Structural static analysis dome

Transcription

1 Structural static analysis dome Calculate the maximum displacements of the dome depicted in Fig.1 and consisting of two types of beams with the crosssectional area: 0.08m*0.21m ( zig-zags ) and 0.07m*0.16m (circles) after applying load FZ = -0.5N. Given material properties are Young s modulus 210e9Pa, Poisson s ratio 0.2 and density 7850 kg/m^3. We will use the element type BEAM4 and we will directly create the finite-element model (i.e. nodes and elements). Fig.1: Computational domain. 1. Setting the element type, material properties and crosssectional areas We set the element type (command: ET, No., type), material properties (UIMP, material number, label,,,value) and real constants (i.e. cross-sectional areas) using commands R, AREA, IZZ, IYY, TKZ, TKY, THETA and RMORE, ISTRN, IXX, SHEARZ, SHEARY, SPIN, ADDMAS. /PREP7 *SET,qs_,-0.5! Setting loads

2 ET,1,4 the element type BEAM4! Setting UIMP,1,EX,,,210e9 properties: Young s modulus UIMP,1,DENS,,,7850 density! Material! Material properties: UIMP,1,NUXY,,,0.2 properties: Poisson s ratio! Material R,1,0.0168, , ,.21, *0.21! Beam: RMORE,, R,2,0.0112, , ,.16,0.07! Beam: 0.07*0.16 RMORE,, Creating nodes We will start with changing the coordinate system to the cylindrical one by CSYS, number of coordinate system. Then we create one node on every circle by N, number of node, X, Y, Z (for easier orientation, nodes on each circle start with a new hundred, see Fig.2). Then we modify Y-coordinate on every second circle by NMODIF, number of node, X, Y, Z, THXY, THYZ, THZX and finally we generate the rest of the nodes by NGEN, copies, increment, NODE1, NODE2, NODINCR, DX, DY, DZ.

3 Fig.2: Numbering of nodes. CSYS,1! Changing of CS to the cylindrical one N,501,1.2,0, 2.45! Creating of the node N,401,2.1,0, 2.3 N,301, 3.27,0,2 N,201, 4.3,0, 1.45 N,101, 5.25,0,0.8 N,1,6,0,0 NSEL,S,,,101,501,200, nodes: 101,301 and 501 NMODIF,ALL,,10! Selecting!

4 Modifying Y-coordinate NSEL,All NGEN,18,1,All,,,,20,,1 Generating the rest of nodes! NPLOT 3. Creating elements Now we will join nodes by elements using command E, staring node, ending node. We will use the *DO command, that is useful to write until *ENDDO as one in the command line. We will start with circles: TYPE,1! Setting the element type REAL,2! Setting the real constants *do,j,0,5 *do,i,1,17 E,i+(j*100),i+1+(j*100)

5 *enddo *enddo *do,i,0,5 E,18+(i*100),1+(i*100) *enddo Then we create zig-zags : REAL,1 *do,j,0,5,2 *do,i,2,18 E,i+99+(j*100),i+(j*100) E,i+(j*100),i+100+(j*100) *enddo *enddo *do,i,0,5,2 E,1+(i*100),101+(i*100)

6 E,1+(i*100),118+(i*100) *enddo *do,j,1,4,2 *do,i,1,17 E,i+100+(j*100),i+(j*100) E,i+(j*100),i+101+(j*100) *enddo *enddo *do,i,0,3,2 E,118+(i*100),201+(i*100) E,118+(i*100),218+(i*100) *enddo

7 /ESHAPE,1 shapes of elements EPLOT plot! Turning on! Element 4. Applying loads and running solution /SOLU NSEL,S,,,1,18,1 nodes on outer circle D,All,,,,,,UX,UY,UZ boundary conditions! Selecting! Defining NSEL,All ACEL,,,10 gravity! Defining F,All,FZ,qs_ load! Applying

8 SOLVE solution 5. Postprocessing /POST1 PLNSOL, U,SUM, 0,1.0 PLDISP,1! Running

9 Static and modal analysis Suspension bridge Do the static and modal analysis of the suspension bridge depicted in Fig.1, when the height of the main pylon is 28m and the distance between cables is 9m. X-coordinate of the first cable can be computed by (Length of the deck (number of cables-1)*distance between cables)/2. The cross-sectional area of all cables is 140mm^2. Material properties for concrete are Young s modulus 200e9Pa, Poisson s ratio 0.2 and density 1700 kg/m^3; and for steel Young s modulus 100e9Pa, Poisson s ratio 0.3 and density 6850 kg/m^3. In the static analysis we will apply the gravity load and then there will be -1m prestress prescribed on every cable. We will study the deformation of the roadway. In the modal analysis we will calculate the first 20 natural frequencies and mode shapes. We will use three types of elements: BEAM54, BEAM3 a LINK11.

