Using Thermal Boundary Conditions in SOLIDWORKS

Using Thermal Boundary Conditions in SOLIDWORKS
Simulation to Simulate a Press Fit Connection
Simulating a press fit condition in SOLIDWORKS Simulation can be very challenging when there is a
large amount of interference between interfacing components. This type of analysis requires a
nonlinear study to capture the large deformations induced by the press fit. There is a no
penetration contact condition that can be used for simulating press fit connections. It is referred
to in the software as a shrink fit condition. When running a nonlinear analysis or a linear static
analysis with the large displacement option enabled, the solver will solve for the shrink fit
condition in the first time step. Depending on the amount of interference, there are situations
where the solver cannot successfully perform the calculation. In these cases, the press fit
condition has to be simulated through other means. Another approach is to apply thermal
boundary conditions to simulate the contraction and expansion of the interfacing components.
This document will cover the workflow of using thermal boundary conditions to successfully
simulate a press fit connection when the shrink fit boundary condition is unsuccessful.
Model Specifics
In this example, the analysis involves a 2 inch diameter round shaft press fit into a bracket with a
1.9 inch round hole. Since the model and the loading are quarter symmetric, a quarter of the
model will be used for the analysis setup.
888.688.3234 | GOENGINEER.COM
Nonlinear Analysis with Shrink Fit No Penetration Contact Condition
Two fixtures were applied to the model. A symmetry fixture was applied to the four surfaces
created by the symmetry cut. This fixture restrained two degrees of freedom. To restrain the
third degree of freedom and prohibit rigid body motion, a use reference geometry fixture was
applied to a single vertex on each component to limit the axial translation. A plane was used for
the reference entity and the normal to plane translation was set to zero. A shrink fit no
penetration contact set was setup between the cylindrical faces of the interfacing components.
888.688.3234 | GOENGINEER.COM
The analysis failed due the large interference between the interfacing components. The warning
that displayed in the nonlinear solver dialog window was: Incremental plastic strain is too large;
Automatic reset. There was too much displacement in the initial time step for each component
and the solver could not satisfy equilibrium constraints.
888.688.3234 | GOENGINEER.COM
Nonlinear Analysis with Thermal Boundary Conditions
In this analysis setup, the shaft was moved axially so that there was no initial contact between the
components. A symmetry fixture was applied to the four surfaces created by the symmetry cut.
This fixture restrained two degrees of freedom for each component. To restrain the third degree
of freedom for the bracket model, an on flat face fixture was applied to one of its surfaces
restraining the movement in the normal direction.
A temperature load was applied to the bracket body heating it up from 75 °F to 500 °F. The
purpose of this load was to expand its hole to be larger than the shaft diameter. The reference
temperature at zero strain study setting was set to 75 °F. This specified that there were no
displacements caused by thermal loading at 75 °F. The thermal expansion coefficient for the
bracket material was increased so that the body would more easily thermally expand. A time
curve was setup to control the heating and cooling of the bracket component.
888.688.3234 | GOENGINEER.COM
Since the component was not restricted from thermally expanding in any direction, the von Mises
stress magnitude after the bracket was heated up to 500 °F was zero.
After the bracket was heated up to 500 °F, the shaft was moved axially to be centered within the
bracket hole. This was accomplished by using another on flat face fixture applied to one of the
shaft surfaces. It was held stationary until the bracket was heated to 500 °F and was then moved
into position through the use of a time curve. The temperature of the bracket component was
then gradually decreased inducing contact between the bracket and the shaft allowing for the
shrink fit connection to develop.
888.688.3234 | GOENGINEER.COM
The following screen shots display the radial displacement and von Mises stress after the thermal
load has been removed from the bracket component.
888.688.3234 | GOENGINEER.COM