General Mechanical

General Mechanical

visco-elastic behavior modeling

    • jonsys
      Subscriber

      I am trying to model a laminated glass consisting of 2 panes and PVB interlayer in-between. The interlayer has a viscoelastic behavior and I have the experimental results. I have already defined the Shear Modulus (time and temperature dependent) [Fig 1]. 


      But this is not enough because the model cannot be solved due to the error in Fig 2. To make it work, despite Shear modulus, I should define either Young's modulus or Poisson's ratio. But I don't know which Properties from the Toolbox should I chose to use in order to correctly describe visco-elastic behavior.


      Any suggestions?


      definition of shear data for the viscoelastic behavior


      Elasticity required

    • peteroznewman
      Subscriber

      Hi Jon,


      Add Isotropic Elasticity and enter a value for Young's Modulus and Poisson's Ratio.


      Regards,


      Peter

    • Sandeep Medikonda
      Ansys Employee

      Hi Jon,


        Peter has already answered your question, but in the context of this question, I wanted to share an interesting article on modeling visco-elastic materials in ANSYS for any one else who might be interested.


      ~Sandeep

    • jonsys
      Subscriber

      Hello Peter,


      thank you for the reply.


      Inserting Isotropic Elasticity is exactly the reason why I had to seek for help here. Since I defined the shear modulus on "Shear Data - Viscoelastic", it means that now I only need to define the Poisson's Ratio because Elastic moduli (E) will change by how the shear modulus (G) changes. However, at "Isotropic Elasticity" it is mandatory to put Poisson's ratio and E (or G) [Fig 3] 1) If I defined G once why should I do it again?


      However, additionally to "Shear-Data Viscoelastic" I have also tried to define E and Poisson's ratio at "Isotropic Elasticity" as you suggested as well. With this two problems arise:
      I) If I increase the loading by 10, the displacement will be increased by 10 as well, typical for isotropic behavior. And this makes me think that viscoelasticity is not being considered
      II) I remove the data at "Shear Data - Viscoelastic" and I get the same results as when the data was there. Still, this means that they are not being taken into consideration


      Regards,


      Jon


       


      isotropic material parameters

    • jonsys
      Subscriber

      Hello Sandeep,


      thank you for the reply. 


      I have already checked that file but it presents such a general overview on implementing viscoelastic behavior in ANSYS. And my problem is more specific; you can also look at the above reply I just did to Peter.


      Regards,


      Jon

    • peteroznewman
      Subscriber

      Hi Jon,



      I) If I increase the loading by 10, the displacement will be increased by 10 as well, typical for isotropic behavior. And this makes me think that viscoelasticity is not being considered



      Viscoelasticity has time as a variable in the computation of displacement, while elasticity is the instantaneous response. If you simulate 100 seconds when load=1, and you compare the displacement results at 100 seconds with the load=10, you should not have a ratio of 10 at t=100 due to the exponential behavior of the viscoelastic material.


      Please create a Workbench Project Archive .wbpz file and attach it to your post above so I can take a detailed look at your data. Note there is a file size limit of 120 MB.


      Regards,


      Peter

    • peteroznewman
      Subscriber

      Hi Jon,


      I recently learned how to do a Creep Analysis in ANSYS and one of the requirements was to turn on Creep Effects in the Static Structural analysis. Maybe that is what you need to do for your viscoelastic model.


      Regards,


      Peter

    • Bhargava Sista
      Ansys Employee

      Jonsys,


      I'll give you a brief overview of viscoelasticity so it'll answer your questions: viscoelastic bevahior has a viscous (time-dependent) component acting upon the elastic (time independent) component. The elastic component can either linear (linear elasticity) or nonlinear elastic (hyperelastic). The viscous component is usually modelled using Prony series which uses the normalized shear moduli and the characteristic time constants (they come in pairs) as the material properties.


      When you input viscoelastic shear data, you'll need to perform curve fitting to calculate the Prony series constants to complete the definition. After you do that, you get the normalized shear moduli and their corresponding time constants. Since the moduli are normalized you still need to define an elastic component for the viscous component to act upon.


      In the example model that you showed above, when the isotropic elasticity is not defined the material had no stiffness behavior associated with it which is why it threw the error. When you defined isotropic elasticity properties and defined 'shear data - viscoelasticity', the Prony constants are missing as you haven't performed curve-fitting yet so there is no viscous behavior associated with it.


      I hope that clears up some of your questions.

    • Bhargava Sista
      Ansys Employee

      Hi Peteroznewman,


      You don't need to turn on the creep effects (in fact you don't get that option under Analysis settings) for viscoelasticity. It is used only for the other creep laws.

    • jonsys
      Subscriber

      Bsista,


      thank you very much for your clear explanation and help.


      For one example I have Prony Shear Relaxation parameters, therefore I implemented the way that you said and everything works well for a certain temperature.


      1) But for other examples I do not have Prony series parameters, therefore, I should do the curve fitting as you suggested but what option should be used for curve fitting? I could not manage to do that.