10 com. When creating the geometry, we will use the *DO command, that is good to write until *ENDDO as one in the command line. Fig. 1: Computational domain. 1. Preprocessing: Input parameters XPylon=2.0 of the main pylon! Coordinates YPylon=-2.0 HPylon=28.0 pylon Deck=68.0 the deck N_cables=7 of cables X_DistCables=9 between cables! Height of the! Length of! The number! Distance X_FirstCable=(Deck-(N_cables-1)*X_DistCables)/2! Coor. of the 1^st cable XAnchor=-38.0 the anchor! Coordinates of

11 YAnchor=-3.0 A_cable= 140E-6 sectional area of the cables! The cross- 2. Creating of the keypoints and lines We will define keypoints (command: K, No. of keypoint, X,Y,Z) and lines (command: LSTR, No. of starting point, No. of end point) using input parameters. (com. To use these commands, one has to be in the Preprocessor of the Ansys Main Menu.) We start with deck: K,1,0,0,0 K,2,X_FirstCable,0,0 K,8,Deck-X_FirstCable KFILL,2,8 K,9,Deck,0,0 *DO,CABLE,1,8 LSTR,CABLE,CABLE+1 *ENDDO then we create pylon: K,10,XPylon,YPylon,0 K,11,XPylon,HPylon,0 LSTR,10,11 cables *DO,I,2,8

12 LSTR,11,I *ENDDO and anchor K,12,XAnchor,YAnchor,0 LSTR,11,12 3. Define the type of element ANSYS Main Menu > Preprocessor > Element Type > Add/Edit/Delete. We click Add and select: BEAM54, BEAM3 a LINK Define element material properties ANSYS Main Menu > Preprocessor > Material Props > Material Models. We select Structural > Linear > Elastic > Isotropic We enter material properties for concrete (deck): EX: 200e9, Poisson s ratio PRXY: 0.2 and density DENS: We click Material > New Model > OK and add new material. Then we enter material properties for the new model steel (cables): EX: 100e9, Poisson s ratio PRXY: 0.3 and density DENS: Setting the real constants (deck, pylon and cables) ANSYS Main Menu > Preprocessor > Real Constants > Add/Edit/Delete. We click Add, select BEAM54, then OK and enter AREA1: 6, IZ1: 6*0.9**3/12, HYT1: 0.5, HYB1: 0.4, press OK. Then we click again Add select BEAM3, press OK and enter: AREA: 6, IZZ: 1.5*4**3/12, HEIGHT: 4, press OK. To set the real constants for cables we will use the command line:

13 *GET,E_OCEL,EX,2 steel! Reading of EX for *DO,IL,10,17 all cables! Cycle for *GET,LL,LINE,IL,LENG of the cable! Reading the length R,IL,A_CABLE*(IL-8)*E_OCEL/LL for cables! Setting the real constants *ENDDO cycle 6. A s s i g n i n g! End of the real constants and meshing of the computational domain We start with deck: MAT,1 Selecting of the material! REAL,1 of the real constants! Selecting TYPE,1 of the element type! Selecting LSEL,S,LOC,Y,0 the lines with y=0 ESIZE,0.5 the size of element LMESH,ALL then we mesh pylon: MAT,1 REAL,2! Selecting of! Setting! Meshing

14 TYPE,2 LSEL,S,LOC,X,XPylon! Selecting of the pylon ESIZE,0.8 LMESH,ALL ESEL,NONE and finally cables: MAT,2 TYPE,3 ESIZE,,1 LSEL,S,LINE,,10,17 cables! Selecting of the *DO,IL,10,17 REAL,IL LMESH,IL CM,E_Cable_%IL-9%,ELEM! Labeling of the cables for element ESEL,NONE *ENDDO ALLSEL 7. Applying loads ANSYS Main Menu > Preprocessor > Loads > Define Loads > Apply > Structural > Displacement > On Nodes. We select base of the pylon and anchor, and press OK. Then we set All DOF = 0. In the same way we set UX and UY = 0 for left end of the deck,

