Structural modal analysis - 2D frame

Transcription

1 Structural modal analysis - 2D frame Determine the first six vibration characteristics, namely natural frequencies and mode shapes, of a structure depicted in Fig. 1, when Young s modulus= 27e9Pa, Poisson s ratio = 0.2, density 2500kg/m^3, and L= 6m, W= 4m, H= 4m. The frame consists of horizontal beams with the cross-sectional area 0.3m*0.6m, where 0.6m is the height of the beams, and lower vertical beams (depicted in green colour) with the crosssectional area 0.4m*0.8m, where 0.8m is the height, and upper vertical beams (depicted in red colour) with the crosssectional area 0.4m*0.6m, with 0.6m height. Use the element type BEAM3. Fig. 1: Geometry of the computational domain for the modal analysis. 1. Select the type of the discipline ANSYS Main Menu > Preferences. We select Structural and click OK.

2 2. Define the type of element ANSYS Main Menu > Preprocessor > Element Type > Add/Edit/Delete. We click Add button, highlight Structural Mass Beam, then 2D elastic 3, press OK and close the Element Types window. (Comment: If this element cannot be found in the GUI menu, type et,1,3 in the command line.) 3. Setting the real constants Since our structure consists of three different sets of beams, we have to define three sets of real constants. ANSYS Main Menu > Preprocessor > Real Constants > Add/Edit/Delete. We click Add button, then OK. In the Crosssectional area AREA we type 0.3*0.6, in Area Moment of Inertia IZZ we enter 0.3*0.6**3/12 and in Total beam height HEIGHT 0.6. We press OK. Afterwards in the Real Constants window we click Add, then OK and enter Real constants for the second set: Cross-sectional area AREA: 0.4*0.8 Area Moment of Inertia IZZ: 0.4*0.8**3/12 Total beam height HEIGHT: 0.8 In the same way we define the third set of real constants: Cross-sectional area AREA: 0.4*0.6 Area Moment of Inertia IZZ: 0.4*0.6**3/12 Total beam height HEIGHT: 0.6. Now your Real Constants window should look like Fig. 2. To close it, we click the Close button.

3 Fig. 2: Real Constants window with three sets defined. The same can be done in CLI by typing R,1,0.3*0.6,0.3*0.6**3/12,0.6 R,2,0.4*0.8,0.4*0.8**3/12,0.8 R,3,0.4*0.6,0.4*0.6**3/12,0.6 in the command line. 4. Define element material properties ANSYS Main Menu > Preprocessor > Material Props > Material Models. We click Structural > Linear > Elastic > Isotropic and in the window that appears, we enter Young s modulus EX: 27e9 and Poisson s ratio PRXY: 0.2. We press OK and close the window. ANSYS Main Menu > Preprocessor > Material Props > Material Models. We click Structural > Density and enter density Dens: 2500, press OK and close the window. 5. Define the geometry We will start with four bottom keypoints:

4 Fig. 3: Create KPs on WP window. ANSYS Main Menu > Preprocessor > Modelling > Create > Keypoints > On Working Plane where we enter the 0,0 (see Fig. 3), press Apply. In the same way we define keypoint with coordinates 6,0 press Apply, then with coordinates 10,0 press Apply, and the last bottom keypoint with coordinates 16,0 and press OK. The same can be done by typing K,1,0,0 K,2,6,0 K,3,10,0 K,4,16,0 in the command line. Now we will generate keypoints on each floor: ANSYS Main Menu > Preprocessor > Modelling > Copy > Keypoints. We click Pick All, and in the following window enter 10 in ITIME Number of copies including original, and 4 in DY Y-offset in active CS. Click OK. In CLI we use the KGEN command and type

5 KGEN,10,ALL,,,,4,,,0 In the next step, we will define lines. Again, also the GUI and mouse can be used, but we will use the *do and L command. To create vertical lines we type *do,i,1,4,1 *do,j,i,33+i,4 L,j,j+4 and to create horizontal lines *do,i,5,37,4 *do,j,i,2+i L,j,j+1 6. Assigning real constants and meshing of the computational domain We start by selecting the horizontal lines (their numbers are in the range of 37 and 63) using the LSEL command. Then we assign attributes by the LATT command, set number of divisions to be 10 by the LESIZE command and finally mesh lines by LMESH. LSEL,s,,,37,63 LATT,1,1,1 LESIZE,all,,,10,,,,,1

6 LMESH,all Now we select all vertical lines by inverting our previous selection using the LSEL,inve command. Since we have two different kinds of vertical beams, we select (for example) the upper beams, see Fig.1, first. LSEL,inve *do,i,1,28,9 *do,j,i,i+4 LSEL,u,,,j Then we assign real constants to them by the LATT command, set number of divisions to be 1 by the LESIZE command and mesh lines by the LMESH command. LATT,1,3,1 LESIZE,all,,,1,,,,,1 LMESH,all Finally we select the bottom beams LSEL,none *do,i,1,28,9 *do,j,i,i+4 LSEL,a,,,j

