0
$\begingroup$

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 enter image description here

$\endgroup$
2
  • $\begingroup$ 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. $\endgroup$ – BarbalatsDilemma Mar 3 '17 at 20:06
  • $\begingroup$ @BarbalatsDilemma I updated my question. thanks for suggestion $\endgroup$ – SAndroid Mar 3 '17 at 23:22
1
$\begingroup$

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

$\endgroup$
3
  • $\begingroup$ How about providing an example? $\endgroup$ – Mahendra Gunawardena Aug 29 '19 at 11:04
  • 1
    $\begingroup$ @Mahendra Gunawardena I added an example. Enter in the ANSYS mechanical program and type these commands in the command line of the GUI. Or create a text file, put the these commands inside of it, change the extension to .mac and run it as macro $\endgroup$ – Victor Verga Aug 29 '19 at 14:58
  • $\begingroup$ Thank you for updating the response. $\endgroup$ – Mahendra Gunawardena Aug 29 '19 at 23:59

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.