15 and UY = 0 for the right end of the deck. Then we apply the gravity load: ANSYS Main Menu > Preprocessor > Loads > Define Loads > Apply > Structural > Inertia > Gravity > Global ACELY: Running the solution ANSYS Main Menu > Solution > Solve > Current LS > OK. In the next step we will apply the -1m prestress on every cable. ACEL,! Removing the gravity *DO,I,1,8 /TITLE,Cable prestress (1m): Cable No.%I% SFEDELE,ALL,ALL,ALL Deleting forces SFE,E_Cable_%I%,1,PRES,,-1 prestress!! Applying the SOLVE! Running the solution *ENDDO 9. Postprocessing static analysis Reaction forces ANSYS Main Menu > General Postproc > List Results > Reaction Sol. We select All items and press OK. Deformed shape ANSYS Main Menu > General Postproc > Plot Results > Deformed Shape.

16 Deflection caused by gravity ANSYS Main Menu > General Postproc > Plot Results > Contour Plot > Nodal Solution. We select DOF solution and Displacement vector sum, and press OK. Deflection caused by -1m prestress ANSYS Main Menu > General Postproc > Read results > By pick. In the window that appears we select e.g. Set 1 click Read and then Close. ANSYS Main Menu > General Postproc > Plot Results > Contour Plot > Nodal Solution. We select DOF solution and Displacement vector sum, and press OK. 10. Modal analysis The aim of the modal analysis is to determine the first twenty vibration characteristics, namely natural frequencies and mode shapes. ANSYS Main Menu > Solution > Analysis type > New Analysis. We select Modal and click OK. ANSYS Main Menu > Solution > Analysis type > Analysis Options. In [MODOPT] Mode extraction method we select Block Lanczos.

17 For No. of modes to extract we enter 20. Press OK. In the following window we enter for FREQE End Frequency 100 and press OK. ANSYS Main Menu > Solution > Solve > Current LS > OK. 11. Postprocessing modal analysis Deflections ANSYS Main Menu > General Postproc > Read results > By pick. In the window that appears we can see all natural frequencies. We select for example Set 1 click Read and then Close. ANSYS Main Menu > General Postproc > Plot Results > Contour Plot > Nodal Solution. In the following window we select DOF solution and Displacement vector sum and press OK. Animating of the mode shapes Utility menu > PlotCtrls > Animate > Mode Shape We set for No. of frames to create 10 and for Time delay 0.5 and click OK. The animation can be stopped by clicking the Stop button. If you do not stop the animation, you will not be able to see other results.

18 Fluid Coming soon.. Solving the geodetic boundary value problem Solve the geodetic boundary value problem in the homogenous domain bounded by two spheres with radii 6371km and 6871km, 5 and 50 meridians, and 10 and 50 parallels. The size of the elements is 5 x 5 x 50km. There is the gravitational acceleration applied on the bottom boundary, the zero Neumann boundary condition on the side boundaries and the gravitational potential on the upper spherical boundary. The gravitational constant is GM= km^3.s^(-2), the gravitational potential can be computed as GM/radius, and the formula to calculate the gravitational acceleration can be obtain as derivative of the formula for calculating the gravitational potential. 1. Defining parameters Ansys Utility Menu > Parameters > Scalar Parameters. In Selection we type GM= and press Accept. In the same way we define Ru=6871, Rd=6371, Lu=50, Ld=5, Bu=50 and Bd=10. All parameters will be seen in section Items in the alphabetical order.

19 2. Setting the type of the problem ANSYS Main Menu > Preferences > Thermal > OK. 3. Setting the type of the element ANSYS Main Menu > Preprocessor > Element Type > Add/Edit/Delete. We click Add, highlight Thermal solid, then Brick 8Node 70, click OK and close the Element Types window. 4. Setting the material properties ANSYS Main Menu > Preprocessor > Material Props > Material Models. We choose Thermal > Conductivity > Isotropic > and in the following window we type KXX 1. We click OK and close the window. 5. Creating of the computational domain We start by changing the coordinate system to the spherical one: ANSYS Utility Menu > WorkPlane > Change Active CS to > Global Spherical the same can be done by typing CSYS, number of the coordinate system: CSYS, 2 Then we create 8 points that define the whole computational domain: ANSYS Main Menu > Preprocessor > Modelling > Create > Keypoints > On Working Plane we write RD,LD,BD, click Apply. In the same way we create point with coordinates RD,LD,BU, press Apply, then point with coordinates RD,LU,BU, again click Apply, and the last point on the bottom boundary RD,LU,BD, click Apply. Then we create points on the upper boundary: RU,LD,BD, Apply, RU,LD,BU, Apply, RU,LU,BU, Apply and RU,LU,BD OK. You should see eight points on the screen.

