Plane Stress example problem

 

Given: The wrench shown is made of a steel with a yield strength of 45,000 psi. and is loaded with a pressure of 150 psi. along its handle as shown. It is 0.4 inches thick and about 7 inches in length.

 

Find: Determine if any yielding occurs because of this load.

 

Solution: The geometry was created in Pro/E, saved as an IGES file and imported into ANSYS 6.1. The plane2 6 node triangle element, plane stress with thickness option was used in the modeling.

 

Material properties were E = 3.e7 psi, nu = 0.3.

 

 

Boundary conditions ux = uy = 0 were applied along the lines where the wrench contacts the bolt.

 

The mesh was refined to eliminate element-solution stress contour discontinuities. The following plots of von Mises stress show a maximum value of 39,333 psi at the fillet radius on the underside of the wrench.

 

Data entered Interactively:

 

Element Type:

 

LIST ELEMENT TYPES FROM      1 TO      1 BY      1

 

 ELEMENT TYPE      1 IS PLANE2       2-D 6-NODE TRI. STRUC. SOLID   INOPR

  KEYOPT(1-12)=    0  0  3    0  0  0    0  0  0    0  0  0       0

 

 CURRENT NODAL DOF SET IS  UX    UY 

  TWO-DIMENSIONAL MODEL

 

Thickness:

 

LIST REAL SETS       1 TO       1 BY       1

 

 REAL CONSTANT SET       1  ITEMS   1 TO   6

   0.4000   0.0000       0.0000       0.0000       0.0000       0.0000

 

Material Properties:

 

EVALUATE MATERIAL PROPERTIES FOR MATERIALS      1 TO      1 IN INCREMENTS OF      1

 

 MATERIAL NUMBER =      1 EVALUATED AT TEMPERATURE OF   0.0000   

  EX   =  0.30000E+08

  PRXY =  0.30000

 

 

(Note: To properly document the model, the axis system, loads and boundary conditions are shown on this plot.)

 

 

Results:

 

The maximum von Mises stress, SEQV = 39,333 psi, is less than the material yield strength of 45,000 psi, so no yielding is likely to occur.

 

 

(Note: In some cases it may be necessary to identify stresses or strains at critical elements and/or nodes, turn on element or node numbering and list the computed values at those locations as shown in ANSYS Tutorial Fig. 3-10. In the above we just used the contour plot legend.)