General Issues and Quick Reference 2
ANSYS Handout:
General Issues and Quick Reference
X.J. Xin
Mechanical and Nuclear Engineering
Kansas State University
1. How to Launch ANSYS 2
1. On MNE Computers in MNE Technology Classroom or Department Computer Lab: 2
2. On Engineering Computer Center computers in Fiedler Hall: 2
3. To quit ANSYS: 3
4. Basic steps in FEM analysis: 3
2. Some General Issues about FEM Simulation 5
1. Physical Units 5
2. Displacement Control versus Displacement Control 6
3. Detailed Distribution of Forces on the Boundaries 6
4. Rigid Body Motion 7
5. Selection of Element Type 9
6. Order of Element 10
7. Convergence of a Solution 10
8. Good Mesh and Bad Mesh 11
3. Quick Reference about Using ANSYS 13
1. Triangular element or quadrilateral element? 13
2. To constrain or not? 13
3. How to generate a good mesh 13
4. Examples of good meshes 14
5. If the model disappears after a wrong zoom-in action, how to get the whole model back to the window again? 16
6. What you should always do first after obtaining the solution 17
7. How to undo a wrong boundary condition? 17
8. How to obtain displacements for a node 17
9. How to obtain displacements for a node - a simpler way 18
10. How to obtain stresses for a node 18
11. How to plot wanted quantities (e.g. stresses, strains, displacements, etc.) along a path (i.e. a user-defined line) 19
12. How to obtain vector plots for principal stresses? 19
13. How to get a hardcopy of or save into a file a picture on the graphics window 19
14. How to find the maximum sigma_xx (SX) 19
15. How to find maximum displacement UX 20
16. How to use on-line help in ANSYS? 20
17. How to create a solid model in ProE and import it into ANSYS? 20
18. How to create a solid model in ANSYS and import it into ProE? 21
19. How to use component and assembly to organize output information? 21
20. How to change the background color of a mesh? 22
1. How to Launch ANSYS
1. On MNE Computers in MNE Technology Classroom or Department Computer Lab:
Create a directory "me533" on Z:\
From Start menu: Programs > ANSYS 7.1 > Configure ANSYS Classic
The interactive ANSYS dialogue box will appear. Set the following:
Working directory: Z:\me533 (You can also select other directory of your preference)
Initial jobname: [a name of your choice, such as hw1] (the default job name is "file")
Uncheck "Use Default Memory Model", and set
Total workspace: 200
Database: 100
Click Run. ANSYS is ready for simulation.
2. On Engineering Computer Center computers in Fiedler Hall:
From Start menu: Programs > Software > CAD > Ansys 7.1 Interactive
or Programs > ANSYS 7.1 > Interactive
The interactive ANSYS dialogue box will appear. Set the following:
Working directory: C:\TEMP
Initial jobname: [a name of your choice, such as hw1] (the default job name is "file")
Uncheck "Use Default Memory Model", and set
Total workspace: 200
Database: 100
Click Run. ANSYS is ready for simulation.
The working directory holds all ANSYS files. Of all ANSYS files, the [jobname].log and [jobname].db are the most important. The *.log file records all commands or actions you performed during the ANSYS interactive session, while the binary database file *.db stores all model binary data.
It's a good idea to click the [SAVE_DB] button frequently. It will save data into the *.db file. Whenever you click [RESUM_DB], ANSYS will read from the db file, and restore all your work up to the last [SAVE_DB]. Use [SAVE_DB] button frequently - computers crash from time to time.
In another ANSYS session, if the *.db file is in the working directory, you can recover the model by "File > Resume from …", then choose the desired *.db file. After you resume from the db file, you may not see anything on the screen. But the model data are read in. You may plot lines, areas, elements, etc. to see the model using "Plot > ..." menu.
Another way to rebuild the model is to use the *.log file. Copy the *.log to anther file with a name different from the [jobname].log, such as mylog.log You can then recreate your model by "File > Read input from …", and select mylog.log. The screen will show all steps you performed from the beginning - assuming there is no error in the log file. But usually the display on the screen is too fast to see clearly. Note that commands or actions in a new ANSYS session are appended to the [jobname].log. If you want the [jobname].log to store only commands or actions in the new session, delete the [jobname].log before launching ANSYS.
CAUTION: If you want to keep your ANSYS models, you need to copy at least the *.log and *.db files in the working directory onto a zip disk or your permanent network account before you log out the computer. All files in the local C:\TEMP will be automatically erased after you log out.
3. To quit ANSYS:
From the menu:
File > Exit …; Save Everything, OK
Or from the ANSYS Toolbar
Quit; Save Everything, OK
4. Basic steps in FEM analysis:
To solve any mechanical problem, we must know or be provided with the following information: (1) the geometry of the structure or component; (2) the material properties; and (3) the applied loads and support conditions (boundary conditions). We then apply the mechanics principles to solve the problem. Finally we will calculate the information of interest, such as stresses and deflection and judge whether the structure is safe or rigid enough.
In FEM, the above procedures are translated into three main steps: (1) preprocessor, (2) solution and (3) postprocessor.
Preprocessor: for creating the model geometry, defining material properties, defining element types and related real constants (such as thickness for a 2D model, cross-section, and moment of inertia for a beam), and meshing the continuum model into "finite element mesh". The boundary conditions can be specified either in the preprocessor or in the next step, solution.
Solution: for specifying displacement boundary conditions and applied loads, and for solving the system equations.
Postprocessor: for post processing wanted information such as deformed shape, deflection of points of interest, various stress components (such as normal xx stress, shear xy stress, principal stress, and von Mises stress) along specified locations (such as a line), error estimate of the analysis, etc.
