ME 442 Overview Marc/Mentat-2011 Tutorial-1 The purpose of this tutorial is to introduce the new user to the MSC/MARC/MENTAT finite element program. It should take about one hour to complete. The MARC/MENTAT program is divided into two parts: the MENTAT pre- and post processor, and the MARC program. In the preprocessing step MENTAT is used to generate the finite element model, apply boundary conditions (loads, displacements, temperatures...), initial conditions, material properties, element geometry, and analysis type (stress, thermal...). This information is stored in an input file, which may be further edited to generate more advanced options. In the processing step, the input file is read by the MARC program, which solves the problem and writes an output file. MENTAT, which performs the postprocessing step, then, reads the output file. Sample Problem The deflection and stress of a three-dimensional cantilever beam will be used to demonstrate capabilities of MARC and MENTAT. Three-dimensional linear solid elements will be used, although others, e.g., beam elements, are possible, and may be preferable. The solid elements are the most general, and will illustrate some of the limitations of beam elements. The beam to be analyzed has dimensions (x,y,z) = (10,1,2) inches and is made of aluminum. Aluminum will be considered elastic and linear with a modulus E = 1(10 7 ) psi and Poissons ratio = 0.334. A 1 lbf load is applied at the right end (x = 10 in.) in the negative y-direction. The left end of the beam (x = 0) is rigidly fixed(all slopes and deflections = 0) to a wall. The maximum deflection for a cantilever beam from two dimensional small deflection beam theory is, Y = - F L 3 / 3 E I where F = 1 lbf is the load, L = 10 in. is the length of the beam, and I is the cross section moment of inertia and is equal to (2 * 1 3 ) /12 in 4. From this equation the maximum deflection for the given load is 0.0002 inches. Shear and the third dimension are unaccounted for in two dimensional beam theory, so the deflection calculated by the program will be slightly different. All problems should be formulated using this procedure. That is, clearly define the problem geometry, boundary and initial conditions, and material properties and do a hand calculation so you know approximately what magnitude the finite element calculation should be. Do this before attempting to run MARC. 1
Finite Element Analysis Log on and start the program, i.e., START > ALL PROGRAMS > MSC.Software > Marc2010 > MarcMentat 2010. Shortly the start-up window will appear. The screen is divided into 5 areas. The upper left, from the MAIN MENU title down to the QUIT button is the dynamic menu area. This area has buttons that contain submenus to preprocess, analyze, and postprocess in addition to configuring the terminal. It is dynamic because it changes when you use different sections of the program. Basically the cantilever beam problem will be solved by stepping down the dynamic menu. The band to the right of the QUIT button is the static menu. These buttons can be used throughout the program, and do not change as you move through the program. Below the QUIT button is the dialogue area. This is where the program prompts you for input and displays error messages. You can scroll up or down by using the appropriate arrow keys on the keyboard. To the right of the dialogue area is the status box that displays messages when the program is busy, or displays the message Ready when the program can accept input. It should say, Ready now. The remaining part of the screen is the graphics area where the model with its boundary conditions, etc., and output plots are displayed. The program is menu driven. Just click on buttons with the mouse to execute commands. When a button that executes a command is pressed, the command appears in the dialogue area. This command may also be typed in from the keyboard instead of using the mouse. Once executed, a command can be undone using the UNDO command in the static menu. To activate a button, move the cursor on top of the button and press the left mouse button (LMB). At Clarkson, it is much faster and much less error prone to operate from the local C:\TEMP directory. Data generated this way will be temporarily stored until you quit, so make sure you save your data to your student account before exiting MENTAT. The FILES menu in the static box allows this directory change. Click on FILES, then CURRENT DIRECTORY. Place the cursor to