Hi

Which shape of structures .

I assume you are trying to input the cross section area of the link through Real Constant. Similar to the case of BEAM188 and BEAM189, providing the cross section area for these elements is done using Section Type and Section Data. Links for more information are:

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

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

I believe you need to pick LINK as the parameter for SECTYPE command. With SECD command, you only give the area. For example, for a 1 m2  cross section you'd do this:

SECT,1,LINK    !---Define a link section type with associated number 1

SECD,1            !---Give a value of 1 for area

...

SECN,1           !---Choose section 1 before meshing

LMESH,   !---Mesh lines with Section 1

Thank you so much. I try to model the bonded force between concrete and steel in ansys. 

I want to use 3 elements: solid 65 (for concrete), link 180 ( for steel) and  combin 39 (for bond ). In ansys 18, Solid 65 and combin 39 were inputed data by using Real constant (make the number Real constants for solid 65  and combin 39) and Link 180 can not make real constants. Before meshing, we have to  input Meshing Attributes, including 3 conditions: material, real constants, and  Element type number. Solid 65 and Combin 39 have 3 conditions, whereas link 180  does not have Real constants . ->can not mesh....Please let  me know how can I solve this problem

You're correct about the mesh prerequisites, As with solving the Real Constant issue for Link180, I think I was clear that this element doesn't take Real Constants and instead you need to use Section which I explained earlier.

To move forward, i need to know why "can not mesh". What is the error message?

Example: solid 65 (real constants 1), Combin 39 (real constant 2), link 180 ( with out real constants)

When I set Meshing Attributes for link 180: real constant was required that I have to choose 1 or 2

you can see this problem on the picture

I just tried a very simple example. This is a single link with 0.01 m2 areaand 1 m long that is fixed at one end and a 1kN force in x direction is applied to the other end. The purpose is to see if it would mesh and solve with what I explained above. This worked for me.

FINI

/CLEAR

/PREP7

ET,1,180

R,1

MP,EX,1,2E11

MP,PRXY,1,.3

SECT,1,LINK

SECD,0.01,0.5

K,1,0,0

K,2,1,0

L,1,2,10

TYPE,1

REAL,1

MAT, 1

SECN,1

LMESH,1

D,NODE(0,0,0),ALL,0

F,NODE(1,0,0),FX,1000

FINI

/SOLU

ANTYPE,STATIC

SOLVE

FINI

/POST1

PLNSOL,U,X

I hope this helps!

From what i see in the figure, you are not selecting the correct SECNUM for the link. Take a look at the piece of APDL script I just wrote.

I try to solve with your command, it announce the error because in ansys 18 link 180 can not input realconstant number

Oh, sorry, there is a typo in the code. Change the SECN,0.01,0.5 with SECD,0.01,0.5 and it should work. I will edit my previous answer for future reference.

Hi friend, thank you so much. I can not set the number of Real constant using Preprocessor->Real constant-> set num ber. However I can set Real constant by command. it is ok

Hey friend. I have the same problem. Did you find a solution?

For link 180 element.

O, much thank you Ranjan Kumar .

So, after this restructured, how apply this to my geometry(to reinforcement bar)?

Non-linear Analysis of Shear Dominant Prestressed Concrete Beams using ANSYS

This study reports the details of the finite element analysis of eleven shear critical partially prestressed concrete T-beams having steel fibers over partial or full depth. Prestressed T-beams having a shear span to depth ratio of 2.65 and 1.59 that failed in shear have been analyzed using the ‘ANSYS’ program. The ‘ANSYS’ model accounts for the nonlinearity, such as, bond-slip of longitudinal reinforcement, postcracking tensile stiffness of the concrete, stress transfer across the cracked blocks of the concrete and load sustenance through the bridging action of steel fibers at crack interface. The concrete is modeled using ‘SOLID65’- eight-node brick element, which is capable of simulating the cracking and crushing behavior of brittle materials. The reinforcement such as deformed bars, prestressing wires and steel fibers have been modeled discretely using ‘LINK8’ – 3D spar element. The slip between the reinforcement (rebars, fibers) and the concrete has been modeled using a ‘COMBIN39’- nonlinear spring element connecting the nodes of the ‘LINK8’ element representing the reinforcement and nodes of the ‘SOLID65’ elements representing the concrete. The ‘ANSYS’ model correctly predicted the diagonal tension failure and shear compression failure of prestressed concrete beams observed in the experiment. The capability of the model to capture the critical crack regions, loads and deflections for various types of shear failures in prestressed concrete beam has been illustrated.

Mr. can you show full example apply create and modify reinforcement section? How its worked

Follow the table 3 and table 4 of it journal.

Following is typical sequence of commands for defining discrete reinforcing elements.

Directly copy and pest in APDL command.

Ranjan Kumar will you please guide me on how you model only one pre-stressing bar while you are using the symmetry option, the pic (prestressing in ansys.PNG) shows that the prestressing strand is toward end side not exactly on center(if you took half).

please clarify my views will be very thankfull

Atiq Ahmad Jan good day! What are practic significate you reseaerch?