MET 210W Page 1 of 13

Handout – ANSYS Examples

ANSYS is a software tool used by engineers to perform variety of analysis on mechanical parts and systems. The focus of this handout is using ANSYS to determine reactions, stresses and deflections in beams and frames.

ANSYS uses the finite-element method to determine the reactions on a structure as well as the stress and deflections at various points on the structure. The basic component of a finite-element model is the element. Graphically, beam elements appear as a line, but to the software, an element is a series of equations that predict how the ends of the element will deform when loaded. For each two-dimensional beam element, six equations are needed to determine the rotation and translations of each node. Nodal translations are defined parallel and perpendicular to the element. Elements connect with each other at nodes. The response of an element to an applied load affects each of the elements connected to it at nodes. A model will have three equations for each node in the model. The deformations at each node are found by ANSYS using matrix math to solve all of the equations for the model simultaneously.

The basic procedure for solving a beam problem using ANSYS is as follows:

  1. Start the ANSYS program.
  2. Specify the element type to be used. In ANSYS, the 2D beam element is designated as BEAM3.
  3. Specify the real constants for the element: area (in2), height (in) and moment of inertia (in4). The area cannot be zero. The height is used to find bending stress. In ANSYS, the distance c is always taken as half of the height. Be aware of this when working with sections which are not symmetrical.
  4. Indicate the material properties: modulus of elasticity (psi) and Poisson’s ratio.
  5. Create nodes. A node is needed at each load and support as well as at any point of importance in the structure, which is any point where the stress or deflection is to be found. Each node will have a unique number. Nodes are located by Cartesian coordinates determined by the user. The length units used MUST be consistent with those used to define the real constants and material properties.
  6. Create elements between nodes. Each element will have a unique number. Elements are defined by selecting a node for each of its end. Elements cannot have zero length.
  7. Apply support constraints to nodes. Translation can be constrained parallel and perpendicular to the element to create pins and rollers. Rotation can also be constrained at a node when creating a fixed support.
  8. Apply concentrated loads and moments to the model at nodes. Loads are typically applied horizontally or vertically. All units must be compatible with other units used in the model. Distributed loads can be applied as pressures to the elements. Warning: the value specified for pressure is applied per unit length of the element. If an element is 12 inches long, a distributed load of 100 lbs/foot would be applied as 100/12 = 8.3333 lbs/inch.
  9. Solve.
  10. Retrieve the reactions.
  11. Retrieve the deflection results at each node.
  12. Retrieve the stress and internal reaction results at each node as needed.
  13. Verify solutions using hand calculations remembering that the necessary conditions for equilibrium are SFx = 0, SFy = 0, SM = 0. Also recall that bending stress is the predominate stress in a beam. Bending stress is determined by s = Mc/I.

EXAMPLE: A rectangular beam, 2-inches wide and 6-inches deep is shown in the figure below. Determine the magnitude and direction of the reactions and the deflection and bending stress at the midpoint of the beam. Use E = 1,500,000 psi and 0.24 for Poisson’s ratio.

1.  Start ANSYS using the sequence: Start Button > Programs > Engineering Programs > Ansys 11.0 > Ansys

2.  Select the following from the Main Menu to specify the element type: Preprocessor > Element Type > Add/Edit/Delete

·  Pick the Add… button

·  Specify Beam and 2D elastic 3

·  Pick OK to close the Library of Element Types. Pick Close to

shut the Element Types dialog box. BEAM3 is now element type 1.

3.  Add the real constants to the model using Preprocessor Real Constants > Add/Edit/Delete

·  Pick the Add… button. Type 1 BEAM3 should be listed in the new dialog box.

·  Make sure Type 1 BEAM 3 is selected and pick OK to open the Real Constant for BEAM3 dialog box. Specify area, area moment of inertia and total beam height as shown below.

·  Pick OK, then Close.

4.  Add the material properties to the model using Preprocessor Material Props > Material Models

·  Double-Click each one: Structural > Linear > Elastic > Isotropic for Material Model Number 1.

·  Specify EX = 1500000 psi and Poisson’s Ratio (PRXY) as .24.

·  Pick OK to close the dialog box.

·  Select Material > Exit to close the Define Material Model

Behavior dialog box.

Planning ahead, five nodes will be needed as shown in the figure below. At nodes 1 and 5, a support will be built. At node 2, a load will be applied. At node 3, results are required. The element between nodes 4 and 5 will have a distributed load.

5.  Create nodes using the sequence Preprocessor > Modeling > Create > Nodes > In Active CS

·  Specify node number and X, Y, Z coordinates in the active coordinate system which is a Cartesian coordinate system by default. If the node number is left blank, ANSYS automatically assigns the next number. Pick Apply to set the node and reopen the dialog box for the next node.

·  Repeat for remaining nodes.

Pick OK to set the last node and close the dialog box.

·  The screen should contain 5 numbered nodes.

·  To plot nodes, select from the toolbar menu: Plot > Nodes.

·  To generate a list of nodes, select from the toolbar menu: List > Nodes… Select the Coord. w/Angles button, then OK. The nodes and their coordinates are listed in another window. This list can be saved or copied and pasted in another program such as Word or Excel.

Planning ahead, four elements will be needed:

6.  Create elements using the sequence Preprocessor > Modeling > Create > Elements > Auto Numbered > Thru Nodes

·  Pick node 1 on the screen, then node 2, then pick Apply. Order is important. Choose the i-node, then the j-node – be consistent left to right.

·  Pick node 2, then node 3, then pick Apply.

·  Pick node 3, then node 4, then pick Apply.

·  Pick node 4, then node 5, then pick OK. This creates the last element and closes the dialog box.

·  Four elements should appear on the screen at this point.

