Learning Forum

[Andreyteston]

Hello, members!

I have been trying to implement the Menetry-Wiilian material model with Exponential Softening behavior on Mechanical APDL. In order to implement this material model is necessary to define seven constants, that I am going to explicit here:

[Ashish Khemka]

nnPlease refer to the link below:nnnRegards,nAshish Khemkan

[Andreyteston]

Hello, Ashish Khemka!nThank you for share this link. I would like to use his contribution to my model. On the other hand, I haven't one customer portal account because I use one license at the University of Passo Fundo/BR.nI wonder if you could share the content of this link otherwise possible.nThanks in advancenn

[ErKo]

nThis might be due to the TBDATA command posted (takes only 6 values in one line - see TBDATA command in the help manual) .nnAn example on how it can be used (so split the TBDATA in two, one having values say from 1-5 and 6 - 7 in separate TBDATA command):n---n---nEc=43.2E3nmatid=2nMP,EX,matid,Ec nMP,NUXY,matid,0.15nnn! MW concrete nRc=67.5 ! uniaxial compressive strengthnRt=3.48 ! uniaxial tensile strengthnRb=80 ! biaxial compressive strengthnnpsi=15nnTB,CONCR,matid,,,MWnTBDATA,1,Rc,Rt,RbnnTB,CONCR,matid,,,DILAnTBDATA,1,psinnOci=0.33 ! relative stress level at start of hardeningnOcu=0.85 ! relative stress level at ku (mlaw=1)nOcr=0.1 ! residual relative stress levelnkcm=0.0020-Rc/Ec ! plastic strain at uni-axial compressive strengthnkcu=0.0035-Ocu*Rc/Ec ! plastic strain defining start of exponential softening lawnnnOtr=0.1 ! residual relative stress level in tensionnGft=0.09 ! area specific fracture energynntb,CONCR,matid,,,HSD2nTBDATA, 1, kcm, kcu, Oci, Ocu, OcrnTBDATA, 6, Gft, Otrn----n----nnIn our mew versions (2020 R2) we do not need to use commands, we can set the material in eng. data, which is nice inside workbench.nnAlso the reinforcements (REINF264) make the workflow of embedding re-bars in concrete very easy saving lots of trouble in modelling RC structure and is now fully available in WB mechanical.

[to2020]

nI hope you are well. I am using the newer versions of ANSYS and I have found the options to input the values in engineering data. nThe following are the values I have inputted for Non-Linear Concrete. nHowever, when I try to run the program, I keep getting error about how an element is failing. I am modelling the following pull-out test and using symmetry to only analyse half of it:I have also used contact sizing and therefore the mesh for concrete near the rebar as well as the rebar has been set to 1mm (This is the smallest I could go for a 150mm diameter concrete cylinder with a height of 170mm on the Academic Version of Ansys). nI have applied the following analysis settings, boundary conditions and loading (force is corresponding to the yield strength of the bar i.e. 541MPa but only half of the load is applied due to symmetry): nnI currently haven't defined a bilinear hardening model for steel as I was having errors running it when I defined it. But since I am only applying the load until yield strength, wouldn't specifying the yield strength be sufficient because it is still linear? nI am also giving link to the model if anyone is kind enough to look through any errors.https://unsw-my.sharepoint.com/:u:/g/personal/z5117866_ad_unsw_edu_au/EbxuvuDD7nBNl0403Sd8AtUBx4S1D9tSU63vP2W9WiJn3g?e=9vZgWDnThank you so much! n