the right of SELECTION and enter C:\TEMP. Then click OK and MAIN with the LMB. You are now ready to begin building the model. Note that the buttons in the menu area have arrows pointing to the right. This means that clicking them will bring up another submenu. Again, we ll generally proceed from the top to the bottom of the dynamic menu. Move the cursor to the MESH GENERATION button and click the LMB. The menu area has changed. You want to use 8-node 3-D elements, but the default class is 4 node 2-D elements. To change this, click the LMB on ELEMENT CLASS. The menu will change again. Note the difference in the type of buttons. The buttons in this group show that only one button can be selected at a time. Click the LMB on HEX(8). To get back to the MESH GENERATION menu, either click the right mouse button (RMB) when the cursor is anywhere within the menu area or the LMB on RETURN at the bottom of the dynamic menu. You are now ready to generate the cantilever beam geometry. There are many ways to do this. One method is to draw curves and points in a manner similar to a CAD program and then generate a finite element mesh from this geometric entity using a mesh generator. Another method is to make a coarse mesh directly, and then subdivide it using the SUBDIVIDE command in the MESH GENERATION menu. For this demonstration, you will make a single element and DUPLICATE it. 2
Click on the ADD button to the right of the NODES in the menu area with the LMB. In the dialogue area you will see a prompt for the node coordinates. Type in coordinates (leave at least one space between entries on each line): 0 0 0 <return> 1 0 0 <return> 1 1 0 <return> 0 1 0 <return> You will see the response node added in the dialogue area after each return and the node appear in the graphics area. Each node will have its own number, so it can be identified. To see node numbers, click the LMB on PLOT in the static menu area. The dynamic menu will change. To show node numbers, click on the NODES SETTINGS button and then the LABELS title with the LMB followed by REDRAW. Then, click the RMB twice anywhere in the menu area to return to the MESH GENERATION menu. You now have four labeled nodes in the global x-y plane at z = 0. Click on FILL in the STATIC menu to fill the graphics area. You need eight nodes to define a hexahedron. You could keyboard in the coordinates of the remaining four nodes.. Instead, you can duplicate the four existing nodes. To do this click the LMB on the DUPLICATE button. First you tell it how to duplicate, then you tell it what to duplicate. You want to duplicate the four existing nodes once in the z-direction, 2 away. Under the TRANSLATIONS button type 2 <return> in the third field. Now tell it what to duplicate by clicking the NODES button. You could type in the numbers 1 2 3 4 <return>, but since you want to pick all of the nodes, it is easier to click on the EXIST button under the ALL: menu at the bottom of the dynamic menu area with the LMB followed by END LIST#. Do this and you will see that the node numbers now have two numbers drawn on top of each other. This is because your viewpoint is the x-y plane. To see all eight nodes, click on the RX+ button on the top line in the static menu to rotate the view about the x-axis followed by FILL. Click the RMB anywhere in the menu area to return to the MESH GENERATION menu. You are now ready to create an element. Click on the ADD button next to ELEMS. You will be prompted to enter the element node(1) number. You could type in number 1, corresponding to node 1, but we will use the mouse. Click on node 1 in the graphics area with the LMB. You will see that the number has been filled in the dialogue area and you will be prompted to enter node(2). Click on nodes 2 through 8 in order. The node order is important when you define an element. If done incorrectly, the element could be distorted or inside out. This can be ascertained with the CHECK command within the MESH GENERATION menu. Within CHECK select INSIDE OUT and CROSS ELEMENTS. If the element is INSIDE OUT, then FLIP it. Also, the nodal input order can be different for different types of elements. Accessing the HELP file in the static menu will provided this information. For this demonstration the order chosen is correct. After you have picked node(8) you will get a message Element added, and the element will be shown in the graphics area. The element should be a hexahedral 1 x 1 x 2 inches. To get a 10-inch long beam, you can