Hello,
I am currently working with PPM 1.3.5.1 and trying first steps with non-linear materials. Here I simulate a simple cylinder made of rubber, which I compress axially.
Now to my question:
Has anyone tried something similar with rubber? Is there a stress-strain curve that works with PPM?
Furthermore I try instead of a force to give up a displacement, unfortunately I have not found out yet.
I must say that the handling of PPM is very intuitive and you have a steep learning curve.
Hello @wlh70. Last year I did some simple research in non-linear behavior using PrePoMax successfully. Rubber is somewhat different since it is a hyperelastic material, and proper material definition must be done. In this post in the CalculiX forum there is an excellent discussion about hyperelastic modeling. You can define it using the keyword editor in PrePoMax and the appropriate coefficients for the material you are using.
In my experience, it is easier to achieve convergence using imposed displacement than forces.
I attach a .gif of my simple model using copper wire with plasticity behavior last year.
Rubbers normally require hyperelastic material models. Ideally, the data for them should be taken from physical tests - there are tools that can be used to derive coefficients of various hyperelastic models from stress-strain curves obtained during experiments. But in many cases, testing is not an option and then you can use research papers with data for rubber of a similar kind. Another way would be to derive the coefficients from consistency with linear elasticity but that works only for the basic neo-Hookean model.
1 Like
First of all, thank you very much for your answers. I need to dig into the subject a little more and will come back with my example.
Now I have understood this with the Calculix Key Word Editor and can describe my hyperelastic materials. For this I used Mooney-Rivlin C10 and C01 coefficients, where I know that these also work in other FEM programs and lead to relavitively correct results. But now I have the problem that when I apply a displacement the stresses fit but not the forces. If I apply a force, the displacements are not correct. If I calculate this analytically, then the force should be approx. factor 10 larger. Where do I make the mistake? The coefficients for Mooney are given in MPa.
Cylinder_D36_H36_70SHA_C10-0-93_C01-0-23_Compression.pmx (338.0 KB)
1 Like
What equation are you using for that analytical solution ?
Unfortunetly in German
Federdaten brechnen von Gummielementen in verschiedenen Ausführungen (schweizer-fn.de)
Here’s what I got in Abaqus from the uniaxial test evaluation of Mooney-Rivlin model with those constants:
Are you sure that your formulas account for hyperelasticity ? It seems that it’s not mentioned there. They also require some different inputs.
You’re right. Hyperelasticity is not taken into account in the Excel calculations. I am actually only interested in the real stiffness curve, which I want to calculate using FEA, based on the Mooney coefficients.
Here would be my excel sheet with the Mooney values
I can see two different C01 on the sequence of posts.
C01=.23 (Excel file)
C01=.28 (prepomax Keyword editor)
¿Which is the good one?
Okay, it was a mistake. C01 = 0,23. Approx C01 = C10/4
But the real problem is that the calculated forces do not fit and I do not know why?
I would really appreciate a solution.
I’m really excited about PrePoMax at the moment and will continue to dig into it.
With the ones calculated analytically ? But that solution doesn’t take hyperelasticity into account.
No, let’s forget about the analytical Excel results and just focus on the Mooney values and my model. Maybe I don’t understand the whole thing yet, because I’m not a FEA specialist and I’m learning the whole thing autodidactically. I come here from the product development of rubber-metal components and would like to master the FEM itself for future designs. Maybe too high a goal, but I would like to at least try. I also know that you have to put a lot of time and knowledge into it and I also know all the pitfalls of FEM. For example, when it comes to stiffness in all six spatial directions, then it fits very well here and there to measurement results, but not for all.
Hyperelasticity very new to me too.
This problem has some interesting and challenging BC. Looking at your deformed view and mesh I’m not sure if you are capturing properly what’s going on in the corner.
I have found that with such a soft material, some wall elements could exceed the height of the base.
I have enforced a larger displacement for you to see what I’m talking about.
Corner fixed :
¿Have you confirmed that the reaction force agrees with the applied force?. This is a highly recommended if not mandatory check on FEM.
I would start with a single element test and displacement control. That’s usually the best way to understand the behavior of advanced material models in FEA. Examples like that are included in Abaqus documentation (Verification Guide).
1 Like
If I apply a displacement of 8mm I’m obtaining a reaction force of 2.550,16 N.
If I apply a force of 2550N I’m obtaining a displacement of -7.9991mm
Did you consider some symmetry? You probably have some wrong value. Are you apling the load as a force, as pressure, to a face or a set of nodes?.
Then I am reassured that you will get the correct result calculated. It is interesting that I got exactly 2500N with my analytical estimation.
Then the error will lie with my inputs, but I do not know where I made the mistake.
Can you share your model?
What formula did you use for that ?
Your material is nearly incompressible (D1=0 means full incompressibility but CalculiX doesn’t support this and thus adds some compressibility so that Poisson’s ratio is 0.475). This may cause volumetric locking when hybrid elements are not used. Unfortunately, they are not supported in CalculiX. I would try with a material having more compressibility first.
I think that was more of a coincidence than an analytical formula.
Here I just used the simple formulas with geometry, Young’s modulus and stiffness to calculate the force backwards. The whole is rather a very very simple approach.