20 The same can be done by typing K, number of keypoint, radius, longitude, latitude in the command line: K,, RD,LD BD, K,, RD,LD,BU, K,, RD,LU,BU, K,, RD,LU,BD, K,, RU,LD,BD, K,, RU,LD,BU, K,, RU,LU,BU, K,, RU,LU,BD, (Com.: since no numbers of points were set, points have been numbered automatically starting with no. 1) The easiest way to create the whole computational domain is to type V, KP1,KP2,KP3, in the command line: V,1,2,3,4,5,6,7,8 (Com.: in this way we have automatically created lines and areas, so it is very important to type numbers of keypoints in the right logical order, i.e. with lines not crossed.) 6. Setting of the size of the elements and meshing of the domain To mesh the computational domain we will use the MeshTool: ANSYS Main Menu > Preprocessor > Meshing > MeshTool In the Size Controls we click Lines Set. Then using the mouse we click all meridians (4 arcs), confirm the selection by clicking OK and in the Element Sizes on Picked Lines window we type in the second line NDIV No. of element divisions 8 (it

21 corresponds to 5 ), press Apply. In the same way we select all parallels and set number of divisions 9. In radial direction we set NDIV 10. Then we mesh the whole domain using: ANSYS Main Menu > Preprocessor > Meshing > MeshTool We check whether Volumes is chosen in the Mesh, then in the Shape we tick Hex and click Mesh button. Then we click on the computational domain and press OK. We see volume being meshed. 7. Setting the boundary conditions We start by applying the gravitational potential on the upper spherical boundary: ANSYS Main Menu > Preprocessor > Loads > Define Loads > > Thermal > Temperature > On Areas. We click on the spherical boundary, press OK, and in the VALUE Load TEMP we type GM/RU, click OK. We can observe a little yellow on the screen. Apply upper value arrow Now we will apply the gravitational acceleration on the bottom spherical boundary: ANSYS Main Menu > Preprocessor > Loads > Define Loads > Apply > Thermal > Heat Flux > On Areas. We click the bottom spherical boundary, press OK, and in VALUE Load HFLUX value we type GM/(RD*RD), press OK. Now we can observe a red mesh on the bottom boundary. 8. Running the solution ANSYS Main Menu > Solution > Solve > Current LS > OK. 9. Visualizing results ANSYS Main Menu > General Postproc > Plot Results > Contour Plot > Nodal Solu. In the Contour Nodal Solution Data window, we highlight Nodal Solution > DOF Solution > Nodal Temperature

22 and click OK. 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.

23 1. Select the type of the discipline ANSYS Main Menu > Preferences. We select Structural and click OK. 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.

24 Now your Real Constants window should look like Fig. 2. To close it, we click the Close button. 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

25 We will start with four bottom keypoints: 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.

26 In CLI we use the KGEN command and type 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 *enddo *enddo and to create horizontal lines *do,i,5,37,4 *do,j,i,2+i L,j,j+1 *enddo *enddo 6. A s s i g n i n g r e a l c o n s t a n t s computational domain and meshing of the 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

27 LESIZE,all,,,10,,,,,1 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 *enddo *enddo 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 *enddo

28 *enddo 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.

29 ANSYS Main Menu > Solution > Analysis type > Analysis Options. In [MODOPT] Mode extraction method we choose Block Lanczos. It 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

30 MODOPT,LANB,6 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 >

31 Deformed Shape and in KUND Items to be plotted we select Def + undef edge. We click OK. Now your ANSYS Graphics window should 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.

32 Another way to read result is to use ANSYS Main Menu > General Postproc > By Pick where we highlight the desired set and click Read button. Fig. 7: Modes and corresponding natural frequencies deformations.