duplicate the element in a manner similar to the way you duplicated the nodes. To do this, pick DUPLICATE with the LMB. Under TRANSLATIONS, type 1 0 0, respectively, in the three fields, then <return>. This time, you want to make nine elements, so to the right of the REPETITIONS button type in 9 <return> Now click the ELEMENTS button. Before you clicked the ALL:EXIST. button. You could do this, but instead, click on the X on the element face in the graphics area. Note that nothing has happened except that the original element has been highlighted. This is because the program is giving you a chance to duplicate more than one element. Since you don t have more elements to duplicate, you need to tell it that this is the end of the list of elements to duplicate. Do one of these options now: 3
1. click the RMB in the graphics area, or, 2. click the LMB on END LIST# button in the ALL: menu, or, 3. type #<return> in the dialogue area. You can see that an element has been created to the right of the original element. To see the whole model, click FILL in the static menu with the LMB. Click the RMB anywhere in the dynamic menu area to return to MESH GENERATION. Note that some nodes have two numbers near them. This is because the elements have been duplicated, like lining up blocks on a table. Each element has its own corner. You don t want separate blocks; you want to join the elements into a single contiguous beam. You do this using the sweep processor. Click on SWEEP button with the LMB. Click the ALL button in the SWEEP menu (Not the REMOVE UNUSED menu). Any nodes within the specified Tolerance (default = 0.0001) are combined. You will see the message Deleting 36 duplicate nodes in the dialogue area. Click the RMB and return to the MESH GENERATION menu. There is now only one node number at each node, but there are gaps in the numbering. To fix this, click the LMB on the ALL button in the RENUMBER menu. Note that the node numbers have changed. You now have a model with 44 nodes and 10 elements. This completes generating the model. Return to the MAIN menu. GEOMETRIC PROPERTIES, which appears next in the MAIN menu, will not be necessary in this case since all information concerning element geometry has been prescribed. Click the MATERIAL PROPERTIES > MATERIAL PROPERTIES buttons. ANALYSIS CLASS default is STRUCTURAL, so no changes here. Click NEW > type STANDARD. Under STRUCTURAL > YOUNGS MODULUS insert 1e7 <return> For Poissons ratio, insert 0.334 <return> Note that the numbers to the right of the buttons in the pop-up have changed. Click OK. Name the material by clicking the NAME button and typing in Aluminum <return> Next, you need to tell the program what elements are aluminum. Click the ELEMENTS ADD button followed by the ALL:EXIST. button. You will see the number 10 appear in to the right of the ELEMENTS menu. You can toggle the ID MATERIALS button to show what elements correspond to the materials you defined. Click this off when done viewing. Next apply boundary conditions. Before doing this, it s a good practice to save your work. Click the SAVE button in the static menu area with the LMB. You will get a message Model saved to model1. in the dialogue area. MENTAT saves files to model#.mud by default, where # is a number starting with 1, and.mud is implied though not shown. If there is already a model1.mud file in your directory, it will save the current model as model2.mud, etc.. Note that every time you click on a button in the dynamic or static area, you had to use the LMB. From now on, if you are instructed to click on a button in these areas, use the LMB. Click on the MAIN button at the bottom of the dynamic menu area. You will return to the original screen you had when you first started. Click on the BOUNDARY CONDITIONS button. You want to apply mechanical boundary conditions, so click on the STRUCTURAL button. First we ll clamp the fixed end of the beam. Click on FIXED DISPLACEMENT. A pop-up menu will appear in the graphics area. Click the ON buttons to the left of X,Y, and Z DISPLACE buttons to turn on those displacements (or degrees of freedom). The default value of zero displacement is appropriate. Either click the OK button at the bottom of the pop-up or the RMB anywhere in the pop-up area to return. 4
