You may try to use the command TB to define a data table for material properties.

I use the Multilinear Isotropic Hardening Model to define a stress-strain curve.

Check the following links for more information.

https://www.sharcnet.ca/Software/Ansys/16.2.3/en-us/help/ans_cmd/Hlp_C_TB.html

https://www.sharcnet.ca/Software/Ansys/16.2.3/en-us/help/ans_mat/amp8sq21dldm.html#miso

Hi,

I have used TB commands in identifying material properties(stress and strain) for steel structures, as below. I hope you can get hint to apply it for concrete structures too.

TBTEMP,,STRAIN

TBDATA,,0.001724,0.0149,0.0253,0.0556,0.131,0.16

TBTEMP,0

TBDATA,,344700000,350000000,382200000,449200000,506200000,508400000

Dear Sir,

You can easily insert curves for concrete using Drucker-Prager concrete model.

For instance:

/prep7

! ELASTIC CONSTANTS

MP,EX,1,20.0E9

MP,NUXY,1,0.2 ! Base Drucker-Prager concrete Rc=30.0E6 ! uniaxial compressive strength

Rt=3.0E6 ! uniaxial tensile strength

Rb=36.0E6 ! biaxial compressive strength delta_t=0.25 ! dilatancy factor tension

delta_c=1.0 ! dilatancy factor compression ! COMPRESSION

kappa_cm=0.0025-Rc/20.0E9

kappa_cr=0.0025

omega_ci=0.33

omega_cr=0.1

!TENSION

kappa_tr=0.0005

omega_tr=0.2 TB,CONCR,1,,,DP

TBDATA,1,Rc,Rt,Rb TB,CONCR,1,,,DILA

TBDATA,1,delta_t,delta_c TB,CONCR,1,,,HSD6

TBDATA,1,kappa_cm,kappa_cr,omega_ci,omega_cr,kappa_tr,omega_tr

This model has good convergence rate and agreement with experimental results.

https://www.sharcnet.ca/Software/Ansys/17.0/en-us/help/ans_mat/mat_geomechanics.html