Objective: To prepare a text file defining the ANSYS FEM model for the elementary truss problem shown below and use ANSYS to solve for natural frequencies and modes.
1. Prepare a text file containing the following information. The 1000 lbf load is not needed.
/FILNAM,truss /title, Simple Truss
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, link1 ! Element type; no.1 is link1
!Beginning with ANSYS Release 13 link1 has been replaced with link180
mp, ex, 1, 3.e7 ! Material Properties, E for material no. 1 mp, prxy, 1, 0.3 ! poisson's ratio for material no.1 mp, dens, 1, 0.736e-3 ! mass density for material no. 1
r, 1, 0.5 ! 'Real Constant' number 1 is 0.5 ! (Cross sectional area) en, 1, 3, 1 ! Element Number 1 connects nodes 1& 2 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.
2. Start ANSYS and select 'Run Interactive' Select the Working Directory
3. Select File > Read Input From (locate and select the file truss.txt that you prepared)
4. Solution > Analysis Type > New Analysis > Modal > OK
5. Analysis Options > Block Lanczos
No. of Modes to Extract 2
Expand mode shapes yes
NMODE No. modes to expand 2
Normalize mode shapes To mass matrix
6. Solve > Current LS > OK
7. General Postprocessor > Results Summary (Shows frequencies calculated.)
8. Read Results > First Set
9. Plot Results > Deformed Shape > Def. + Undef.
The first mode of vibration is shown in the figure below.
(Use PlotCtrls > CaptureImage to print or save your plots. Can also use Animate to visualize motion.)
To list the nodal deformation values for the mode use
List Results > Nodal Solution > DOF solution > All DOFs DOF
10. For the next mode: Read Results > Next Set
11. Plot Results > Deformed Shape > Def. + Undef. etc.
Last update 5-2-03