SURVEILLANCE DE L’INTÉGRITÉ DES STRUCTURES - GMC 724
Département de génie mécanique
DEVOIR 2 Modélisation de la propagation d’ondes guidées
Ramy Mohamed et Patrice Masson
Jun 2011
1
1. Ansys Tutorial 1.1 Planning Your Simulation Before you start your simulation, you need to determine the main parameters of your simulation, as have been mentioned in the lecture. The main set of parameters that need to be determined prior to the simulation: •
The minimum wavelength for the propagating modes, which in turn depends on the maximum resolvable frequency fmax.
Figure 1: The maximum resolvable frequency determination. Figure 1, shows the time trace of the excitation signal, 5.5 cycles sinusoidal modulated 450 kHz tone burst and the corresponding Fourier transform (using the timeFreq.m file). Based on the frequency selected, you can determine the minimum wavelength from the dispersion curves as shown in Fig. 2; the wavelength λS0, and λA0 can be determined from the slope of the line connecting the origin of the dispersion curves of the material and the intersection of the fmax with the curve. So, for example λA0=d*tan(θA0) x 10-3 ( in m) at the frequency fmax, where d is the thickness of the plate in mm.
2
Figure 2: The minimum wavelength to be determined from the dispersion curves. •
Determine the approximate element size; the main guiding rule is to have 20 points per minimum wavelength. Which for a 4 noded plane element amounts to hx = λA0/20.
•
Since we have chosen to dimension our geometry in m, we have to make sure that the rest of the units are consistent with that choice. For example Young’s modulus should be in (Pa), CL or CS in (m/s), ρ in (kg/m3).
•
Since we have determined the approximate element size, we can determine the stable time step using the following equation for rectangular elements
1
∆t =
cp 1 2 + 1 2 hy hx
where cp is the phase velocity of the fastest propagating mode. After having determined the stable time step, we have an idea about how many time steps (in Ansys terms substeps) are going to be produced, so we can proceed with the simulation using Ansys.
3
1.2 Running Your Simulation 1.2.1 Start ANSYS and set the general configuration parameters of the simulation 1- Start >> Ansys13.0 (or Ansys12.1) >> Mechanical APDL Product Launcher 2- The product Launcher should start, browse for the folder that will contain your model, and determine the name of the model. If the folder does not exist the launcher program will ask you if you would like to create a new folder with the specified name. • Check if the Simulation Environment is ANSYS • Select the High performance computing setup tab, then check use Shared-memory parallel (SMP), to enable the multicore processor support. • Check the type of License provided, if it is educational then there will be a limitation on the number of the nodes, if your model does not fit the limited number of nodes supported by the educational license you can use the same computer that was used in Lab 2, in the SHM lab. It has an Academic Research license. • Click on the Run button • The space that is required by the simulation results could be huge. So, make sure that the drive that your folder resides in have enough space ~ 500 MB. 3- The Ansys Mechanical APDL interface should start, as shown in figure 1, with the Ansys Output window shown on the right side. The output window could be hiding behind the interface so it is recommended that you adjust the size of the windows in order to see both of them. Figure 1 shows the different names that will be used when we refer to different menus or items that will be used during the modeling steps. When there is a Main menu >> submenu >> subsubmenu, it means that the selection of different menus remains in the same window. Then it will be followed by the action to be taken. Utility Menu Command Input Ansys Toolbar
Message Area
Figure 1: The Ansys mechanical APDL GUI. After each of the following steps, you have to save your work; this could be done by pressing the Save_DB button in the Ansys toolbar. If your work was interrupted or closed for any reason, you can start the Ansys using the same procedure and Resume_DB will give you the last saved changes. In the command input type (/config,nres,5000) where 5000 is the number of substeps that could be written to the results file. The default is 1000 which is by no means sufficient for a Lamb waves simulation. Remember this
4
step has to be taken at the begin level. So, it is not saved with the data base, every time you want to increase the nres in an ANSYS session you have to do that, whether you start a new database or resume an existing one. To have a remark saved regarding the units used in the model, it is preferred to have (/units, SI) in order to have a reminder attached to the DB. It does not mean there is any unit conversion is done.
