Institute of Mechatronics and Information Systems

Size: px

Start display at page:

Download "Institute of Mechatronics and Information Systems"

Preston Phillips
6 years ago
Views:

1 EXERCISE 4 Free vibrations of an electrical machine model Target Getting familiar with the fundamental issues of free vibrations analysis of a simplified model of an electrical machine, with the use of a finite element computation system ANSYS. Program 4.1 Determine the free vibrations frequency spectrum of a simplified model of an electrical machine stator. Task 4.1 Determine first ten frequencies of free vibrations and their modes for a simplified model of the stator with casing and feet of an electric motor Data Dimensions of the magnetic core: - inside radius r in = 0.12 m: - outside radius r out = 0.14 m: - core length l m = 0. 1 m. Dimensions of the casing: - casing length l cas = 0. 2 m; - casing thickness t cas = m; - height of the motors axis h = m; - distance between feet l f = 0. 2 m; - feet thickness t f = 0, 005 m. Material parameters of steel: - Young s modulus 11 E = 2 10 Pa; - Poisson s coefficient ν = 0. 3 ; - density 3 ρ = kg/m 3 ; Note: use a DOT as the decimal point Finite Element Method solution Finite elements A suitable finite element should be selected for each specific computed construction (object). The investigated object is a solid block. This kind of solid should be divided into elements with four walls - tetrahedron (in the following steps). Paweł Witczak, Prof. D.Sc. Ph.D. M.Sc. Eng 23

2 From the main menu of the ANSYS software select Preprocessor: Main Menu Preprocessor and then Element Type Add/Edit/Delete, in the Element Type window click the button Add, in the Library of element type : in the left box select Solid, in the right box select Tet 10node 187, apply your choice by clicking the OK button. An element Type 1 called SOLID187 was declared The chosen element has been saved in the Element Type table. The properties of the saved elements can be checked by clicking: Options... Help. To finish click: Help OK Close. Close the Element Type window Materials Adequate material properties of the computed construction should be entered. Perform this task as follows: Main Menu Preprocessor Material Props Material Models, in the window Define Material Model Behavior : in the left box select Material Model Number 1, in the right box select Structural (double click) Linear Elastic Isotropic, in the next window, in position EX enter the value of Young s modulus: 2e11, in position PRXY enter the value of Poisson s coefficient: 0.3, click OK to apply the entries, select Density - enter density of steel material: 7.8e3 (or 7800), click OK to save the entry. The entered parameters have been saved in Material Number Model Magnetic core The ANSYS software enables modelling of basic solid objects almost automatically. Half of a hollow cylinder is created in the following way: Main Menu Preprocessor Modelling Create Volumes Cylinder By Dimensions. In the window Create Cylinder By Dimensions, in the appropriate positions enter: RAD1 - outside radius of the magnetic core: 0.14, RAD2 - inside radius of the magnetic core: 0.12, Z1, Z2 - coordinates of the magnetic core length: 0, 0.1, TETA1 - initial angle (in degrees): 0, TETA2 - final angle (in degrees): 180, click OK to save the entries. To visualise a three dimensional depiction of the created volume click the cube icon on the right side of the screen. Check the operation of the other icons. The position of the X-Y-Z axes can bee seen on the screen. Paweł Witczak, Prof. D.Sc. Ph.D. M.Sc. Eng 24

3 Fig Half of the magnetic core model. The whole magnetic core model can be created by mirroring the entities against the X-Z plane. Main Menu Preprocessor Modelling Reflect Volumes, in the window Reflect Volumes click Pick all and mark X-Z plane Y, click OK to save the entries. Click Plot Replot in the command line at the top of the screen. Fig Magnetic core model after executing the command Replot. Paweł Witczak, Prof. D.Sc. Ph.D. M.Sc. Eng 25

The separate halves should be glued in order to form one model of the whole magnetic core. Main Menu Preprocessor Modelling Operate Booleans Glue Volumes Pick all.

4 The separate halves should be glued in order to form one model of the whole magnetic core. Main Menu Preprocessor Modelling Operate Booleans Glue Volumes Pick all. Casing of the stator The X-Y plane is positioned at the end of the magnetic core, 0.1 meters long. In order to place the outer casing symmetrically against the core the appropriate coordinates must be entered: Z1 = m and Z2 = 0.15 m. Main Menu Preprocessor Modelling Create Volumes Cylinder By Dimensions. In the window Create Cylinder By Dimensions, in the appropriate positions enter: RAD1 - outside radius of casing: 0.14, RAD2 - inside radius of the casing: 0.145, Z1, Z2 - coordinates of the casing: , 0.15, TETA1 - initial angle (in degrees): 0, TETA2 - final angle (in degrees): 360 (full hollow cylinder), click OK to save the entries. Fig Creating model of the casing. Paweł Witczak, Prof. D.Sc. Ph.D. M.Sc. Eng 26

Fig. 4.1.4 Magnetic core and casing model.

5 Fig Magnetic core and casing model. Feet The mounting feet will be modeled as blocks (cubes), the appropriate dimensions should be entered into the table: Main Menu Preprocessor Modelling Create Volumes Block By Dimensions. In the window Create Block By Dimensions, enter the coordinates: Fig Creating model of the foot (vertical part). Paweł Witczak, Prof. D.Sc. Ph.D. M.Sc. Eng 27

6 Fig Model with vertical part of the foot. In the same way we create the horizontal part of the foot, entering the appropriate coordinates: X1, X2-0.1, 0.12, Y1, Y , , Z1, Z , Fig Model with complete foot. Paweł Witczak, Prof. D.Sc. Ph.D. M.Sc. Eng 28

The second foot can be created using the symmetry (Reflect) in plane Y-Z. In case of the display configuration as below, mark the rectangular volumes: V4, V5 OK. Fig. 4.1.