33 Structural static analysis Analyzing 2D frame In this tutorial we will analyze 2D frame (see Fig.1) consisting of 2D beams with respect to resistance to two different kinds of loads: (a) the downward shift of the point denoted by the number 5 (see Fig.1) by 5 cm, (b) the gravity load (when gravity acceleration is 9.81m.s^(-2)). The cross-sectional area of all beams is 0.3m*0.4m, where 0.4m is the height of the beams. The distance L=5m, the Young s modulus is 27GPa, the Poisson s ratio is 0.2 and density 2800kg/m^3. Fig.1: Geometry of the computational domain. In our implementation, we will use the element type BEAM3 and the so-called load step files. A load step is simply a configuration of loads for which a solution is obtained, i.e. you can use different load steps to apply different sets of

34 loads, for example gravity load in the first load step, wind load in the second load step, both loads and a different support condition in the third load step, and so on. 1. Select the type of the discipline ANSYS Main Menu > Preferences. We select Structural and click OK. 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: Although in version 13 and 14 of ANSYS, this element has been removed from the GUI menus, it is still available by typing the command: ET, 1, BEAM3. 3. Setting the 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*0.4, in Area Moment of Inertia IZZ we enter 0.3*0.4**3/12 and in Total beam height HEIGHT 0.4 (see Fig.2). We press OK and close the Real Constants window.

35 Fig.2: BEAM3 entering real constants. The same can be done by typing R,1,0.3*0.4,0.3*0.4**3/12,0.4 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 for density DENS: 2800, press OK and close the window. One can see both density and linear isotropic material properties to be entered (see Fig.3). Fig.3: BEAM3 entering material properties. 5. Create the geometry We will start with keypoints. Since they are equally distributed, we will define parameter L=5 to create them. Utility Menu > Parameters > Scalar Parameters In Selection line we type L=5 and press Accept. We close the Scalar Parameters window. Now we can define keypoints using parameter L according to Fig.1. We will start with the bottom keypoints and then we

36 will copy them. You can use either the GUI menu ANSYS Main Menu > Preprocessor > Modelling > Create > Keypoints > In Active CS where you enter the coordinates of bottom keypoints, or CLI by typing: K,1,0,0 K,2,L,0 K,3,2*L,0 K,4,3*L,0 K,5,4*L,0 Then we create remaining keypoints by ANSYS Main Menu > Preprocessor > Modelling > Copy > Keypoints. We click Pick all button and in the following window we type number of copies 5 (including the original), in Y write L and press OK, see the following figure. Then we connect keypoints using the mouse and the GUI menu: ANSYS Main Menu > Preprocessor > Modelling > Create > Lines > Lines > Straight Line and using the mouse we create lines. Be careful to click on every keypoint to create all 36 lines as they are depicted in Fig.4, and then click OK to close the

37 window. Fig.4: Analyzing 2D frame lines. 6. Meshing of the computational domain ANSYS Main Menu > Preprocessor > Meshing > Size Cntrls > ManualSize > Lines > Picked Lines. We pick all horizontal lines and enter the number of divisions NDIV to be 5, press OK. For vertical lines we follow the same way and set the number of divisions 1. Then we mesh all lines by ANSYS Main Menu > Preprocessor > Meshing > Mesh > Lines and clicking Pick All. Now all lines should be depicted in the same light blue colour. 7. Creating the Load steps files Load step file 1: a downward shift of the keypoint 5 by 5cm. To apply constrains on keypoints, we go to the Utility Menu to switch ON Numbering of keypoints: Utility Menu > PlotCtrls > Numbering We tick KP Keypoint numbers and click OK. Then we plot keypoints using Utility Menu > Plot > Keypoints > Keypoints. ANSYS Main Menu > Preprocessor > Loads > Define Loads > Apply > Structural > Displacement > On Keypoints. We pick keypoints 1, 2, 3, 4 and 5, click OK, and in the Apply U,ROT on KPs window, we highlight ALL DOF and click OK. Since no value of ALL DOF (displacements in X and Y direction and rotation) has

38 been given, ALL DOF equals 0. ANSYS Main Menu > Preprocessor > Loads > Define Loads > Apply > Structural > Displacement > On Keypoints. We pick the keypoint 5, press OK, and in the Apply U,ROT on KPs window we highlight UY (ALL DOF must be turned off). For the VALUE Displacement value we type and press OK. We write the Load step file 1 using ANSYS Main Menu > Preprocessor > Loads > Load Step Ops > Write LS File, type 1, and click OK (see Fig.5). Fig.5: The Write Load Step File window. Load step file 2: gravity load (when gravity acceleration is 9.81m.s^(-2)). ANSYS Main Menu > Preprocessor > Loads > Define Loads > Apply > Structural > Displacement > On Keypoints. We pick keypoint 5, click OK, and in the Apply U,ROT on KPs window we highlight ALL DOF, enter 0 in VALUE Displacement value line and click OK. ANSYS Main Menu > Preprocessor > Loads > Define Loads > Apply > Structural > Inertia > Gravity > Global. We type 9.81 in Ydirection and click OK. Note that a positive acceleration in the Y direction stimulates gravity in the negative Y direction (see a red arrow pointing in the positive Y direction in Fig.6).

