Hello! Today we will begin with part one of a three-part series on friction heating during
braking. This series is intended for Ansys users with previous knowledge and experience in building
FEA models. Part 1 will cover our geometry materials moment of inertia contacts and mesh.
Part 2 will cover model setup and kinetic energy verification and Part 3 will cover
post-processing results. So to get started! Let's take a look at our assembly our model
is comprised of minimal geometry including the brake pads and rotor. The pads are made of two
pieces a steel backing plate and a ceramic friction pad. Our rotor is a multi-body part
consisting of the frictionally slash thermally significant portions and the inertially
significant portions with altered densities. Using our geometry and densities we can make preliminary
estimates of the rotational inertia before starting the analysis. These can assist in making
minor adjustments to the density of the initially significant components so we can approach Target
values before verifying and Mechanical. In this example a slightly lower principal moment about
the y-axis is predicted but with an error of less than one percent based on Mechanical calculations.
Moving over to workbench we're going to be using a coupled field transient
analysis system. This will be found on the left side of your menu and if not there we
can always go to view all and add it by clicking the check mark. Moving over to Mechanical we can
start by reviewing our geometry. Here we check the rotor to see that topology sharing is active
which it is and then going down to the properties option in the details view we can check the moment
of inertia about the principle 1 2 and 3 axes. Next we verify our material assignments to ensure
non-thermal portions of the model have altered densities. Here we're using an insert material
assignment to scope them to each component accordingly with modified densities assigned
and labeled accordingly. We do this to ensure the thermally significant portions of the model have
the appropriate material properties so the thermal conductivity values are preserved.
Closing the geometry and materials tabs we can start reviewing our connections
or contacts throughout the model. We'll start with the revolute joint applied to the rotor.
This is going to be used to apply that acceleration input and rotate our model
up to our desired RPMs. Of note is the reference coordinate system here
which we need to orient so that our blue RZ free rotation is possible in the proper direction.
Moving on we have our frictional contacts between the brake pads and the rotor.
A couple of details on the setup are the fact that we have a friction coefficient of 0.25
we have small sliding off due to the fact there's a large amount of sliding in this
model and we have increased our normal stiffness factor to 10. This is so there's not a lot of
penetration between the contact and the target and thus the sliding can perform appropriately.
The thermal conductance value here is set to manual but this is the default value
applied by Ansys and then within each of these contacts we actually have command Snippets.
Here you'll see the first one KEYOPT, CID, 1, 1. This is critical in the fact that this
opens up the thermal degree of freedom within our contact. Next, we have the RMODIF 15 and 18.
RMODIF 15 designates what percentage of energy is converted into thermal energy during friction
and here we have it set to 1 or 100 percent. RMODIF 18 is the ratio of how much energy is
put into the contact side of our contact and the target side of our contact. Here a value of 0.5
designates the fact that 50% will go to our contact and 50% will go to our target.
Next, we'll move down we have two bonded contacts in between our backing plate and our friction pad
just to keep them together and then we have our two joints. These are applied to the
outside of our brake pads and they are allowing translation in the X direction. Again this is
reference to the reference coordinate system which we set up ourselves and this is going
to allow us to apply pressure or a force onto each pad to create that friction for stopping.
Moving ahead we'll do a quick overview of our mesh settings. Nothing here is essentially
critical except for the face mesh between the router and the pads. This is why we're
using a hexagonal mesh because we want a nice structured surface for our contacts to work on.
From here you'll want to go to part two of our three-part series focusing on
model setup and kinetic energy verification. Thank you for watching and have a nice day.