Hello, in this video from the Ansys How To series, we will discuss
• What is interference fit and where is it used?
• How to set it up in Ansys Mechanical? • And how to post-process and interpret the results?
Let's go!
An interference fit is created when two or more parts have geometric penetration between them.
We use contact algorithm to detect this penetration and apply contact forces to push
the parts apart until there is no more penetration.
In this process, the parts may deform, develop
compressive stresses, and create a contact pressure between the two parts.
This contact pressure is often used to establish connection between different parts called
as a press-fit or friction fit where the frictional force between them resists the applied forces.
The performance of such joints depends on the tightness of the fit which in turn is
directly dependent on the amount of initial penetration.
The same concept is often extended to other modeling applications such as installation
of gaskets and O-rings. So, how to setup and solve interference fit in Ansys Mechanical?
Well, I’ll show you how to do that.
So here’s the model for a pin and a hole, the radius of the hole is 0.49 mm, and the
radius of the pin is 0.5 mm, a little larger than that of the hole. So, when the pin is
installed in it, an interference fit is created.
We can inspect this in the geometry in section view.
Now, let’s setup the contact pair for this
interference fit. Insert a contact group and insert a contact object for this pair.
Pick the contact and target surfaces for the contact pair.
The contact and target designations describe two sets of surfaces that may come in contact with each other,
where the contact points can't penetrate the target faces.
Let us go ahead and pick the surface.
In this case, since both, the sides have similar material properties and geometry,
let us go ahead and pick the surface of the pin as contact and the surface of the hole as the target side.
We’ll leave the contact behavior to be program controlled so the solver can swap the sides
if it deems necessary. By default, the contact type is set to Bonded
which implies that there is no relative motion between the two surfaces. However, as the
interference is resolved, there is a relative motion between the contact and the target surfaces.
So, it should be set to one of the nonlinear contacts, in this case we’ll pick
a frictional contact and set the coefficient of friction to be 0.2.
Now we would like to set up two contact parameters for interference fit analysis, pinball radius
and Interface treatment.
Insert Contact Tool to generate initial contact results.
From Initial Information we can observe that contact is initially closed and that
there is a geometric penetration of 0.01 mm which is the true geometric penetration or
geometrically imposed interference.
Notice that resulting pinball region by default
is bigger than the geometric penetration. Pinball radius should be bigger than the geometric
penetration, this is because the solver can detect the contact only if both the contact
and target surfaces are within pinball radius.
Now let us see what change happens to the
contact initial information if we reduce the pinball radius to 0.005mm.
The contact status changes to open with no interference.
If we increase the pinball radius to 0.015mm which
is bigger than the interference, the contact status is closed with interference of 0.01mm.
Under contact, there are three options available for the Interface Treatment.
This contact parameter defines how the contact interface of the contact pair is treated.
The first option, “Adjust to Touch” is used when there’s an interference or gap
between the surfaces in the geometry that is not intended to be physical. In that case,
With the “Add Offset, Ramped Effect”, the interference is resolved within one full
load step, which is recommended for nonlinear, large deflection analysis.
Setting this option to “Add Offset, No Ramping”, the solver would try to resolve the full interference
in only one substep, which may be challenging to solve especially when nonlinearities are prominent.
So, in this case we’ll set this option to “Add Offset, Ramped Effects”.
Next we will define Analysis Settings
Interference fit is usually resolved in the
first load step where no other external loads are applied.
Any external loads such as displacements,
forces or pressure loads should be applied in the following load steps.
In this example, we’ll define a displacement load to simulate the pin pull out, so we’ll use two load steps.
It’s recommended to turn auto time stepping ON
so the interference can be resolved gradually so the solver can capture any path dependent
behavior and for better numerical convergence.
Define the substeps for each load step (25-10-100,
100, 10,10000). These numbers are picked such that the solver has enough room to adjust
the load increment in case it has trouble with convergence or, conversely, to increase
the load if it's easy to converge. Turn ON the large deflection as this is a nonlinear
simulation.
We intend to calculate the contact forces
in this case so set up output controls for extracting contact forces – Go to Output
Controls and Turn on the nodal forces to yes.
This is needed to extract the force reaction
for the contact for post processing. Everything else is left as “Program Controlled”.
Next, let’s define boundary conditions – Apply a Fixed Support to the plate and a Displacement
boundary condition to the Pin. The Pin is constrained in X,Y direction to arrest any
rigid body rotation about its axis. It is constrained in Z-direction in first load step
but set it to a value of 1.7 mm in the second load step where it is pulled out axially.
That completes setting up of the model so let’s go ahead and solve it.
During the solution we can monitor the status via Solution information.
Solver output shows the solver log file along with any warnings or errors.
The Force and Displacement Convergence graphs show convergence pattern for each substep and load step.
Deformation and Stress plot trackers can be inserted to monitor deformation and stress during the solution.
These tools help us track both the convergence pattern and the accuracy during solution process.
Once the solution is done, we can postprocess results.
Insert Total Deformation and Equivalent Stress plots.
Insert Equivalent Stress result for the first load step.
A maximum equivalent stress of 4200 MPa is developed in the plate
due to press fit. Now, animate the total deformation across
all the substeps and load steps, we can see that the surface of the hole is pushed away
from the surface of the pin to resolve the interference.
Now, we would like to examine the contact results using Contact Tool.
Insert contact pressure, penetration, and frictional stress.
Specify the load step for which you would like to check the results.
We can see contact status, pressure, penetration and frictional stress for the first load step.
- In the first load step the contact status is “sticking” and contact is closed
- We can see that the contact pressure gradually
developed from 0 to about 3000N. This is the first load step as the interference is resolved.
- This correlates with the Contact penetration which is also increasing in the first load step.
It is important to understand that the interference is not the same as the penetration.
The interference is referred to the overlap in geometry which is physical
whereas the penetration is a numerical adjustment. The contact algorithm is calculating the amount
of force necessary to resolve the interference.
The solver decreases the interference gradually
by internally moving the contact surface.
As the interference is ramped,
the contact force linearly increases.
This force is equal to the contact stiffness times penetration
so, if we keep the stiffness constant the penetration is increasing which is exactly what
we see in the first load step.
- Next, we observe that the Frictional stress
in contact is small during the first load step keeping the pin from sliding during the
interference resolution.
Insert Probe to examine Force Reaction for the Displacement boundary condition.
Duplicate Force Reaction feature and change location method to Contact region and scope to the frictional contact
Set the Result Selection to Z axis, to see contact reaction force in Z direction.
The reaction force in Z direction due to the Displacement boundary condition at the onset
of load step 2 shows how much force is needed to pull out the pin, it starts to decrease
as pin slides out of the hole. Eventually the reaction force drops to zero.
The contact reaction force is small in the first load step. The frictional force is keeping
the pin from moving during the interference resolution in the first load step. In the
second load step the frictional force is high, so to be able to pull the pin from the hole
the axial force of about 830N would be necessary.
In conclusion, the procedure presented in this video is applicable for most interference
fit problems . The key contact settings are to use a nonlinear contact, a big enough pinball
radius, select the appropriate interface treatment.
Other settings such as mesh density, loads
and boundary conditions and analysis settings can be picked similar to other nonlinear finite
element analyses.
I hope this video answered your questions
about How to set up and solve interference fit problem in Ansys. Hope to see you next
time on our next topic. Bye for now.