39 Fig.6: Load step file 2 constrains and gravity load. We write the Load step file 2 using ANSYS Main Menu > Preprocessor > Loads > Load Step Ops > Write LS File and type 2, click OK. 8. Running solution ANSYS Main Menu > Solution > Solve > From LS Files. In the Solve Load Step Files window we type 1 for LSMIN Starting LS file number, 2 for LSMAX Ending LS file number and press OK, see Fig.7. ANSYS will begin solving the problem and will post a message Solution is done! when it has finished. We close the message window and go to the next step. Fig.7: Running solution from Load step files. 9. Visualization and listing of results Results can be read by ANSYS Main Menu > General Postproc > Read Results > By Pick. In the following window, see Fig.8, we highlight the first set, click Read and then Close.

40 Fig.8: Reading of results from Load step files. Deflection: 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. Results after applying first kind of loads can be seen in Fig.9. Fig.9: Load step file 1: deflections. Deformation: ANSYS Main Menu > General Postproc > Plot Results > Deformed Shape and in KUND Items to be plotted select Def + undef edge. We click OK to view both the deformed and the undeformed object. Your graphics window should look like Fig.10.

41 Fig.10: Load step file 1: Deformation. Member force in the X and Y directions, and member moment about Z axis: ANSYS Main Menu > General Postprocessor > Element Table > Define Table. We click on Add and in Define Additional Element Table Items for Lab User label for item write MFORXA. Then in Item, Comp Results data item we highlight By sequence num, and SMISC, and enter 1 after SMISC, in the selection box. We press APPLY. In the same way we define all items according to Fig.11, where Time Stamp denotes the number of the Load step file that has been read. We click OK and close the Element Table Data window. Fig.11: BEAM3 element table. To plot the items that we have defined we go to ANSYS Main Menu > General Postproc > Plot Results > Contour Plot > Line Element Results and in the Plot Line-Element Results window, and for Member force in the X direction we list MFORXA for

42 LabI Elem table item at node I and MFORXB for LabJ Elem table item at node J and click OK (see Fig.12). Results are depicted in Fig.13. Fig.12: BEAM3 The Plot Line-Element Results window. Fig.13: Load step file 1: Member force in the X direction. To plot Member force in the Y direction we follow the same way as before and highlight MFORYA for LabI Elem table item at node I and MFORYB for LabJ Elem table item at node J and click OK. Results can be seen in Fig.14.

43 Fig.14: Load step file 1: Member force in the Y direction. Finally for Member moment about Z axis we select MMOMZA for LabI Elem table item at node I and MMOMZB for LabJ Elem table item at node J and change Fact Optional scale factor to -1 to invert the plot. The ANSYS graphics window should look similar to Fig.15. Fig.15: Load step file 1: Member moment about Z axis. To list items in the Element Table, we go to ANSYS Main Menu > General Postproc > List Results > Element Table Data. We highlight all MFORXA, MFORXB, MFORYA, MFORYB, MMOMZA, MMOMZB and click OK. A list, see Fig.16, with similar values should pop up. To save these results to a file, we click File within the results window (at the upper left-hand corner of this list window) and select Save as.

44 Fig.16: Load step file 1: Listing of Element table. Now we plot and list results after applying the second load step file. First we read results using ANSYS Main Menu > General Postproc > Read Results > By Pick, where we highlight the second set and click Read and Close. Then we update the Element Table using ANSYS Main Menu > General Postproc > Element Table > Define Table click Update and Close. Afterwards we follow the same way as in case of the first kind of loads. Results can be seen in the following figures. Fig.17: Load step file 2: Deflections.

45 Fig.18: Load step file 2: Deformation. Fig.19: Load step file 2: Member force in the X direction. Fig.20: Load step file 2: Member force in the Y direction.

46 Fig.21: Load step file 2: Member moment about Z axis. Fig.22: Load step file 2: Listing of Element table. To obtain more precise solution, we can refine the mesh on horizontal lines and recalculate computations. 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.

