AN INTRODUCTION TO ANSYS SETTING UP FOR USING ANSYS 1. 2. Login to CAE Windows NT Account Enter the START menu, then proceed through GENERAL ENGINEERING into ANSYS 5.3 into RUN INTERACTIVE NOW.
SAMPLE ANSYS SESSION Overview Presented below is an introductory session to ANSYS. In this session, you simulate the loading of a square, elastic plate with a central hole under plane stress conditions. Because of the symmetry of the problem, you only need to model 1/4 of the plate as indicated on the right-hand side below; the lines labeled 1 and 2 are lines of mirror symmetry:
1
2
The purpose of the analysis is to determine the stresses and strains surrounding the hole. From such an analysis you can tell, for instance, the stress at which the plate will begin to yield (based on a von Mises criterion). There are analytical solutions for this problem (one of which is shown in Dieter's book, chapter 2), so it is possible to check the numerical answers from finite element analysis (FEM) based on the analytical solutions. The analysis below proceeds through the following steps 0. 1. 2. 3. 4. 5. 6. Define the type of problem (structural) Define the element-type to be used. Specify material properties. Define the shape of the object. Mesh the object Define the "loads" ("load" can mean stresses, displacements, temps., etc) Obtain a solution.
7. Access and interpret the results. The Details After entering into ANSYS you should be presented with a collection of windows. The first window you are interested in is at the left-hand side of the screen and called ANSYS MAIN MENU. It contains headings like PREFERENCES PREPROCESSOR etc. 0. Define the type of problem (structural) To specify the general type of problem in which you are interested (a structural problem), click with your mouse on PREFERENCES This opens a window. Click on WILL SHOW next to STRUCTURAL. You can now hit OK to get out of PREFERENCES. You are now going to work in the PREPROCESSOR. Essentially, most of your work is done here (steps 1-5 above). 1. Define the element-type to be used. Click PREPROCESSOR if you haven't already. Next choose ELEMENT TYPE Choose ADD/EDIT/DELETE Choose ADD which takes you a library of element types. Choose STRUCTURAL SOLID Choose QUAD 4NODE 42. . Then hit OK. You are doing a two-dimensional problem and the Quad 4node 42 element is a 2dimensional element (or, if needed, an element for cylindrical symmetry, which can be treated as quasi 2-d element). The element can either do plane stress or plane strain; You can vary this option by getting into the OPTIONS window. By default, the element is set to plane stress. Now get out of the ELEMENT TYPES and back into the PREPROCESSOR by clicking CLOSE.
2
Next, you want to specify the important material parameters. 2. Specify material properties. In the PREPROCESSOR, choose MATERIAL PROPERTIES Choose MATERIAL MODELS LINEAR ELASTIC ISOTROPIC You want to input properties, say EX = 200e3 (the young's modulus of steel in MPa) and poisson's ratio PRXY = 0.3. You then want to save the material parameters by hitting OK and closing the MATERIAL MODELS window. You should return to the PREPROCESSOR window. You are now ready to start detailing the shape of the object. 3. Define the shape of the object. From the PREPROCESSOR WINDOW choose MODELING In MODELING choose CREATE then choose AREAS and RECTANGLE You can size and locate the rectangle by choosing BY DIMENSIONS To create a 1010 square, fill in the boxes with 0 10 0 10 Click OK to get out of the DIMENSIONS box and then close the RECTANGLE box. At this point, a big rectangle should appear on the screen. You are next going to introduce a circle to the drawing so that you can subtract it from the rectangle. In the AREAS window choose CIRCLE then choose BY DIMENSIONS and set OUTER RADIUS 3 and ENDING ANGLE 90 Then hit OK 3
and close the CIRCLE and CREATE windows. You should now be back in the PREPROCESSOR. You want to subtract the circle from the rectangle so open MODELING and then OPERATE BOOLEANS SUBTRACT At this point a SUBTRACT AREAS box will open up. In addition, you should look carefully for instructions in a grey dialog box or window at the bottom left of ANSYS screen menu window. The instructions request that you click with the mouse on the area from which you are going to subtract something. CLICK THE MOUSE SOMEWHERE IN THE CENTER OF THE RECTANGLE, and then hit OK Next, the dialogue box requests that you use the mouse to indicate the area to be subtracted. CLICK THE MOUSE ON THE CIRCLE then hit OK Close the SUBTRACT and OPERATE windows and return to the PREPROCESSOR. The object should look something like this:
4
2 5 3 1
I have numbered the sides of the object in the above diagram to help with subsequent instructions; the numbers are not shown on the ANSYS screen (actually, ANSYS also numbers the lines, and the numbers do not coincide with mine – but we don't use the ANSYS numerology here, so I won't worry). You can now get out of MODELLING. You are now ready to mesh the object. 4. Mesh the object In the PREPROCESSOR go under MESHING and choose SIZE CNTRLS then LINES and PICKED LINES