7 The second foot can be created using the symmetry (Reflect) in plane Y-Z. In case of the display configuration as below, mark the rectangular volumes: V4, V5 OK. Fig Creating model of the second foot. Now we have the whole, needed structure, therefore the separate parts must be added: Main Menu Preprocessor Modelling Operate Add Volumes Pick all, Fig Simplified model of an electric motor. Paweł Witczak, Prof. D.Sc. Ph.D. M.Sc. Eng 29

8 Division of the model into finite elements Attributes At the beginning attributes should be assigned to the model, that means: types of elements used, actual constants (in this case thickness of the walls) and materials. Main Menu Preprocessor Meshing Mesh Attributes All Volume. In the window Volume Attributes the proper entries of material number and element type can be seen on the figure below. Fig Declaration of the volume s attributes. Element dimension In the next step the dimension of the element should be declared. The accuracy of the problem s solution depends, inter alia, on the dimensions of the elements. However too small elements and therefore large number of elements causes that the computation time is unnecessarily prolonged. Lets assume that the edge of the elements, in our case, should be equal 0.01 mm. Main Menu Preprocessor MeshTool. In the window MeshTool, in the section Size controls select Global Set SIZE element edge length, enter: Meshing Main Menu Preprocessor MeshTool. In the window MeshTool, in the section Mesh the software displays the solid s division Volumes. Below the shape is displayed: Tet (tetrahydron) and option Free - the software will automatically select the optimal finite element division. Finish by clicking the option Mesh. The screen will display the volumes of the model divided into finite elements. The elements are connected in the nodes located in the intersections of the mesh. Paweł Witczak, Prof. D.Sc. Ph.D. M.Sc. Eng 30

Fig. 4.1.11 Division of the model into finite elements (meshing). Boundary conditions Each construction must be fixed (supported).

9 Fig Division of the model into finite elements (meshing). Boundary conditions Each construction must be fixed (supported). It is easier to operate on the drawing with the surfaces of the object s volume. In addition it is convenient to use the numbering of lines and points of the construction s geometry. In the menu bar at the top of the screen select PlotCtrls, in the next windows choose: Numbering, then Plot Numbering Control Area OK. Fig Numbering of the planes. Paweł Witczak, Prof. D.Sc. Ph.D. M.Sc. Eng 31

10 We assume that the analyzed structure is fastened by the surfaces on the bottom of the feet. Enter: Plot Areas. The boundary conditions are given as loads and constraints applied to appropriate nodes on the chosen areas (surfaces): Main Menu Preprocessor Load Define Loads Apply Structural Displacement On Areas. Click with the mouse on the chosen surfaces. In the case displayed in Fig A50 and A 59 In the window Apply U, Rot on Areas confirm the choice of the surface OK, and then: All DOF OK. Close the Preprocessor after entering all the data. NOTE: Alternatively, additional boundary conditions can be entered later blocking the displacements in the planes perpendicular to the axis of the motor, at the ends of the cylindrical casing Solution Determination of the result of calculations is performed in the Solution segment of the ANSYS software. Choose: analysis type: modal analysis, calculation method (option): Lanczos, number of deflection shapes (modes) to be considered: 10, range of frequencies to be considered: from 0 to Hz. Main Menu Solution Analysis Type New Analysis choose Modal OK. Next select the analysis options: Main Menu Solution Analysis Type Analysis Options In the window Modal Analysis, in section Mode extraction method, mark Block Lanczos and in the window No. of modes to extract enter 10. In the lower section: Expand mode shapes mark the box Yes, and No. of modes to expand enter 10. Click OK to save the entries. In the window Block Lanczos Method, in the box Start Freq enter 0, in the box End Frequency enter Click OK to save the entries. The computer performs the calculations after clicking consecutively: Main Menu Solution Solve Current LS. The end of the computation process is announced by a window with the text: Solution is done. Click Close Results The visualisation and analysis of the results is possible in the segment General Postproc. Numerical results The numerical results of all calculated free vibration frequencies are summarised in: Main Menu General Postproc Result Summary. Paweł Witczak, Prof. D.Sc. Ph.D. M.Sc. Eng 32

11 The ordinal number of the deflection shape (mode), of natural vibrations, is given in the first column of the results table SET. The second column TIME/FREQ presents the value of the calculated frequency of the vibration for the particular mode. Visualisation and animation of results It is more convenient to view the results as animated pictures of the deflections. Choose the following options: Main Menu General Postproc Read Results First Set. In the menu bar at the top of the screen select PlotCtrls, in the next windows choose: Animate Mode Shape... DOF solution Deformed Shape OK. Animation of the first mode of free vibrations of the beam should appear on the screen. Fig Example of the model deflection shape for the third mode. The (apparent) speed of the beam s movement can be adjusted by the delay slide, in the Animation Control window. Stop and close the animation: click Stop Close. The other deflection shapes (modes) of the natural vibrations can be inspected by loading next sets of data: Main Menu General Postproc Read Results Next Set. In the menu bar at the top of the screen select PlotCtrls, in the next windows choose: Animate Mode Shape... DOF Solution Deformed Shape OK. Last edited 4 December 2013 Paweł Witczak, Prof. D.Sc. Ph.D. M.Sc. Eng 33

Institute of Mechatronics and Information Systems

Institute of Mechatronics and Information Systems EXERCISE 2 Free vibrations of a beam arget Getting familiar with the fundamental issues of free vibrations analysis of elastic medium, with the use of a finite element computation system ANSYS. Program