47 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 Add/Edit/Delete > Add > > Element Type > 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 > 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

48 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 Y 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 H

49 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: 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

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

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

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

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

54 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.

55 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

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

57 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

58 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 Solving stationary heat equation problem in 2D using APDL APDL is an abbreviation for ANSYS Parametric Design Language that is a scripting language used to automate common tasks as

59 well as to build a model in terms of parameters. As we can see in Fig. 1, geometry is more complicated in terms of more materials, keypoints and areas, hence APDL will be used. Fig. 1: Geometry of computational domain and illustration of boundary conditions. Fig. 2: Illustration of material properties and areas. We will start by opening the preprocessor, setting the proper element type, i.e. element type that is designed for 2D problems with temperature as a degree of freedom in each node, and we will define conductivities for all six materials.

60 In general, to open the preprocessor menu, we type in the prompt /prep7 The command for setting the element type is ET,1,element type number To define materials for thermal problem, we write MPTEMP,1,0 and then we define conductivities for all materials MPDATA,KXX,No. of mat.,,value of conductivity The proper practical implementation is in the following Table /PREP7 ET,1,55 MPTEMP,1,0 MPDATA,KXX,1,,0.043 MPDATA,KXX,2,,0.5 MPDATA,KXX,3,,0.049 MPDATA,KXX,4,,1.48 MPDATA,KXX,5,,0.99 MPDATA,KXX,6,,0.42 To create the geometry, we number all keypoints according to Fig. 1 and calculate their X and Y coordinates according to thicknesses given by Fig. 1. The command for creating keypoints is K, No.of keypoint, X, Y, Z. In our case, only 2D computational domain is of interest, so Z coordinates are zero and do not have to be filled-in. In this way, we will create all 19 keypoints.

61 K,1,0,0 K,2,0.12,0 K,3, ,0 K,4,0.12,0.5 K,5, ,0.5 K,6, ,0.5 K,7, ,0.6 K,8, ,0.6 K,9, ,0.62 K,10, ,0.62 K,11,0.12,0.9 K,12, ,0.9 K,12, ,0.9 K,13, ,0.9 K,14, ,0.9 K,15, ,0.93 K,16, ,0.93 K,17,0,1.4 K,18,0.12,1.4 K,19, ,1.4 Then we have to create areas. Since all areas are defined by line segments and ANSYS automatically joins points by line segments, we will create the areas just by keypoints. The general command is A,KP1,KP2,KP3,KP4,, where KPi denotes the number of keypoint. The areas are numbered automatically in order they were created. The practical implementation in our case is A,1,2,4,11,18,17 A,2,3,6,5,4 A,4,5,12,11 A,5,6,7,9,10,14,13,12 A,7,8,10,9 A,13,14,16,15 A,11,12,13,15,19,18

62 Since we have already defined all materials and created all areas, now we are able to assign materials to areas. We start by selecting the area of interest, the general command is ASEL,S,,,No.of area, where letter S denotes that a new set is chosen. material to area by AATT, material number,,1,0. By command ASEL,ALL we reselect all areas. So we write We assign

63 ASEL,S_,1 AATT,1,,1,0, ASEL,ALL ASEL,S_,2 AATT,2,,1,0, ASEL,ALL ASEL,S_,3 AATT,3,,1,0, ASEL,ALL ASEL,S_,4 AATT,4,,1,0, ASEL,ALL ASEL,S_,5 AATT,5,,1,0, ASEL,ALL ASEL,S_,6 AATT,5,,1,0, ASEL,ALL ASEL,S_,7 AATT,2,,1,0, ASEL,ALL The next step is dividing the domain into set of elements. We start by setting the size of elements through ESIZE, size of elements, number of divisions. Then we set the shape of elements by MSHAPE,0,2D where 0 denotes quadrilateral elements and 2D dimension. By

64 MSHKEY,0 we choose the so-called free meshing, by 1 we would choose the so-called mapped meshing. Finally, we mesh all areas by AMESH,all. We type ESIZE,0.01,0, MSHAPE,0,2D MSHKEY,0 AMESH,all We will prescribe boundary conditions on lines according to Fig. 1. The general formula for convection boundary condition is SFL, number of temperature. SFL,6,CONV,25,,-11, FLST,2,5,4,ORDE,5 FITEM,2,8 FITEM,2,13 FITEM,2,19 FITEM,2,22 FITEM,2,24 SFL,P51X,CONV,6,,20 line, CONV, Film coefficient,, bulk

