Customer Training Material. Contact Control. Mechanical. ANSYS, Inc. Proprietary 2010 ANSYS, Inc. All rights reserved. WS3.1-1

Transcription

1 Workshop 3.1 Contact Control Introduction to ANSYS Mechanical WS3.1-1

2 Goals Workshop 3.1 investigates contact behavior on a simple assembly. It is meant to illustrate how rigid body motion can occur as a result of improper contact set up. Problem statement: The model consists of a simple assembly file. Our goal is to set up contact among the parts in the assembly and see how non symmetric loading can effect the results. WS3.1-2

3 Assumptions We ll assume the friction between the arm shaft and the holes in the side plates is negligible. We ll make the same assumption for the contact between the arm shaft and the stop shaft. Finally we ll assume the stop shaft is fixed to each of the side plates. Side Plate Arm Shaft Side Plate Stop Shaft WS3.1-3

4 Project Schematic Open the Project page. From the Units menu verify: Project units are set to US Customary (lbm, in, s, F, A, lbf, V). Display Values in Project Units is checked (on). WS3.1-4

5 ... Project Schematic 1. In the Toolbox, double click Static Structural to create a new analysis system RMB on the Geometry cell and Import Geometry. Browse to Contact_Arm.stp. 2. WS3.1-5

6 Preprocessing 3. Double click the Model cell to open the Mechanical application Set/check the working Unit System: Units > U.S Customary (in, lbm, lbf, F, s, V, A) 4. WS3.1-6

7 ... Preprocessing 5. RMB the Connections branch and Rename Based on Definition. 5. The result is contact regions are now defined with respect to the parts associated with each. Notice the type of contact (e.g. bonded, etc.) is also shown. WS3.1-7

8 ... Preprocessing 6. Based on the assumptions stated earlier change 3 of the contact regions to No Separation as shown here: a. a. Use the CTRL key and select the 3 contact regions shown here. b. In the details change the contact type to No Separation. Each contact region could be changed individually, selecting all 3 merely saves time. b. WS3.1-8

9 Environment 7. Fix the assembly (highlight the Static Structural branch (A5): a. Select the 2 faces on the ends of the Side Plates. b. RMB > Insert > Fixed Support. a. b. WS3.1-9

10 ... Environment 8. Apply a force load to the ArmShaft: a. Select the end line on the top of the ArmShaft. b. RMB > Insert > Force. c. In the force details change to Component d. Set: Y component = - 10 lbf (minus 10) Z component = +1 b. a. c. d. WS3.1-10

11 Initial Solution 9. Highlight the Solution branch (A6) and RMB > Insert > Deformation > Total. 10. Solve (you will see a warning message that the model may be unconstrained). Highlight the Total Deformation to view the result Although slight, we can see the ArmShaft is beginning to move sideways. We have no contact or boundary condition to prevent this motion as it is currently set up. If the magnitude of the load becomes large enough, the solution will fail. WS3.1-11

12 Modified Environment 11. Add a frictionless support to the ArmShaft: a. Select one of the faces on the end of the shaft for the ArmShaft. b. RMB > Insert >Frictionless Support. Either end of the shaft can be chosen. a. b. A frictionless support provides a constraint which is normal to the surface. In this case the shaft will be free to rotate but cannot move out of plane (in this case the Z direction is constrained). WS3.1-12

13 Modified Result Once again solve the model and inspect the deformations. As can be seen the ArmShaft is now prevented from moving. In setting up contact models it is important to assess what motions have and have not, been accounted for. WS3.1-13