Learning Forum

[Raphikk]

Hello,

I am studying the load distribution of a ceramic-matrix-composite bolted joint and wish to incorporate the bi-modulus relationship between the tensile stress and strain, specified by the initial modulus, matrix cracking stress, material stiffness reduction factor and ultimate stress. I would like to use this material model for the in plane stresses of the composite substrate (x,y here) and hence have a better prediction of the stress for given strain.

According to the Mechanical APDL Element reference the code to use is TB, ANISO with 18 constants defined by TBDATA, however, I don't know how do add this as an external APDL command in workbench.

Here is a screen shot from the manual

[John Doyle]

The commands below would be need to be put in a command object under the subject part in the Project Tree. One thing worth mentioning however, is that this is a legacy mat'l option that only works with older core element types. This law is only usable with elements: PLANE42, SOLID45, SOLID92, SOLID95, LINK1, PLANE2, LINK8, PIPE20, BEAM23, BEAM24, SHELL43, SHELL51, PIPE60, SOLID62, SOLID65, PLANE82, SHELL91, SHELL93, and SHELL143.  So in addition to defining the material properties, you need to also reassign the element type from the 18x series (used in WB-Mechanical) to an equivalent core element type. The ET command included below assumes you need solid95, but this might need to be modified depending on your application.nTB,ANISO,matidnTBDATA,1,C1,C2,C3,C4,C5,C6ttt!Tensile yield stresses in the material x, y, and z directions following by tangent modulinTBDATA,7,C7,C8,C9,C10,C11,C12tt!Compressive              nTBDATA,13,C13,C14,C15,C16,C17,C18 t!Shear               net,matid,95 !change element type to core.n

[Raphikk]

Hello jjdoyle, thanks a lot for your help on this! As you predicted, the command could not run without a modification of the element type. This will be very useful to my analysis of C/SiC bolted joint. nThanks againn