You may use ANSYS Composite Pre/Post (ACP). You can define your failure criterion in this module. 

Hi Mohammaed,

there are many failure criterias in ANSYS like Hashin's, Max. stress, Max. strain, etc. You can use these inbuilt criterias directly. It is available in ANSYS 15.0. but if you have older version than you have to use the stress-strain data stored in postprocessing for failure criterias. You need to write then APDL codes for that. 

Thank you dears for your attention and helpful answers

I am using ANSYS 14.0, in which failure criteria can be dealt with in tow ways:

1- In the Preprocessor

Preprocessor>material proprieties>Material models>Nonlinear>Inelastic>Non-metal plasticity>Failure Criteria

2- In the postprocessor

General postprocessor>Failure criteria>Add/Edit

In the tow ways I can attach the input data with material type used for CFRP (solid185), but the problem is that failure criteria in both cases is not working while analyzing the problem by ANSYS, and changing values of input data will not affect the results (specially the failure load of the strengthened reinforced concrete beam and maximum deflection), as if ANSYS is not using the input failure criteria in preprocessing stage.

My question here is:

How exactly I can input the stress and strain limits for CFRP used to externally strengthen the concrete beam which is incrementally loaded in a way that will determine the failure load of CFRP and then the failure load of the RC beam.

Regards

in ansys 14.0 and 15.0, the failure criteria for composite can be defined in APDL via the commands (TB, DMGI) and TBDATA, check out in ansys command reference and material reference for more details 

For older version of ANSYS, like ANSYS 14, you will need to write an APDL code and input it the ansys command for the failure criteria. You can use TBDATA and

TB, DMGI and

FCTYP, ADD, EMAX, SMAX, TWSI, TWSR

The FCTYP command modifies the list of active failure criteria.

By default, active failure criteria include EMAX, SMAX, TWSI, and TWSR.

The command affects any subsequent postprocessing listing and plotting commands (such as PRESOL, PRNSOL, PLESOL, PLNSOL, and ETABLE).

A single FCTYP command allows up to six failure-criteria labels. If needed, reissue the command to activate or remove additional failure-criteria types.

=======================================================

FCTYP, Oper, Lab Activates or removes failure-criteria types for postprocessing.

POST1: Failure CriteriaCompatible Products: – | – | Premium | Enterprise | Ent PP | Ent Solver | DYNA

Oper

Operation key:

ADD

 — 

Activate failure-criteria types. This option is the default behavior.

DELE

 — 

Remove failure-criteria types.

Lab

Valid failure-criteria labels. If ALL, select all available (including user-defined) failure criteria.

EMAX

 — 

Maximum strain criterion (default)

SMAX

 — 

Maximum stress criterion (default)

TWSI

 — 

Tsai-Wu strength index (default)

TWSR

 — 

Inverse of Tsai-Wu strength ratio index (default)

HFIB

 — 

Hashin fiber failure criterion

HMAT

 — 

Hashin matrix failure criterion

PFIB

 — 

Puck fiber failure criterion

PMAT

 — 

Puck inter-fiber (matrix) failure criterion

L3FB

 — 

LaRc03 fiber failure criterion

L3MT

 — 

LaRc03 matrix failure criterion

L4FB

 — 

LaRc04 fiber failure criterion

L4MT

 — 

LaRc04 matrix failure criterion

USR1 through USR9

 — 

User-defined failure criteria

===================================================

In newer versions, you can create files like the Failure.xml

Layer Int All 1,1000000 1 Display DropDown All Elemental,Nodal Elemental Inverse DropDown All Yes,No Yes %DAUSERFILES%\SolveFailure.py %DAUSERFILES%\EvaluateFailure.py 1 0 Layer Dependant Failure Maximum strain 101,100 Layer Dependant Failure Maximum stress 101,100 Layer Dependant Failure Tsai-Wu strength index 101,100,102 Layer Dependant Failure Inverse of Tsai-Wu strength ratio index 101,100,102 Layer Dependant Failure Hashin fiber failure 101,100,102 Layer Dependant Failure Hashin matrix failure 101,100,102 Layer Dependant Failure Puck fiber failure 101,100,102 Layer Dependant Failure Puck inter-fiber (matrix) failure 101,100,102 Layer Dependant Failure LaRc03 fiber failure 101,100,102 Layer Dependant Failure LaRc03 matrix failure 101,100,102 Layer Dependant Failure LaRc04 fiber failure 101,100,102 Layer Dependant Failure LaRc04 matrix failure 101,100,102 Maximum Failure Criteria Layer Elemental Maximum Failure Criteria Failure Criteria Elemental Maximum Failure Criteria Value 102 Elemental

As I understood, you are looking for putting limits on stress or strain. From the ANSYS Mechanical APDL Material Reference, you can read:

"Material strength limits represent maximum stresses or strains that a material can sustain. This data table defines the strength limits and other related constants required for computing failure criteria (FC) index of a material under various loading conditions. Specify a TBOPT value on the TB,FCLI command to correspond to the stress limits (TBOPT = 1) or strain limits (TBOPT = 2)."

Or another option can be using the FC command. To specify a failure criterion, use the family of FC commands. These FC commands can be used for any 2-D or 3-D structural solid element or any 3-D structural shell element: FC, FCDELE, and FCLIST. A typical sequence of commands to specify a failure criterion using these commands follows:

FC,1,TEMP,, 100, 200 ! Temperatures

FC,1,S,XTEN, 1500, 1200 ! Maximum stress components

FC,1,S,YTEN, 400, 500

FC,1,S,ZTEN,10000, 8000

FC,1,S,XY , 200, 200

FC,1,S,YZ ,10000, 8000

FC,1,S,XZ ,10000, 8000

FCLIST, ,100 ! List status of Failure Criteria at 100.0 degrees

FCLIST, ,150 ! List status of Failure Criteria at 150.0 degrees

FCLIST, ,200 ! List status of Failure Criteria at 200.0 degrees

PRNSOL,S,FAIL ! Use Failure Criteria