·  To plot elements, select from the toolbar menu: Plot > Elements

·  To generate a list of elements, select from the toolbar menu: List > Elements > Nodes + Attributes. The elements are listed in another window by element number. The list contains the material number, element type number, real constant numbers, nodes and other information for each element. This list can be saved or copied and pasted in another program such as Word or Excel.

·  To display node and element numbers, select from the toolbar menu: PlotCtrls > Numbering…

Planning ahead, three support constraints have to be created. A pin is at node 1 which will constrain translation in both the x- and y-directions. A roller at node 5 will constrain translation in the y-direction.

7.  Create constraints (supports) using the main menu sequence Solution > Define Loads > Apply > Structural > Displacement > On Nodes

·  On the screen, select nodes 1 and 5 and pick OK on the dialog box.

·  Pick UY in the DOFs to be constrained window, then OK to apply the supports. These nodes are constrained vertically. UY is ANSYS for displacement in the y-direction. Since the displacement value was applied as zero (empty window in dialog box) the node will not move vertically.

·  Repeat this process by selecting node 1 and applying the UX constraint to it. Blue triangles should appear for each constraint applied to the model.

·  Note that if a fixed support is needed, its node would have UX, UY, and ROTZ all applied.

8.  Create the concentrated load using the Main Menu sequence Solution > Define Loads > Apply > Structural > Force/Moment > On Nodes. Pick node 2 on the screen and pick OK on the dialog box.

·  Set the direction of the force to FY and specify the value of the force as -200 which will represent 200 pounds down at node 2. Pick OK. A red arrow should appear on the model to represent this force.

·  Create the distributed load using the main menu sequence Solution > Define Loads > Apply > Structural > Pressure > On Beams. Pick element 4 on the screen and pick OK on the dialog box.

At this point, the model should look like this:

9.  To solve the model, use the following main menu sequence: Solution > Solve > Current LS. Pick OK from the information box that appears. Pick the Close button when ANSYS indicates that the solution is done. It should take less than a minute to solve simple beam and frame problems.

10.  To obtain beam reactions, use the following main menu sequence: General Postproc > List Results > Reaction Solu. Pick All Items in the window and pick OK.

11.  Get the deflections of each node using the main menu sequence: General Postproc > List Results > Nodal Solu.

·  To plot the deformed shape of the beam, use the main menu sequence: General Postproc > Plot Results > Deformed Shape

12.  An Element Table has to be created to obtain the stress values and internal reactions at the nodes. Use the main menu sequence: General Postproc > Element Table > Define Table. Pick the Add… button.

Quantity at i-Node / Suggested Label / Sequence / Sequence Number
i-node / j-node
Bending Stress / BENDSTR / NMISC / 1 / 3
Bending Moment, M / MMOMZ / SMISC / 6 / 12
Shear Force, V / MFORY / SMISC / 2 / 8
Axial Force, F / MFORX / SMISC / 1 / 7

·  To list the values in the element table use the main menu sequence General Postproc > Element Table > List Elem Table

If a model has more nodes, say one per foot, the MMOMZ values could be copied to Excel to create an XY(Scatter) chart which would be the moment diagram for the beam. Of course, the moment for the last node would have to be added manually.

It should be noted that each of the options used to add items to the model has a delete option which is used to remove the items from the model. Hunt around as needed to use these options. If nodes and elements are deleted from the model, their numbers are automatically reused when new ones are created. Be sure to use the PlotCtrl > Numbering to check the numbers used in the model. The numbers can be compressed by using the menu sequence Preprocessing > Numbering Ctrls > Compress Numbers. For example, if the following are all nodes that are created in a model:

Compressing the node numbers does this:

If you wish to save the ANSYS model, use the File > Save As option. Specify a location and filename.

EXAMPLE: Determine the reactions at the supports and internal pin of the frame shown below. Use E = 29000000 psi, n = .3, A = 1 in2, height = 1, and moment of inertia = 1 in4.

The ANSYS solution for this problem is pretty much the same as it was for the beam. The frame has an additional step.

1.  Start ANSYS.

2.  Specify the element type as BEAM3

3.  Specify the real constants: area = 1, moment of inertia = 1, and height = 1. The stress isn’t going to be determined in this solution, so these numbers aren’t really that important but they can’t be zero.

4.  Specify the material properties: EX = 29000000, PRXY = .3

5.  Create the nodes indicated in the table above. Note that two nodes are needed at each internal pin – point B in this case.

6.  Create the elements for this model as follows:

Element Number / i-node / j-node
1 / 1 / 2
2 / 2 / 3
3 / 4 / 5
4 / 5 / 6

Note that each member of the frame is constructed with two elements. The members are not connected at this point. Before the model can be solved, the translational degrees of freedom for nodes 3 and 4 have to be “coupled”. Use the main menu sequence Preprocessor > Coupling/Ceqn > Couple DOFs to begin the coupling process. Select the two nodes to be coupled. Use the box option in the select dialog box. Pick OK when selected.

·  Specify 1 for the reference number.

·  Pick DOF Label UX

·  Pick Apply

·  Specify 2 for the reference number.

·  Pick DOF label UY

·  Pick OK to apply and close the dialog box.

·  Two green triangles should appear at the internal pin indicating that the two degrees of freedom have been coupled.

7.  Create the pins at A and C. Use UX and UY at both nodes 1 and 6.

8.  Apply the concentrated loads. At node 2, FX = 300 and at node 5, FY = -400.

9.  Solve

10.  List the reaction solutions:

·  To get the forces on all the nodes, use the main menu sequence General Postproc > List Results > Element Solution. Scroll down and click on Structural Forces, then select X-Component of force. Pick OK. The values in this list are the element forces acting ON the node. Show these forces in the opposite directions on the element.