Surface to Surface Contacts

Build a cantilever beam (10-inch x 0.5-inch, Part 1, Aluminum 6061) and force a wedge (0.5-inch to 0.75-inch thick taper, 4-inch long, Steel A-36) under the end. Perform a 2D analysis.

This example only covers setting up and performing the analysis. For instructions on building the model, see Surface to Surface Contact Model. If you did not build the model, you can open the surf2surf_input.ach file in the Models subfolder of the Autodesk Simulation installation directory.

  1. Place the restraints on the cantilevered beam. Use Selection Shape Rectangle and Selection Select Vertices to select the nodes at the left end of the beam. Right-click and select Add Nodal Boundary Conditions. click Fixed and then click OK.
  2. Restrain the wedge in the vertical direction. Select the nodes along the bottom of the wedge. Right-click and select Add Nodal Boundary Conditions. Activate the Tz check box and click OK. The 2D wedge is free to move in the Y direction.
  3. To simulate pushing on the wedge, apply one prescribed displacement to the 0.75-inch face of the wedge. Select the vertex at the middle of the right vertical edge of the wedge. Right-click and select Add Nodal Prescribed Displacement. Type -4 in the Magnitude field and select Scalar Y. Click OK to apply the prescribed displacement.
  4. Set the element type for both parts. In the tree view, click the Element Type heading for Part 1, hold the Ctrl key, and click Element Type for Part 2. Right-click and select the 2D command.
  5. In the tree view, click the Element Definition heading for Part 1, hold the Ctrl key, and click Element Definition for Part 2. Right-click and select the Edit Element Definition command. Type 1 in the Thickness field.
  6. In the tree view, right-click the Material heading for Part 1 and select the Edit Material command. Expand the Aluminum folder, select the Aluminum 6061-T6; 6061-T651 item and click OK.
  7. In the tree view, right-click the Material heading for Part 2 and select the Edit Material command. Expand the Steel ASTM folder, select the Steel (ASTM-A36) item and click OK.
  8. Using Selection Shape Point or Rectangle and Selection Select Surfaces, click the bottom surface of the beam and the top surface of the wedge. Right-click in the display area and select Contact Surface Contact. This creates an entry in the tree view. Click Enter to accept the default name.
  9. Right-click the Analysis Type heading in the tree view and select the Edit Analysis Parameters command.
  10. Assume that the wedge will be pushed under the beam in 1 second. Type 1 in the Duration field and 100 in the Capture rate field.
  11. The load curve controls the motion of the prescribed displacement. To ramp the motion over 1 second, enter the following load curve. Since the magnitude of the prescribed displacement is four inches, the wedge will be pushed four inches.

                 Time

                   Multiplier 1

    0 0
    1 1
  1. Click the Output tab. To see how much force is required to push the wedge, activate the check boxes for Output reaction forces and Nodal reaction forces due to contact.
  2. Click OK.
  3. Run the analysis: use Analysis Analysis Run Simulation. As each step is calculated, the results are displayed in the Results environment.
  4. In the Results environment, select Results Contours Other Results Reactions Reaction Force (Negative) Y to review the reaction force results.
  5. Select the node to which the prescribed displacement was applied. Right-click in the display area and select the Graph Value(s) command. This will open a new presentation window and graph the reaction force at that node throughout the analysis.
  6. Click the 1 <Stress> presentation in the tree view to return to the contour display. Use Results Contours Stress von Mises to view the stresses.

The results obtained should be approximately as follows. (Different versions may have different default values for the surface to surface contact which can cause slight differences in the results.)

An archive of this model (surf2surf.ach) is located in the Models subfolder in the Autodesk Simulation installation directory.

Parent topic: Mechanical Event Simulation