Now that you have defined a fixed boundary condition you need to tell the program where to place it. Click the NODES ADD button. To pick the four nodes on the left end of the beam place the mouse cursor in the graphics area slightly above and to the left of node 4. Hold down the LMB and drag the mouse to slightly below and to the right of node 5. Release the LMB and you will see that the four nodes are highlighted. Click the END LIST# button, and see the boundary conditions applied as arrows at the four nodes. Also notice the number at the right of the NODES menu is 4. You should give this boundary condition a meaningful name so you won t get confused later. Do this by clicking the NAME near the top of the menu area. Then type FixAllDisp <return> The name just above the NAME button has changed from apply1 to FixDisp. Now add a vertical load of 1 lb on the right end of the beam. Put a point load of 0.5 lb on the top corners of the beam so the beam will not twist. Click on the NEW button near the top of the menu area. The title has changed to apply2. Click on the POINT LOAD button. Another pop-up menu appears in the graphics area. Click on the ON button to the left of the Y FORCE button. Click on the Y FORCE button and type in -0.5 <return> Click the RMB button. Now pick the NODES ADD button. Click on node 26 with the LMB and note that it is highlighted. Then click on node 44, and it to will be highlighted. Click on the RMB in the graphics area to end the list. Click on the NAME button, and type PointLoad <return> to name this boundary condition. Click the RMB in the dynamic menu area to move back to the BOUNDARY CONDITIONS menu. Click the ID BOUNDARY CONDITIONS button to show all of the boundary conditions. When you are done inspecting the boundary conditions, click the ID BOUNDARY CONDITIONS button again to turn this feature off. Click SAVE to save your work and return to the MAIN menu. Remove the node numbers in PLOT > NODES-SETTINGS > toggle LABLES off, DRAW, and return to MAIN. You are now ready to define the type of analysis. Click on LOADCASES in the MAIN menu. You are doing a structural analysis, so retain the default setting STRUCTURAL. Under NEW, select STATIC. Then select PROPERTIES. Click on LOADS. Note that both the fixed displacement and point load are selected (highlighted). The program lets you define many boundary conditions for the same geometric model. Say you wanted the axial deflection of this same beam under a unit axial load. You could apply axial load boundary conditions. This is where the pop-up you are viewing becomes useful. You could deselect the axial load and run the analysis. Then, select the axial load case and deselect the bending load and rerun without having to repeat the rest of the model. Since you have only two conditions and they are both needed for this analysis, click the OK button (or the RMB anywhere in the pop-up menu). Also, select STEPPING PROCEDURE-FIXED and set # STEPS to 1. Only one step is needed in this static analysis. Return to the MAIN menu and SAVE. Click on the JOBS button. This menu is used to put the finishing touches on your analysis. Under NEW select STRUCTURAL. Under PROPERTIES select a LOADCASE from AVAILABLE. Then lcase1 should appear under SELECTED. Other items in this menu to consider are: ANALYSIS OPTIONS > use defaults, JOB RESULTS > select CAUCHY STRESS under tensors and EQUIVALENT Von Mises Stress under scalar. ANALYSIS DIMENSION: Use default, 3-D INITIAL LOADS > not required in this static analysis, but check that the boundary conditions are selected. 5
The next thing you have to do in the JOBS menu is choose the correct element type. There are several types of elements that can be used with an eight-node hexahedral geometry. Each type has different properties. Select ELEMENT TYPES. In this menu consider: ANALYSIS CLASS > STRUCTURAL ANALYSIS DIMENSION > 3-D SOLID > FULL INTEGRATION > type 7 > OK The dialogue area prompts you to Enter element list. In this case, select ALL EXIST. Element 7 is a full integration trilinear shape function. This means that strain varies linearly within the element in all directions but stress is constant. Toggle the ID TYPES and ID CLASSES buttons to view the same. Click the RMB anywhere in the dynamic menu area to get back to the JOBS menu. SAVE your work. Your job is now ready to RUN.. There is a choice on how to submit a job to the MARC program. You could write a MARC output file (done with the UTILS button in the static area), or you could run MARC from inside MENTAT. We will do the latter. Click on the RUN button in the JOBS menu, and a pop-up will appear. Select RESET > SUBMIT (1) > MONITOR. Your job is now running