65 Now it is time to leave preprocesor and open solution by typing /SOLU The command that initiates the solution is SOLVE It reads data from database to calculate solution and writes results to database and also to the results file. In the same manner we type /SOLU SOLVE To plot results, we open general postprocessing by /POST1 and type PLNSOL, TEMP,,0 that is a command for plotting the temperature contours. So finally we type /POST1 PLNSOL, TEMP,,0

66 Solving stationary heat equation problem in 2D using GUI The computational domain with lengths and thicknesses of all materials as well as boundary conditions is given by Fig. 1. Fig. 1: Geometry of computational domain and illustration of boundary conditions.

67 1. Select the type of the discipline ANSYS Main Menu > Preferences > Thermal > OK 2. Select the type of element for our BVP, we choose 2D thermal solid element Plane 55 ANSYS Main Menu > Preprocessor > Element Type > Add/Edit/Delete > Add > Select Thermal Mass Solid, Quad 4Node 55 > OK > Close 3. Setting material properties No. Material Conductivity 1 Plaster Isolation Porotherm Plaster 0.99 ANSYS Main Menu > Preprocessor > Material Props > Material Models > Thermal > Conductivity > Isotropic > KXX = 0.81 OK

68 Then click Material > New Model > write 2 and Conductivity > Isotropic > KXX= OK. Material Number 2 will appear in the left column of the Table. same way, we define all four materials, and close the Material Model Behaviour window. again Model In the Define 4. Creating of the computational domain The overall geometry is defined in ANSYS by keypoints which we specify using coordinates from Fig.1 and the following Table. No. X[m] Y[m] No. X[m] Y[m] No. X[m] Y[m] a) Define keypoints ANSYS Main Menu > Preprocessor > Modeling > Create >Keypoints> In Active CS Define the 1st point with coordinates X=0, Y=0 and press APPLY. In the same way, we define all Keypoints. With given keypoints, we are able to create areas.

69 4b) Define areas ANSYS Main Menu > Preprocessor > Modeling > Create > Areas > Arbitrary > Through KPs. Write numbers of keypoints that define the 1st area (i.e. 1,2,4,3,12,11) and press APPLY. To define the second area, write 3,4,6,5,13,12. To define the third area, we write 5,6,8,7,14,13 and finally for fourth write 7,8,10,9,15,14. Press OK. To check geometry, we go to Utility Menu Numbering of areas. to switch ON Utility Menu > PlotCtrls > Numbering... > AREA Area numbers OFF (then OFF will be toggled to ON), OK

70 You should see four different colored areas with no lines crossed as they are depicted in the following Figure. With properly defined computational domain, we can divide it into elements. There are several ways to do that and we will use the so-called Mesh Tool. 5. Meshing of the computational domain ANSYS Main Menu > Preprocessor > Meshing > Mesh Tool In Element attributes choose Areas and click SET. Then write number of 1st area, namely 1, and press OK. In the following table for Material number choose 1, press APPLY. In the same way attach material 2 to area 2, and so on.

71 In Size Controls choose Areas and click SET. Then press Pick All, and in the following table write Press OK. Finally, in Mesh check whether Areas option is chosen, press Mesh button and then Pick all button. You should see the area being meshed. To check proper material assignment, go to Utility Menu > PlotCtrls > Numbering...> Elem/Attrib numbering choose Material numbers press OK. You should see meshed computational

72 domain with each material depicted in different colour. Afterwards, we can apply boundary conditions. Since the zero Neumann BC is automatically applied on each part of the boundary where no other BC has been prescribed, we will prescribe the Newton BC only. 6. Prescribing boundary conditions ANSYS Main Menu > Preprocessor > Loads > Dene Loads > Apply > Thermal >Convection > On Lines Choose outside boundary, namely two lines as they are depicted in Fig. 1, and write 25 for VALI Film coefficient and -11 for VAL2I Bulk temperature, press OK. Then do the same for inside boundary and write 6 for VALI Film coefficient and 20 for VAL2I Bulk temperature, press OK. You should see red arrows.

73 7. Running solution ANSYS Main Menu > Solution > Solve > Current LS > OK Note Solution is done! appears, press Close. You can close also /STATUS Command window. 8. Visualization of results ANSYS Main Menu > General Postproc > Plot Results > Contour Plot > Nodal Solu and in DOF Solution choose Nodal Temperature. Press OK.