7 and in the same way we assign attributes and mesh them. In the end we select all lines by the LSEL,all command. LATT,1,2,1 LESIZE,all,,,1,,,,,1 LMESH,all LSEL,all 7. Applying loads The only loads valid in a typical modal analysis are zerovalue displacement constraints. If you specify any nonzero displacement constrain, ANSYS will assign a zero-value constraint to the degree of freedom instead. Also other loads can be specified, but ANSYS will ignore them. If you do not specify constraints, ANSYS will calculate rigid body modes (zero frequency). ANSYS Main Menu > Preprocessor > Loads > Define Loads > Apply > Structural > Displacement > On Keypoints. We pick four bottom keypoints and set ALL DOF = 0. The same can be done by using the DK command. DK,1,,,,0,ALL DK,2,,,,0,ALL DK,3,,,,0,ALL DK,4,,,,0,ALL 8. Setting the type of analysis and running solution ANSYS Main Menu > Solution > Analysis type > New Analysis. We tick Modal and click OK. ANSYS Main Menu > Solution > Analysis type > Analysis Options. In [MODOPT] Mode extraction method we choose Block Lanczos. It

8 is a generally recommended method for large symmetric eigenvalues problems that uses the sparse matrix solver. In No. of modes to extract we specify the number of modes we want to extract, i.e. 6. The [NMODE] No. of modes to expand is usually the same as the number of extracted modes, i.e. 6 (see Fig.4). We press OK.. Fig. 4: The Modal Analysis window. In the following window we type 100 in FREQE End Frequency and click OK. At this point, we have told ANSYS to find a particular quantity of modes and to look within a particular frequency range. If ANSYS finds that quantity before it finishes the frequency range, it will stop the search. If ANSYS does not find that quantity before finishing the frequency range, then it will stop the search. ANSYS Main Menu > Solution > Solve > Current LS > OK. Then we close message windows. The list of commands for setting the type and options of modal analysis, and running the solution is /SOLU ANTYPE,2 MODOPT,LANB,6

9 MXPAND,6,,,0 MODOPT,LANB,6,0,100,,OFF solve 9. Listing and visualization of results Natural frequencies: We can use ANSYS Main Menu > General Postproc > Results Summary or we can type SET,LIST. A list with six frequencies, see Fig.5, will pop up. Note that each mode is stored in a separate substep. Fig. 5: The Results Summary with natural frequencies. Modes: We turn on displaying the shape of elements using Utility menu > PlotCtrls > Style > Size and Shape and in [/SHAPE] Display of element we click ON. Then we read results for a first substep by ANSYS Main Menu > General Postproc > First Set. We plot deflection by ANSYS Main Menu > General Postproc > Plot Results > Contour Plot > Nodal Solu and in Nodal Solution > DOF solution we highlight Displacement vector sum and click OK. Your ANSYS Graphics window should look similar to the first plot of the Fig.6. We observe that the value of the maximum deflection is DMX= and the value of the first frequency is FREQ= Then we plot deformed geometry through ANSYS Main Menu > General Postproc > Plot Results > Deformed Shape and in KUND Items to be plotted we select Def + undef edge. We click OK. Now your ANSYS Graphics window should

10 look similar to first plot of the Fig. 7. Again we observe the value of the first frequency and maximum deflection. Fig. 6: Modes and corresponding natural frequencies deflections. To see the deformed geometry for the second substep, we read results for the second substep by ANSYS Main Menu > General Postproc > Next Set and we repeat the procedure. Another way to read result is to use ANSYS Main Menu >

11 General Postproc > By Pick where we highlight the desired set and click Read button. Fig. 7: Modes and corresponding natural frequencies deformations.

12 Structural Static Analysis - Warren deck truss bridge Find the deflection of each node, when FY = -200KN is applied on the KP = 20, L= 6m, H= 8m and bridge consists of I-beams where W1 = 0.6m, W2 = 0.6m, W3 = 0.8m, t1= 0.2m, t2 = 0.2m, t3 = 0.2m. Fig. 1: Geometry of the computational domain with illustration of boundary conditions. 1. Select the type of the discipline ANSYS Main Menu > Preferences > Structural > OK 2. Define the type of element ANSYS Main Menu > Preprocessor > Element Type > Add/Edit/Delete > Add > Select Beam, 2 node 188 > OK > Close (Comment: BEAM188 is a linear (2-node) beam element in 3D with six degrees of freedom at each node: translations in X, Y and Z directions, and rotations about the X, Y and Z directions.) 3. Define element material properties ANSYS Main Menu > Preprocessor > Material Props > Material Models > Structural >

