Learning Forum

[lincs2k9]

I have tried to apply (TB, ANISO) command in Ansys workbench. It doesn't work. Always shows the below error message. 

I added the below command snippet in the geometry section. I added tensile yield stress with a corresponding tangent modulus of x,y & z direction. Can anyone help me to find out where I made a mistake?

[Wenlong]

Hi,

TB does not have an "ANISO" material model name. You need to use a valid material model name defined here: https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v201/en/ans_cmd/Hlp_C_TB.html?q=tb

Hills yield surface allows you to define an anisotropic yield surface, but it won't let you define anisotropic tangent modulus. Please check this page for your desired material model. https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v201/en/ans_mat/amp8sq21dldm.html%23matRIPisohillyield. Below is an example of how to use TB, Hills

Regards,

Wenlong

 

 

[lincs2k9]

Hello Wenlong,

Thank you for your reply. You said that TB does not have an "ANISO" material model name. But in Ansys help section there have mentioned this material model-

https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v194/ans_arch/anisotropicopt.html?q=TB,%20ANISO

https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v194/ans_arch/old_TB_HILL.html

[lincs2k9]

Actually I have an orthotropic material with different nonlinear stress-strain curves in fiber (X-direction) & transverse (Y/Z-direction) direction. I need bilinear or multilinear hardening material model for orthotropic material (Just like 'Bilinear isotropic hardening'/'multilinear isotropic hardening'). But those are for isotropic material. I need those for orthotropic material as I have to define the stress-strain curve in different directions in different temperatures. How can I do that?

[peteroznewman]

Consider using ACP Pre/Post to define fiber directions and fiber properties that are highly anisotropic, while the matrix that holds the fibers remains isotropic. ACP Pre/Post is used to build up a Composite Fiber material consisting of one or more layers whose fibers can run in one or more directions. The overall properties of the layup then emerge.

[lincs2k9]

Hello Peter,

Good to hear from you! Thank you for your reply.

Actually my composite material consists of unidirectional fiber and epoxy adhesive. I used the 'RVE' method to obtain homogeneous material properties of my mentioned composite. I obtained directional young's modulus, poisson's ratio & shear modulus. I want to use this data to create a new material (just like what material designer section in Ansys does) for further analysis. But compared to other composite material, my composite material is shown bilinear stress-strain curve at high temperature. So, I have to define plasticity material properties as well as my obtained elastic properties. That's why I want to know how can I define the stress-strain curve in different directions in different temperatures?

 

[Wenlong]

Hi,

Oh, I see, so TB, ANISO is an archived material model. While the features in this archive remain available for use, better alternatives are available and recommended in most cases. So it is recommended to use newer technologies. 

As for the negative yield stress, it does seem odd to me too. Let me investigate more and get back to you.

Regards,

Wenlong

 

 

 

[lincs2k9]

Hello Wenlong
Thank you for giving your time.
As I have mentioned earlier that I have to define plasticity material properties/ stress-strain properties in different direction in different temperature, so is there any other option except (TB, ANISO) in Ansys workbench?

[Wenlong]

Hi,

I find out the reason: you need to define data for the compressive and shear part as well. It works for me now. 

Regards,

Wenlong

 

[lincs2k9]

Thank you for giving your time. I have also checked that issue. Problem was that I defined only tensile yield stress and tangent modulus.
Another question is-
In your previous reply you said that it is recommended to use newer technologies. Is there any new alternative in Ansys except TB, ANISO?
I asked that because I found that TB,ANISO doesn’t support temperature dependent material property. But I have to add various direction yield stress, tangent modulus based on different temperature.

[Wenlong]

There is Hills anisotropic yield criterion, however, I am not aware of an anisotropic hardening model. The available material combination can be found here: https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v201/en/ans_mat/elemamoco050301.html?q=anisotropic%20plasticity, you can see from that page that all the available hardening law is either isotropic or kinematic.

Regards,

Wenlong