shape if dependent on the element size. At some sizes/shape, the math allows it to converge. At other sizes/shape, the mathematical approximations cause the beam to twist or something, and it is not able to converge.

For the thin cantilever beam under extreme bending, you ideally want 2 or more elements through the thickness. Since the thickness is 1.5 mm, that would imply a mesh size of 0.75 mm.

Since the material model is set to Hyperelastic, it should not be using the basic material properties like Young's Modulus, Poisson's Ratio, and Shear Modulus. But I see that those values are not realistic (the Poisson's ratio must be less than 0.5, and Shear Modulus is determined from the Youngs Modulus and Poisson's ratio and cannot be larger than the Youngs modulus.) In the unlikely event that the basic properties are affecting the analysis, I would suggest entering realistic values.

One last question: how did you get the Mooney Rivlin constants? How confident are you that they are correct? I am getting singularity warnings which do not make sense unless the mesh is completely distorted (which it should not be distorted; I am using 2 mm mesh size) or the material properties are an issue.