modelling truss in ANSYS

Question

I want to model an ideal truss in ANSYS 16.1 and by ideal I mean all of the joints are pinned joints and so the momentum can not be transferred at joints(like attached image). The problem is that I don't know how to model the pin joints for the truss structure. I would be appreciated if some body can help me by providing solutions or ideas. Cheers

Answer 1

To create a pinned jointed truss structure you only need to define the points, which corresponds to the joints, and connect them using using lines that will be meshed with trusses elements. By definition, the truss elements have pinned joints, so you do not have to worry about modelling each of the defined joints.

Example

! 2D Truss Analysis ! /title, Truss ! /PREP7 ! preprocessor phase ! ! ! define keypoints ! K,1, 0, 0 ! keypoint, #, x, y K,2, 50, 100 K,3, 100, 0 K,4, 150, 100 K,5, 200, 0 K,6, 250, 100 K,7, 300, 0 ! ! define lines connecting kps ! L,1,2 L,1,3 L,2,3 L,2,4 L,3,4 L,3,5 L,4,5 L,4,6 L,5,6 L,5,7 L,6,7 ! ! element definition ! ET,1,LINK1 ! truss element, type 1 R,1,100 ! real constant 1 ! Cross sectiona area: 100 mm^2 ! MP,EX,1,200e3 ! material property 1 ! Young's modulus: 200 GPa ! LESIZE,ALL, , ,1,1,1 ! specify divisions on unmeshed lines LMESH,all ! mesh all lines ! FINISH ! finish pre-processor ! /SOLU ! enter solution phase ! ! Apply constraints at kps ! DK,1,ALL,0 ! define a DOF constraint at a keypoint DK,7,UY,0 ! ! Apply loads ! FK,1,FY,-100e3 ! define a force load to a keypoint FK,3,FY,-100e3 FK,5,FY,-100e3 FK,7,FY,-100e3 ! SOLVE ! solve the resulting system of equations FINISH ! finish solution-phase ! ! Enter postprocessor-phase ! /POST1 PRRSOL,F ! List Reaction Forces PLDISP,2 ! Plot Deformed shape PLNSOL,U,SUM,0,1 ! Contour Plot of deflection ETABLE,SAXL,LS, 1 ! Axial Stress PRETAB,SAXL ! List Element Table PLETAB,SAXL,NOAV ! Plot Axial Stress