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
-
$\begingroup$ 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. $\endgroup$– BarbalatsDilemmaMar 3, 2017 at 20:06
-
$\begingroup$ @BarbalatsDilemma I updated my question. thanks for suggestion $\endgroup$– SAndroidMar 3, 2017 at 23:22
1 Answer
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
-
$\begingroup$ How about providing an example? $\endgroup$ Aug 29, 2019 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 $\endgroup$– OmgAug 29, 2019 at 14:58
-
$\begingroup$ Thank you for updating the response. $\endgroup$ Aug 29, 2019 at 23:59