in the MARC program in the background. If you have made no mistakes, after a few moments you should see the number 3004 next to EXIT NUMBER. If there is a different number, you have made a mistake. Click on EXIT MESSAGE to see what the error message means. Also, you can get a listing of the input and output files by clicking on EDIT OUTPUT FILE. Errors are quite often obvious when scanning this file. Search on error. If successful (EXIT NUMBER 3004), you can now view the results of your analysis. Click on the OPEN POST FILE (RESULTS MENU) button and model1_job.t16 should appear on the top of the dynamic menu under POST FILE. The.t16 is the binary output file. Click LAST followed by DEF & ORIG under DEFORMED SHAPE, then SETTINGS under the DEFORMED SHAPE menu. Click the AUTOMATIC button. This scales the deflection so that you can view it. Click RESET VIEW and FILL in the STATIC menu for a better view. Next click the RETURN button. This button is the same as the RMB in the menu area. Use these interchangeably. Click the NEXT button, and you will see the beam deflect. To get numerical answers, click the SCALAR button, select DISPLACEMENT Y in the pop-up menu, then RMB. Click the CONTOUR BANDS button and the beam will change to a contour plot of the y- displacements with a maximum value of 0.000118 in.. You could also view the numerical value at each node by selecting NUMERICS instead of CONTOUR BANDS. The resulting plot is rather busy, but if you use ZOOM from the static menu you could easily read a numerical value 0.000118 in. at x = 10 in.. The deflection calculated from beam theory is -0.0002 in.. These answers aren t close. Your FEM analysis hasn t given you the correct result! You have been set up. This is to show you that even though an analysis has been performed correctly, the answer may not be correct. The problem with this analysis is that the mesh is too coarse for the element type and problem conditions. Element type 7 assumes that the displacement between the nodes is a straight line, so you were trying to analyze the beam with ten straight-line (linear) segments. More elements will provide a better representation of the bending of this beam, so you will now refine your model. Click CLOSE and return to MAIN. Mesh Refinement Let s get a better answer by refining the mesh. First however, the format of this tutorial will be changed to be more concise. Proceed through the menus as indicated. FILES from static RESTORE Save this to be refined model under a new name, say, model2, SAVE AS model2 <return> 6
FILL to fill the graphics area with the model MAIN MESH GENERATION SUBDIVIDE Note the defaults. You wish to divide each hexahedron in half in each dimension, so the defaults are good. ELEMENTS ALL:EXIST. END LIST (#) RETURN Note again that you have to sweep to get rid of the extra nodes, and renumber. SWEEP ALL near the top of the menu RETURN RENUMBER ALL RETURN You now have 80 elements and 189 nodes. SAVE in the static menu. The nodes with the boundary conditions have been retained, but more nodes have been placed on the fixed end. This means that you need to apply boundary conditions to the new nodes on the fixed end. MAIN BOUNDARY CONDITIONS STRUCTURAL PREV or NEXT until FixAllDisp is found NODES ADD add all nodes on the left boundary END LIST# you now have 9 nodes on the fixed boundary MAIN SAVE JOBS > RUN > RESET > SUBMIT 1 > MONITOR When you see the 3004 exit number, then view the results as before. Now the maximum deflection is 0.000168 in. This is much closer to the 2-D beam theory solution of 0.0002 in.. It is still unclear if this answer is correct. In general, it is a good idea to refine your mesh until the change in the answer is small, say a few percent, depending on the problem, desired accuracy, etc.. Mesh and element refinement will be the subject of the first lab assignment. Finally, look at the distortion of the transverse y-z cross section of the beam at x = in.. Rotating the beam about the x-axis, ZOOMing, and observing NUMERIC output of the result can accomplish this. Alternately, the PLOT PATH plotting option could be used. In either case, two-dimensional beam theory states that transverse cross sections remain similar. What does the FEM model show? Is it correct? Explain. Before you quit MENTAT, save your work to your student account. Once you quit all data in the C:\TEMP directory will be lost. To quit MENTAT from the MAIN menu, select QUIT, then EXIT. Then logout from the system. 7