Learning Forum

[Alejandro Filgueira]

Hi!

I need to model a polymer (polypropylene) to perfom with it non-linear simulations (impact test, high deformation load status, etc...). The only information I have available to model the behaviour of this polypropylene is:

• Tensile Modulus: 1.100MPa
• Tensile Strain at Yield: 11 %
• Tensile Stress at Yield: 29 MPa

For the tests I need to consider both the elastic and the plastic behaviours of the plastic, because high deformations are expected.

Do you have any suggestion of what model should I use in Ansys Workbench and what specific values should I use for this modellization? 

 

Thanks

 

[Ashish Khemka]

Hi,

Please see if the following post helps you:

Material model for Polypropylene for impact simulation of box? (ansys.com)

Regards,

Ashish Khemka

[Alejandro Filgueira]

Hi Ashish,

I read that post but didn't give me enough information. 

To begin with, I would need to be able to perform basic static tests with the plastic. So I am not sure Explicit Materials are the answer for this. I would need the way to describe an elastic behaviour with different parts: a linear part at the beginning and another area with a decrease in the slope of the stress-strain curve up to the 29MPa. How could I achieve this using Ansys Workbench?

 

 

Thanks

 

Alejandro

 

[Armin_A]

Hi Alejandro,

It looks like that you need a multi-linear elasticity model for your application. As far as I know, this model is not available via Workbench but it may be accessible via Mechanical APDL (MAPDL) commands. Please refer to the thread below where a similar topic was discussed:

Errors with Multilinear Elasticity material model (ansys.com)

[Alejandro Filgueira]

Thanks Armin.

I was able to phisically test the plastic and get a strain-stress curve. Is there any way in Workbench to model a material by entering these stain-stress points? As far as I have investigated I just have seen this possibiliy in the hyperelastic materials. Is there any other altenative?  

[Armin_A]

Hi Alejandro,

Do you see the bilinear elastic behavior in your experiment? If not, you can simply use a plasticity model within Ansys Workbench such as the "Multilinear Isotropic Hardening" to directly input the stress versus plastic strain curve into the model. Once you open Engineering Data, this model is available under "Plasticity" under the Toolbox. 

[Alejandro Filgueira]

Thanks Armin. But if I have raw strain-stress values in a chart, how can I separate the values that I have to input in the "Multilinear Isotropic Hardening" model? In this model the strain you have to input is the plastic strain, not the elastic one, right?

[Claudio Pedrazzi]

Couldn't you simply subtract from each total (raw, measured) strain value the elastic strain, corresponding to yielding stress divided by E?

e_plast=e_tot - Sy/E

[Armin_A]

Hi Alejandro,

What you obtained experimentally is likely engineering stress versus engineering strain curve. You should convert it to true stress versus true plastic strain before providing it to the model.

Please note that your resulting hardening curve should only be increasing with plastic strain, i.e., if your experimental data is noisy, an error message may appear when you solve the model. In such a case, it might be a good practice to fit a mathematical function (such as power-law or Voce functions) to your data so that it becomes smooth with true stress only increasing by plastic strain.