1.2.2 Create the geometry, select element types and create materials 1- Main menu >> Preferences Select Structural then Press OK This is done for customization of the future options and GUI only for structural applications. 2- Main Menu >> Preproccessor >> Modeling >> Create >> areas >> rectangle >> By 2 Corners Fill in the dimensions WP x is the origin of the working plane in x direction WP x is the origin of the working plane in x direction Width is the length of the plate; Height is the thickness of the plate 3- Main menu >> Preproccessor >> Element Type >> Add/Edit/Delete A new window Element Types will appear click on Add button Select from the left list Structural >> solid Select from the right list Quad4node 182 then click OK Now the defined element types should reflect your choice (Type 1 Quad4node 182) Click the options button, then in the pop up window set Element Behavior K3 from the drop down list to plane strain then OK.
5
Close the element type window. 4- Main Menu >> Preproccessor >> Material Props >> Material Models In the Define Material Model Behavior Window, click on the Structural>> Linear >> Elastic >> Isotropic In the Linear Isotropic Properties for Material 1 window input the value of Young’s modulus in EX, and Poisson’s ratio in PRXY, then click OK. In the Define Material Model Behavior Window, click on the Structural>> Density In the Density for Material 1 window input the value of materials density in DENS, then click OK Exit the Define Material Model Behavior window from menu item material >> Exit or click the upper right x. Now; having defined the geometry, the element type and the materials props, you are ready to start meshing your geometry.
6
1.2.3 Create the mesh, and loading function 5- Main Menu >> Preproccessor >> Meshing >> Mesh Tool Lines click on set, a selection window will appear in the left part of the screen, use the mouse and left click on the upper and lower lines of the rectangle to select them, then press OK in the Element size on picked lines window. A new window will appear, set the element size in the SIZE to the required dimension, and click OK. The same procedure should be done for the left and right edges of the rectangle to determine the element size that will be used for meshing. The element size should be determined by the minimum wavelength that could be propagating in the structure. At least 20 points per wavelength, for the Quad4Node 182 element the element size is equal to λ/19. Then click on Mesh button, click on pick all in the Area to mesh, OK, and then Close to close the mesh tool. 6- Now we are set to define the force as function of time, this is a crucial step in the simulation and should be handled with care. Utility Menu >> Parameters >> Functions >> Define/Edit The Function Editor window will appear as shown in figure, select Multivalued function based on regime variable, type in the , any name that you would like, (for example time1) . The value of the = in the second row will change accordingly to the name that you used, click in the space following the equal sign, and then from the drop down menu select TIME. Or type {TIME} in the space. So, you should end up with figure. Click on the upper tab Titled Regime 1, in the Regime 1 Limits set the limits of the time variation of your load (for a sinusoidal tone burst (t= n/fo) where n is the number of the cycles, and fo is the central frequency of the excitation). In the Result =, input the function that you want to use, for example for a sin modulated n cycles sinusoidal toneburst you can use the following function: sin(2*3.14*fm*{TIME})*sin(2*3.14* fo*{TIME}) where fm = (0.5 fo /n) is the modulating frequency. To plot the function, you can use the GRAPH button; increase the Number of Points to make the figure clear and to get an idea about the sampling rate of the results to be used later in determining the frequency of writing the output files. To retrieve the previous plot of the mesh you can use Main Menu >> Plot >> Elements. In Regime 2 tab, select the upper limit as the end of your simulation time tfinal and the value equal to 0*{TIME}. Save your function to a file named “filename.func”, then close the Function Editor from file >> close. Ansys have to read the function file and translate it into a table based on the time step that you are going to use in your simulation. That is the reason that it enables you to construct the function independent of specific simulation parameters.