13 Linear > Elastic > Isotropic In the window that appears, enter the following geometric properties for steel: Young s modulus EX: 210e9 and Poisson s Ratio PRXY: 0.3. Press OK and close window. 4. Define the cross section details ANSYS Main Menu > Preprocessor > Sections > Beam > Common Sections In the window that appears, choose I-beam as a Sub-Type and type W1 = 0.6, W2 = 0.6, W3 = 0.8, t1= 0.2, t2 = 0.2, t3 = 0.2 Press OK. 5.Create keypoints Utility Menu > Parameters > Scalar Parameters In Selection line type L = 6, press Accept, and then H = 8 and Accept. Close window. Now we can define keypoints by using parameters L and H according to Fig1. You can use GUI: ANSYS Main Menu > Preprocessor > Modeling > Create >Keypoints> In Active CS. use CLI: K, keypointnumber,x,y No X 0 L 2*L 3*L 4*L 5*L 6*L 7*L 8*L 9*L 10*L 11*L 12*L Y No X 0 L 2*L 3*L 4*L 5*L 6*L 7*L 8*L 9*L 10*L 11*L 12*L

14 Y H H H H H H H H H H H H H generate them by using KGEN command: First we create keypoint 1 and 14 by K,1,0,0 K,14,0,H and then we generate all other points in both rows by KGEN,13,1,,,L KGEN,13,14,,,L where number 13 denotes that we want to generate 13 keypoints, that are equally distributed from point 1 (and 14) in the L distance in X direction. 6.Create lines You can create lines again by GUI:

15 ANSYS Main Menu > Preprocessor > Modeling > Create > Lines > Lines > Straight Line CLI: L, KP1, KP2 where KP1 and KP2 are keypoints that define line, namely L,14,2 L,2,16 L,16,4 L,4,18 L,18,6 L,6,20 L,20,8 L,8,22 L,22,10 L,10,24 L,24,12 L,12,26 L,14,15 L,15,16 L,16,17 L,17,18 L,18,19 L,19,20 L,20,21 L,21,22 L,22,23 L,23,24 L,24,25 L,25,26 L,1,2 L,2,3 L,3,4 L,4,5 L,5,6 L,6,7 L,7,8 L,8,9 L,9,10 L,10,11 L,11,12 L,12,13 L,1,14 L,2,15 L,3,16 L,4,17 L,5,18 L,6,19 L,7,20 L,8,21 L,9,22 L,10,23 L,11,24 L,12,25 L,13,26 we can use *do with L command to create lower horizontal lines: *do,i,1,12 L,i,i+1

16 to create upper horizontal lines: *do,i,14,25 L,i,i+1

17 to create vertical lines: *do,i,1,13 L,i,i+13

18 to create lines inclined the left: *do,i,2,12,2 L,i,i+14

19 to create lines inclined the right: *do,i,2,12,2 L,i,i+12

20 7. Meshing of the computational domain ANSYS Main Menu > Preprocessor > Meshing > Mesh Tool In Size Controls section of Mesh Tool choose Lines and click SET. Then press Pick All, and in the following table for NDIV (No. of element divisions) write 1. Press OK. Finally, in Mesh check whether Lines option is chosen, press Mesh button and then Pick all button. Now all lines should be meshed. To check meshing, go to Utility Menu > Plot > Elements and plot elements. 8. Prescribing boundary conditions ANSYS Main Menu > Preprocessor > Loads > Define Loads > Apply > Structural > Displacement > On Keypoints Click KP1, press OK, and for DOFs to be constrained choose All DOF, and for VALUE Displacement value write 0. Press Apply.

21 Then click KP13, press OK, and for DOFs to be constrained choose UY (check that All DOF is not selected), and for VALUE Displacement value write 0. Press Apply. ANSYS Main Menu > Preprocessor > Loads > Define Loads > Apply > Structural > Force/Moment > On Keypoints Click point in the middle of the upper row, press OK, and the following window for Lab Direction of force/mom choose FY and for VALUE Force/moment value write Press OK. 9. Running solution ANSYS Main Menu > Solution > Solve > Current LS > OK 10. Visualization of results ANSYS Main Menu > General Postproc > Plot Results > Deformed

22 Shape > choose Def + undeformed and click OK ANSYS Main Menu > General Postproc > List Results > Nodal solution > choose Displacement vector sum and click OK

23 PRINT U NODAL SOLUTION PER NODE ***** POST1 NODAL DEGREE OF FREEDOM LISTING ***** LOAD STEP= 1 SUBSTEP= 1 TIME= LOAD CASE= 0 THE FOLLOWING DEGREE OF FREEDOM RESULTS ARE IN THE GLOBAL COORDINATE SYSTEM NODE UX UY UZ USUM E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E-04 MAXIMUM ABSOLUTE VALUES NODE VALUE E E E-03

24 Utility menu > PlotCtrls > Style > Size and Shape In [/SHAPE] Display of element click ON ANSYS Main Menu > General Postproc > Plot Results > Contour Plot > Nodal Solu > Stress > von Mises stress press OK