4
A menu window will open up and the box at the bottom left of ANSYS will ask you to use the mouse to pick the lines to be meshed. CLICK ON LINES 1 AND 2 WITH THE MOUSE. If you accidentally click on the wrong line, you can undo your choice by hitting the secondary button on the mouse. Doing this will turn the mouse cursor from an upwardpointing arrow to a downward-pointing arrow . If you click on the unwanted object with the downward pointing arrow, it is taken off the list of picked lines. You can then reset to by hitting the secondary mouse button a second time. After choosing lines 1 and 2 you should hit OK and a new menu will pop up. Set the following boxes: Ndiv Space and hit OK To help you see what you have done, you can now go up to the PLOT menu under the main utility window at the top of ANSYS and click LINES. This action will cause the computer to show the boundary lines including nodes established on lines 1 and 2. There are 20 nodes (Ndiv = 20) on each line, and the nodes near the outer surface are separated by thrice the separations of nodes near the inner circle (Space = 1/3). We want to produce a higher mesh density near the inner circle (hole) because it acts as a stress concentrator; the stress varies rapidly within this region. Next, hit PICKED LINES again and choose the circular-shaped inner line labeled 3 in the above diagram. Set Ndiv 21 Space 1 Hit OK and get out of the SHAPE AND SIZE WINDOW (you should be back in the PREPROCESSOR?) Next, click MESH Click the mouse on AREAS Click the mouse on MAPPED then -CONCATENATE- LINES The computer will ask you to pick the lines to concatenate (join together for the purpose of meshing); you should choose lines 4 and 5 in the above diagram. The reason for doing this is that it is impossible to construct a 5-sided object (your rectangle with a hole) from 4-sided pieces (the elements quad 4node 42). You join together two of the sides to make the object 4-sided. Hit OK Next, choose 3 OR 4 SIDED The computer will ask you to choose the area to be meshed. Choose your rectangle, then hit 5 20 1/3
OK. The computer should think a little bit then produce a mesh that looks something like a spider web:
You are now finished meshing the area. Close the windows and return to PREPROCESSOR. If for some reason the mesh looks asymmetric or messy, you can try repeating the meshing sequence and fiddle around until you get something that looks nice (this will probably not be a problem). 5. Define the Loads Back in the PREPROCESSOR window, choose (DEFINE) LOADS at the bottom of the window. In this window, choose TIME/FREQUENCY TIME&SUBSTEPS And enter Time at end of Step 10 Number of Substeps 10 (Choose STEPPED Boundary conditions) And hit OK Next, in the LOADS window hit APPLY then STRUCTURAL Then PRESSURE and finally 6
ON LINES The computer will ask you to choose with the mouse the lines on which the pressure is to be applied. Choose line 4 (top of rectangle) with the mouse, then click OK The computer will ask you for the amount of pressure. A positive number corresponds to a compressive pressure, while a negative number corresponds to a tensile pressure. A reasonable value of stress corresponds to -E/100 or -E/1000; you might use -1e3 corresponding to E/200 (if earlier you used E=200e3). After you input the number hit OK then close the PRESSURE window. At this point little one or more little red arrows will appear on the screen indicating that a traction exists. Next, in theSTRUCTURAL menu, choose DISPLACEMENTS then SYMMETRY ON LINES The program will ask you to indicate the lines of symmetry; you should choose lines 1 and 2. You then finish with an OK and close everything up to PREPROCESSOR. You are now back in the MAIN MENU. Finally, you are ready to ask the computer to solve the problem that you have set up. 6. Obtain a Solution From the MAIN MENU pick the SOLUTION window. From the SOLUTION window, choose SOLVE then CURRENT LS (i.e., load step) then hit OK The program will crunch along, and will eventually halt and produce a pretty picture showing the boundary conditions on the plate. 7. Plotting the results Back in the MAIN MENU choose GENERAL POST PROCESSOR Then READ RESULTS. Choose what you want plotted (LAST RESULTS, STRESS, Y-DIRECTION, then hit OK And get back into GENERAL POST PROCESSOR. Next hit PLOT RESULTS and ELEMENT SOLUTIONS
7
You then have to decide what it is you want to plot. You can now animate the picture by going to the ANSYS/UNIVERSITY UTILITY MENU at the top of the computer screen and clicking PLOTCTRLS ANIMATE DEFORMED RESULTS STRESS Y-DIRECTION You can plot stress vs position by going into GENERAL POSTPROCESSOR PATH OPERATIONS DEFINE PATH Then clicking onto two nodes that you wish to define as the first and last points along a path along which you wish to obtain the stress or strain. After selecting nodes, click OK Then under PATH OPERATIONS click MAP ONTO PATH And, for instance, click STRESS Y-DIRECTION OK Next, click PLOT PATH ITEMS SY OK
(for instance) (for instance)
8