The above three general steps will be the same for any commercial FEM software packages. But each package has its own way of naming the substeps within each general step. We will learn the ANSYS way. ANSYS GUI tries to follow the logic steps in solving a mechanical problem, and logical thinking usually helps. Also, by exploring the various options presented by the GUI, you will learn more and better.
ANSYS is a rather versatile program and can solve structural (stress-deformation), heat transfer, fluid flow problems. It can also perform dynamic and impact analysis. But we will focus on static deformation-stress analysis only (called "structural" option in ANSYS).
2. Some General Issues about FEM Simulation
1. Physical Units
FEM program does not specify the units for any variable. It is up to the user to make sure the units of the variables are consistent. The rule for maintaining unit consistence is as follows: the units for a primary variable can be chosen freely, while the units for a derived (secondary) variable must be derived from the units of the primary variables. A primary variable is one whose units cannot be expressed by the combination of the units of other primary variables, while a derived variable is one whose units can be expressed by the combination of the units of the primary variables.
For structural problems, the user can choose time, length, and mass as the primary variables, or time, length, and force. An example for the derived variable is stress, because the units of stress can be expressed by force/length2. Assuming that time, length, and force are the primary variables (because the units of any of these three variables can never be expressed by the combination of the units of the other two), the user can use meter, millimeter, or inch for length, and kilogram, Newton or pound for force. But the units for the stress, which is a derived variable, must be derived consistently from the units of length and force.
As an example shown in the figure above, a 2D plane strain plate is subjected to traction P=120 lb/in at the bottom. The Young's modulus E is psi (pounds per square inches). If length L is in inches and the traction is in pounds per inch, then strains are always dimensionless, while displacements will be in inches and the stresses in psi. The user can also choose to use other units, see the table below:
Choice / Length / Force / Traction / Stress / What to use in ANSYS / SolutionsL / P / E / Displ. / Stress
1 / in / lb / lb/in / Psi / 6 / 120 / / in. / psi
2 / m / N / / Pa / 0.1524 / / / m / Pa
3 / mm / N / / MPa / 152.4 / 21.0 / / mm / MPa
Note:
1 lb=4.448 N = 0.454 kg, 1 inch=25.4 mm = 0.0254 m, 1 Pa=1 N/m2, psi = pounds per square inches, 1 ksi = 1000 psi = 6.895 MPa
2. Displacement Control versus Displacement Control
In FEM, the prescribed displacement boundary condition and the given traction (or force) boundary condition are the most common types. (There are other types such as elastic support which will not be considered here.)
Prescribed displacement boundary condition means that the nodes will be fixed (zero displacements) or move to the desired positions according to the prescribed values regardless of the rigidity of the deforming structure. This corresponds to an infinitely rigid loading mechanism. Given traction (or force) boundary condition means that a given amount of traction (or forces) will always be applied to the specified element edges (or nodes) regardless of the deformation of the elements or nodes. This corresponds to an infinitely flexible (compliant) loading mechanism.
Both prescribed displacement b.c. and force boundary b.c. are just idealization of the actual situation. Most boundary conditions of actual engineering problems are in fact under elastic support. The idealized boundary conditions, however, greatly simplify the mathematics. If the support or loading grip is more rigid than the structure, prescribed displacement b.c. is a good approximation. If the support or loading grip is much softer than the structure (or the boundary is a free surface), prescribed traction or force b.c. is a good approximation.
3. Detailed Distribution of Forces on the Boundaries
In practice, the detailed local distribution of boundary tractions can be quite complicated. Take the example illustrated in the following figure. In original problem (a), a steel ball of weight P is tied to the bottom of a plate. In FEM model (b), the load is modeled as a point force of P acting at the center of the bottom edge. In model (c), the load is modeled as three point forces of P/3 acting at three points symmetric about the centerline. In (d), the load is modeled as 3 point forces, P/4, P/2, P/4, with the center force weighted twice as the other two. In (e), the load is modeled as distributed traction of P/L acting along the bottom edge. Because the loads in all four models (b) to (e) give the same force resultant and moment, according to Saint Venant's principle, the difference in the load distribution on the boundary only affects the stresses and strains close to the loading zone. In other words, in regions reasonably away from the bottom edge, the stress-strain fields for all four cases will be almost the same. Consequently, (b) to (e) are all acceptable FEM models for the original problem (a).
For models (f) and (g), however, even though the force resultants are the same, the moments are different from the original problem. For model (h), the force resultant is 1.5P. Therefore (f), (g) and (h) cannot be accepted as the equivalent to the original problem (a).
(a) Actual problem (b) OK (c) OK (d) OK
(e) OK (f) Not OK (g) Not OK (h) Not OK
4. Rigid Body Motion
Since the equilibrium and constitutive law of deformed solids are built on stresses and strains which involve only the derivatives of the displacements rather than the displacements themselves, the solution for the displacement field will not be unique if all boundary conditions are of prescribed traction/force type, and solutions may differ by a rigid body motion (as rigid body motion causes no stresses and strains). In numerical simulation, this means that if the structure is not constrained to prevent rigid body motion, the coefficient matrix of the governing equations will be singular (refresh the memory about the Kramer's rule about linear equations...). It is therefore important to impose properly additional boundary conditions if the constraints of the original problem are insufficient to prevent such rigid body motion.
There are many ways to prevent rigid body motion in 2D. One simple way is to fix an arbitrary point (A) of the structure (both the x and y degrees of freedom of A are constrained), then select another point (B) away from A and constrain B from rotating about A. This can be achieved by restraining the degree of freedom of B vertical to line AB, as illustrated in the following figure.