7
8
1.2.4 Set boundary conditions, initial conditions and start the analysis 7- Main Menu >> Solution >> Analysis Type >> New Analysis Select Transient and click OK, then accept the default solution method as full by clicking OK. 8- Main menu >> Solution >> Define Loads >> Apply >> Structural >> Displacement >> On Nodes This step in the analysis correspond the nonempty set of Γg where there should be at least one point with fixed displacement to have non-singular stiffness matrix. This part also, needs some consideration, you are advised to consult the mode shapes in order to determine which point to fix. Selecting a node by picking form the graphics screen, is the easiest way to select a node. Another method will be provided in the postproccessing part of this tutorial that could be more accurate for determining a node location that you need to fix. A window titled Apply U, ROT on Nodes appear, select All DOF, then press OK. By leaving the Value blank, you accept the default values of zero. Or you can set the value directly to zero. 9- Utility Menu >> Parameters >> Functions >> Read form File Select the file that you previously saved under the filename.func, a new window appears, in the Table Parameter Name type a name for the table to be used later in the force determination. Then press OK. 10- Main menu >> Solution >> Define Loads >> Apply >> Structural >> Force/Moment >> On Nodes Apply F/M on Nodes picking window appear, pick the node where the forces are to be applied, then click OK. • Select the direction of force • In the Apply as drop down list select Existing table. • Select the name of the table that you have defined in step 9; OK. 11- Now we have defined the boundary conditions and the loading, what remains to have a well posed problem is to define the initial conditions Main menu >> Solution >> Define Loads >> Apply >> Initial Condit’n >> define • Pick all, OK • All DOF, OK. You can see that we need two initial conditions for a transient analysis, one for the displacement and the other for velocity. This is because the equations governing the wave propagation phenomena are 2nd order PDEs. 12- Now we are ready to define the time step and the frequency of the output. Main menu >> Solution >> Load Step Opts >> Unabridged Menu You will see that the menu changes to the full version, so we are able to select Time/Frequenc >> Time-Time step. • In the Time and Time Step Options window • Time at end of load step = tfinal. • Time Step Size = 0.5*Δt ( already determined from planning stage). • Minimum Time Step = 0.1*Δt • Maximum Time Step= Δt • Then press OK. We are still in the Load Step Opts. So, we can determine the frequency of output Load Step Opts >> Output Ctrls >> DB/Results File
• •
Item Item to be controlled select from the drop down list Nodal DOF solu For setting the frequency for output, in the FREQ file write frequency select Every Nth substep and put the value of N as suitable. Press OK.
13- In the command input type “Check” and see if there are any warnings or errors in the output window. 14- Main Menu >> Solution >> Solve >> Current LS The status of your simulation will pop up, read it and close it, then press OK in the Solve Current Load Step and watch the progress of your simulation in the output window. If every thing was done as in this tutorial you should receive a message (Note) saying that “Solution is done” press Close.
9
1.2.5 Postprocessing 15- Utility Menu >> Parameters >> Scalar Parameters In the selection window type “Sensor_pt = node(x, y, z)”, the Sensor_pt is a name that you can choose feely. While the (x, y, z) provide the coordinates of the required node. Then Press Accept. This method of naming points or nodes could be used instead of all the picking steps that was used previously by selection from the Graphics window.
10
16- Main menu >> TimeHist PostPro
• • •
In the Time History Variables window click on the plus sign. Select in the Add Time History Variable, select Nodal Solutions >> DOF solutions >> X Component (or Y component of Displacement). OK. Then after the variable appears in the variable list, you can press on the graphing icon to show the results.
Finally, you can consult the Utility Menu >> Help >> Ansys Tutorials to increase your familiarity with the software.
11
2. Assignments For Assignment spend some time with the Ansys help and find out how the fixing of one point on the boundary could be avoided using axisymmetric boundary conditions. If successfully understood you can use axisymmetric BC for the assignments. Otherwise, you have to select the points of fixation wisely and mention in each of the assignments how you chose it.
2.1 Assignment (1):
Use the same procedures that was provided in the tutorial to model a symmetric excitation using the geometry shown 10 N 1 mm 10 N
700 mm
The forces have amplitude 10 N, and the time dependence is Sinusoidally modulated 5.5 Cycles, at three different frequencies of your choice. Provide the results (time history of the Ux and Uy displacments) at the same location (which you should chose), and explain the results. Correlate your results with the group velocity, and check if there is a difference between the theoretical value and the numerical one. If there is any difference explain why. The material is Glass, with the same values used in obtaining the dispersion curves for Lab2. Provide a detailed account of the effect of the frequency on the dispersion the numerical signal witness. [Hint: For the correlation with the group velocity you will need to record the time history at to distant points at least and find out the time of flight between the two signals).
2.2 Assignment (2): This is the last assignment, try to model the geometry used in Lab 2 (dimensions should be taken form the experimental setup), selecting the location of the measurement corresponding to the center of the sensor used experimentally. (Use PACSHARE for obtaining the material properties and the dispersion curves for the Glass) Explain how you could select the point of fixation in order to not interfere with the results in each assignment.
10 N 4 mm 10 N
[Hint: To model the geometry, you can use two rectangles, followed by Boolean operations to glue the two prior to meshing, Main Menu >> Modeling >> Operate >> Booleans >> glue >> Areas]. This should give ideal bonding results, (i.e. as if the two plates were made from the same material from the start). Explain the results.
12
