I'm modeling an RC Beam with ANSYS Workbench 18.2, following a tutorial that uses ANSYS Workbench 2019.
However, the option "link/truss" is missing from the values of "Model Type" when I select the rebars.
Dear Serag,
You can use this command it works the same.
ET,MATID,LINK180
MPDATA,EX,MATID,,2.1e5
MPDATA,PRXY,MATID,,0.3
TB,BISO,MATID,1,2
TBDATA,,500,0
R,MATID,10,,0
The first line defines the rebar to link 180.
The second line defines the modulus of elasticity.
Thethird line is Poisson’s ratio of steel.
The Fourth line yield strength.
The fifth line is the radius of the bar.
Best regards.
Thanks Almoutaz Bellah Alsamawi
1) I've removed this version and installed ANSYS 19.2, the option is there under the name "link".
2) In ANSYS Workbench it's easy to define cross sections, and materials, except for some concrete parameters for CONCRETE65 element type [this is from my understanding from the tutorial I'm currently following]
This is the link for it:
https://www.youtube.com/watch?v=Sg7jmuD7GiY&list=PLYX5ua4SRf6zibnuG3WM43gLJkUVBUgkx
Serag Hassouna
There are some parameters that need to be defined manually as:
1 Shear transfer coefficients for an open crack.
2 Shear transfer coefficients for a closed crack.
3 Uniaxial tensile cracking stress.
4 Uniaxial crushing stress (positive).
5 Biaxial crushing stress (positive).
6 Ambient hydrostatic stress state for use with constants 7 and 8.
7 Biaxial crushing stress (positive) under the ambient hydrostatic stress state (constant 6).
8 Uniaxial crushing stress (positive) under the ambient hydrostatic stress state (constant 6).
9 Stiffness multiplier for cracked tensile condition, used if KEYOPT(7) = 1 (defaults to 0.6).
I talked about it in the published work:
https://www.researchgate.net/publication/357478646_Numerical_Parametric_Study_of_Fully_Encased_Composite_Columns_Subjected_to_Cyclic_Loading
You can take a look for more explanations.
Best of luck.
Almoutaz Bellah Alsamawi
Would you mind sharing how to define concrete's stress-strain relation in ANSYS, as well as these other parameters?
To be honest, I'm mainly using Mechanical APDL, at which I can provide the values only for the positive part of the relation.
Negative strains are refused, hence, the tensile side of action is not incorporated properly in the model I'm working on.
I'm modeling an experiment of combined torsion and flexure, when I provide the compressive side of the relation I receive tiny displacements far far away from the reported experimental results.
Try this commend
ET,MATID,SOLID65
R,MATID,0,0,0,0,0,0
RMORE,0,0,0,0,0
MP,EX,MATID,29250
MP,PRXY,MATID,0.2
TB,CONCR,MATID,1,9
TBTEMP,22
TBDATA,0.3,1,0.8,3,30
TB,MISO,MATID,1,30,0
TBTEMP,22
TBPT,,0.0001,2.925
TBPT,,0.0002,5.7
TBPT,,0.0003,8.325
TBPT,,0.0004,10.8
TBPT,,0.0005,13.125
TBPT,,0.0006,15.3
TBPT,,0.0007,17.325
TBPT,,0.0008,19.2
TBPT,,0.0009,20.925
TBPT,,0.001,22.5
TBPT,,0.0011,23.925
TBPT,,0.0012,25.2
TBPT,,0.0013,26.325
TBPT,,0.0014,27.3
TBPT,,0.0015,28.125
TBPT,,0.0016,28.8
TBPT,,0.0017,29.325
TBPT,,0.0018,29.7
TBPT,,0.0019,29.925
TBPT,,0.002,30
TBPT,,0.0021,30
TBPT,,0.0022,30
TBPT,,0.0023,30
TBPT,,0.0024,30
TBPT,,0.0025,30
TBPT,,0.0026,30
TBPT,,0.0027,30
TBPT,,0.0028,30
TBPT,,0.0029,30
TBPT,,0.003,30
TBPT,,0.0031,30
TBPT,,0.0032,30
TBPT,,0.0033,30
TBPT,,0.0034,30
TBPT,,0.0035,30
yield strength is 30 MPa
Best of luck
- Badges
- Science topic