# modelling truss in ANSYS

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

• You should give some more details on exactly which part is giving you trouble, so that anyone who answers can give you a specific answer rather than just a broad description of how to do trusses in ANSYS. See the how to ask help page for more info on asking good questions. Mar 3, 2017 at 20:06
• @BarbalatsDilemma I updated my question. thanks for suggestion Mar 3, 2017 at 23:22

! 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