Using ANSYS Simple truss problem

Using ANSYS - Simple truss problem

Objective: To prepare a text file defining the ANSYS FEM model for the simple truss problem shown below and to then use ANSYS to find the solution for displacements and stresses in this truss.

Note: with ANSYS Release 13 link1 has been replaced with link180.

truss1.bmp (127638 bytes)

1. Use Notepad to prepare a text file that contains the information shown below. Save the file as 'truss1.txt'.

/FILNAM,truss
/title, Simple Truss

/prep7

n, 1, 25.0,  0.0, 0.0    ! Node 1 is located at (25.0, 0.0, 0.0)
n, 2,  0.0, 18.0, 0.0
n, 3,  0.0,  0.0, 0.0

et, 1, link180             ! Element type; no.1 is link180

sectype, 1, link           ! Type of cross section is link

secdata, 0.5               ! Cross sectional area = 0.5 sq in

mp, ex, 1, 3.e7          ! Material Properties, E for material no. 1 
mp, prxy, 1, 0.3         ! & poisson's ratio for material no.1

en, 1, 3, 1              ! Element Number 1 connects nodes 3 & 1
en, 2, 2, 1

d, 3, ux, 0.             ! Displacement at node 3 in x-dir is zero
d, 3, uy, 0.             ! Displacement at node 3 in y-dir is zero
d, 2, ux, 0.
d, 2, uy, 0.

f, 1, fy, -1000.         ! Force at node 1 in y-direction is -1000.

finish

/solu                    ! Select static load solution
antype, static
solve
save
finish

/post1                   ! Use 'ssum' to compute sums interactively
etable, Stress, ls, 1    ! Create a table of element stress values
etable, Volume, volum    ! Create a table of element volumes

2. Start ANSYS and Select File > Working Directory set the directory for your work.

3. Select File -> Read Input From (locate and select the file truss1.txt that you prepared)

Once the solution has been computed,

4. Plot -> Elements

5. PlotCtls -> Numbering -> Node numbers ON, Element numbers ON

6. PlotCtls -> Symbols -> Applied B.C.'s

7. General Postprocessor -> Plot Results -> Deformed Shape -> Def. + Undef.

truss1o.bmp (141702 bytes)

(Use PlotCtrls > Hard Copy > To Printer (or To File) to print or save your plots)

8. General Postproc > Read Results > First Set

9. List -> Results -> Nodal Solution -> DOF Solution

10. General Postproc > List Results > Element Solution > Line Element Results > Element Results > OK

11. List -> Results -> Element Table Data -> Stress, Volume

12. For additional Plot manipulation: PlotCtls -> Pan, Zoom, Rotate

Back