      2) I want to see the behavior of the material while the temperature is changing, therefore I can define the Isotropic Elasticity behavior dependant on temperature [Fig 4]. But I don't know how to get output dependant on temperature; Is there anything that I should add at the Analysis Settings? Do you have any suggestions?


       


      Fig 4

    • jonsys
      Subscriber

      Hi Peter,


      I think that the answer from bsista solved the problem, but thank you for the readiness to help.


      Regards

    • Bhargava Sista
      Ansys Employee

      Jonsys,


      Happy to help!


      Regarding your questions


      1) You should have the stress relaxation data (stress vs time) that you input under 'Shear data-viscoelastic'. After you input the data, select Prony Shear Relaxation under Viscoelastic. This should place a Curve-fitting object since the data is available. When you right-click on Curve-fitting you should get an option to solve curve fit. You'll need to pick the number of terms under Prony shear relaxation, this is a trial and error approach so start with 1 term and increase them only if you're unable to find a good fit. This step can be tricky as you're dealing with nonlinear regression based optimization. You'll need to change the initial seed values to improve the quality of curve-fit. This involves a bit of learning curve so I'd recommend that you spend some time.


      2) If you have defined temperature dependent Young's modulus and apply a thermal load in Mechanical, the change in temperature must change the material stiffness accordingly and this should reflect in your results. You don't need to turn anything ON/OFF under Analysis settings.

    • jonsys
      Subscriber

      Bsista,


      thank you!


      1) While I did some searching and implementation based on your suggestions which are very helpful, the upcoming questions arise:


      i) Is it enough to check the curve fitting only visually on the Chart (Chart of Properties Row)?
      ii) Increasing the term will improve the solution, but what might be other disadvantages rather than computational power?
      iii) What does scale and offset represent [Fig 1] and what does a seed value mean?


      I know this might be too much questions to answer, so even if you suggest me some resources to read it would be enough.


      2) You mean like this (Thermal Condition) [Fig 2]? Is that the same as if I input "Environment Temperature" under "Static Structural" [Fig 3]?


      Fig 1
      fig 1 scale offset


       


      Fig 2


      fig 2


      Fig 3
      fig 3

    • peteroznewman
      Subscriber

      Jon,


      I'm interested to learn about visco-elastic materials in this discussion, but I will add what I understand about figures 2 and 3.


      Environment temperature is the starting temperature of all the bodies. If you apply a Thermal Condition like temperature to one or more bodies, the temperature will be ramped from the starting Environment temperature to the value set in the Thermal Condition.  


      Say you had one body with a hole and another body with shaft in that hole, and the diameters are equal. If you define contact between the shaft and hole faces, and the coefficient of thermal expansion of the shaft material is greater than the material with the hole, then you can solve for the stress caused by the expansion of the shaft in the hole by applying a Thermal Condition that increases the temperature by 8 degrees C.


      If you changed the environment temperature to 122 degrees C and the Thermal Condition to 130 degrees C, the diameters of the hole and shaft would start out as equal but you could see a different stress if the materials have temperature dependent properties as the temperature increases by 8 degrees C from that higher starting temperature.


      Regards,


      Peter

    • Bhargava Sista
      Ansys Employee

      Jonsys,


      I think Peter already answered your second question so let me take the first one:


      Ideally, you would want to look at quantities such as error residue to judge the quality of fit but for most practical purposes visual inspection works just fine.


      Regarding the number of terms, the more the merrier does not work here. Adding more terms make the model more nonlinear which is the reason why it's easier to find a better fit. However, this also increases the tendency for the model to be unstable (stress decreases with increasing strain - negative stiffness). This can result in element distortion errors. Rule of thumb is to increase the number of terms only when a lower order model is unable to capture the response.


      I'm not sure how exactly the offset and scale terms work but the suggestion is to not use them (leave the defaults).


      Regarding references, I'd recommend reading about viscoelasticity in the ANSYS help documentation (Material reference and theory reference). Other references include some texts such as Applied Mechanics of Solids by Allan Bower, Nonlinear Solid Mechanics: A Continuum Approach for Engineering by Gerard Holzapfel.


      Good luck!

    • jonsys
      Subscriber

      Bsista and Peter,


      I want to thank you for your answers throughout this constructive discussion. They were very helpful.


       


      Regards,


      Jon

    • masud407
      Subscriber

      Hey Jon,


       


      Can you please exactly tell me what data that I need to insert to simulate viscoelastic properties in ANSYS workbench?

    • masud407
      Subscriber

      Hello Bsista,


       


      Can you please explain me a little bit about the process of curve-fitting? Do I need to put the isotrophic elasticity properties along with prony shear relaxation and shear data viscoelastic data?Thanks in advance.

    • peteroznewman
      Subscriber

      Masud,


      Please start a New Discussion. This topic is marked as solved.


      Regards,
      Peter

    • masud407
      Subscriber

      Peter,


       


      Thanks for your reply. I have already created a new discussion. Here is the link:


       


      https://forum.ansys.com/forums/topic/adding-visco-elastic-properties-in-ansys-workbench/


      Regards,


      Masud

Viewing 19 reply threads
  • You must be logged in to reply to this topic.