Learning Forum

[ihsanbuetk1995]

Hello everyone,

I am modeling a tensile test of a surgical staple joining two pieces of artificial skin in ANSYS Workbench 2024 R2.

Experimental setup:

• 100 N load cell
• Crosshead speed: 0.333 mm/s
• Tensile loading until failure

Since the loading rate is slow, should I use Static Structural or Transient Structural analysis or explicit? Also, can failure (skin tearing or staple pull-out) be captured in Static Structural, or do I need a damage/cohesive zone model?

Any suggestions or relevant tutorials would be greatly appreciated.

Thank you.

[peteroznewman]

Static Structural is the preferred analysis. Transient Structural is unnecessary because the velocity is so low that inertia forces the transient analysis adds to the static analysis are all practically zero.

If you want to see skin tearing or staple pull-out, you will need a material damage model or cohesive zone model. These models can solve in Static Structural right up to the point of separation.

What experimental material testing data do you have for the artificial skin?

[ihsanbuetk1995]

I am using true stress-strain data converted from the engineering stress-strain data obtained from our experiments. I performed curve fitting using the Mooney-Rivlin hyperelastic model; however, the simulation results do not agree well with the experimental data. Could anyone suggest possible reasons for this discrepancy or recommend a more suitable material model?

Thank you.

[ihsanbuetk1995]

[ihsanbuetk1995]

here is materail properties carve fitting i getting from experimenatl

[peteroznewman]

Hyperelastic material models are elastic which means when you remove the load, the material returns to the initial shape.

When fitting hyperelastic coefficients to experimental data, it is vital that only data in the elastic range is included.

The experimental data you show looks like it includes the damage portion of the tensile test, where the material was taken beyond the elastic range and into the plastic or damaged range.

Because you fit invalid data to the hyperelastic material model, your simulation results will have significant deviation from experimental data.

Another mistake you made is using True Stress and Strain in the hyperelastic experimental data.  You must use Engineering Stress and Strain for the experimental data when fitting the coefficients in the Hyperelastic material models.

You can have a Viscoplasticity material model that includes the elastic portion of the material response and a rate-dependent material model for the plastic portion of the material response.

https://ansyshelp.ansys.com/public/account/secured?returnurl=/Views/Secured/corp/v261/en/ans_mat/rate.html

Many materials exhibit stress relaxation over time when held at a fixed amount of displacement or exhibit creep behavior when held at a fixed stress level which manifests as strain continuing to increase over time.  There are material models to represent this viscoelastic behavior.

https://ansyshelp.ansys.com/public/account/secured?returnurl=/Views/Secured/corp/v261/en/ans_thry/thy_mat6.html

A material can have more than one model to represent different behaviors. For example you can have both the Hyperelastic model and the PRONY model for viscoelasticity.