Set multi model for one hyper-elastic material?

[SM1994]

I am trying to model a hyperelastic material in Abaqus, but after evaluating the material properties, it seems that the Neo_H model is appropriate until 50% strain, and then Ogden-1 is suitable.
How can I set in the Abaqus that it uses Neo-H until 50% strain and then switch to Ogden?
Thanks

 

[FEA way]

It's not possible to change material models during analysis. However you could run new analysis with Ogden model using deformed mesh and stresses imported from previous simulation (the one with Neo-Hookean model) as initial conditions.

 

[SM1994]

Thanks for your response.
I am not sure if I have understand what you mean, would you please elaborate on that?
do you mean that I first let the simulation finishes using Neo-H and then build another simulation on than with Ogden? how can I do such a thing? I will get twice deformed surface,don`t I?
Thanks

 

[FEA way]

First simulation (with Neo-Hookean model) should be completed up to the point when this model stops giving good results. Then you can import deformed mesh from this analysis to new one (with Ogden model). Add stresses from the end of previous simulation as initial stresses (Predefined Field --> Step: Initial --> Mechanical --> Stress). Continue loading the model in new analysis. This is basically import capability (see the chapter "About transferring results between Abaqus analyses" in Abaqus documentation) but without importing material state.

 

[IceBreakerSours]

Do you trust the experimentalist and the test data you have?

*********************************************************
Are you new to this forum? If so, please read these FAQs:

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[SM1994]

Thank you all for your responses.
Yes, I am pretty sure about the data

 

[IceBreakerSours]

Which hyperelastic material was tested? Have you tried higher order Ogden or other material models? Have you looked at published literature to see if someone has already characterized the material?

*********************************************************
Are you new to this forum? If so, please read these FAQs:

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[SM1994]

It is Ecoflex 50 manufactured by Smooth on.
I tried all model with different orders. Ogden with order more than one, will be unstable for my material.
I looked at the literature, but I could not find anything appropriate, but I will do it again.

 

[IceBreakerSours]

Out of curiosity: What sort of physical test was performed? I am asking because some tests can be tricky to simulate. In such cases, there are small (unavoidable) discrepancies between the physical test and the model which can cause divergence in the behaviors.

*********************************************************
Are you new to this forum? If so, please read these FAQs:

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[SM1994]

I only had access to the uniaxial testing machine.
I wish I could get some biaxial, but I do not have access to such a machine to do that.

 

[IceBreakerSours]

Are you trying to do an inverse FEA or a fundamental material characterization? In the former case, you mesh the geometry of the actual specimen whereas in the latter case you use the analytical equations or a single element/integration point to identify the constants for a given material.

*********************************************************
Are you new to this forum? If so, please read these FAQs:

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[SM1994]

I am doing inverse FEA
I know the actual displacement, but I want to get the displacement using FEA as well.
I found some models in the literature in which the coefficient had been expressed, but it did not work for my case.
Cheers

 

[IceBreakerSours]

I would try the fundamental characterization route first (simply because there are far fewer sources of uncertainty). There is a feature in Abaqus/CAE that identifies constants for you from test data (I have not used CAE in a while so I don't remember exactly how to access it). Of course, a key assumption is that the test data is imported appropriately. Unless there is something unique about this material, I bet this route will work out fine. In fact, I can't imagine why it wouldn't.

*********************************************************
Are you new to this forum? If so, please read these FAQs:

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[FEA way]

Indeed, Abaqus offers a feature named Material Calibration. To use it double click Calibrations in the Model Tree. Then expand the Calibration-1 and double click Data Sets. Import data set (your test data) and confirm. Then double click Behaviors and choose "Hyperelasticity with Permanent Set". In Uniaxial tab select previously created Data Set and click the "Extract uniaxial data sets" button. Pick yield point from viewport. Finally, click Create Material button and then Ok to create new empty material. Choose it as Material in Edit Behavior window.

 

[SM1994]

Thank you for the hint
I did it, but I got the error saying I do not have enough data to do the calibration, I am not sure if it is talking about the number of the data or quality of them? since I have got about 600 data.
PS: I could not figure out what exactly is this calibration doing? or supposed to do?

 

[FEA way]

This feature extracts the parameters for plastic (permanent set) and hyperelastic material behavior with Mullins effect from imported experimental data. Your test data may not be sufficient to define all these behaviors.

 

[SM1994]

For the hyperelastic, Abaqus has an inbuilt material model evaluation, in which it indicates what model is stable for the input data set and apparently is more accurate and more robust than the calibration method, but I am not sure if this is my case and causing the problem.
I have used that and found out the Ogden N=1 and NH is appropriate for my model

 

[IceBreakerSours]

Excellent. There can be many reasons why the inverse FEA method was not working well; hard to say without digging into the details. Read a reference article/book chapter about it and that should give you some ideas. Simulia's social community or learning hub (or, whatever the heck it is called!) has good resources available as well.

Now, although you have characterized the material and estimated/identified the constants for the chosen material model, keep in mind that the characterization process assumes the material was under a simple tension (in this particular case). If, for some reason, that was not the case, then significant errors will creep into the analysis. If you are thinking: "What could go with a uniaxial tensile test?", think again

*********************************************************
Are you new to this forum? If so, please read these FAQs:

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083