Hello and welcome!
Gravitational acceleration can be included in a static analysis.
But it may be a bit confusing for new users since parts should not move or accelerate in a static analysis.
In this video, we will discuss different types of inertial loads
like acceleration, rotational velocity, and rotational acceleration
and what inputs are needed for their definition in a static analysis.
Ready? Let's get started!
The material selection and definition of its properties is the first step of any finite element analysis.
For a Static Structural analysis on the Workbench Project page,
we have a default material of Structural Steel already defined under Engineering Data.
And it has the necessary material parameters defined for us to carry out the stress analysis.
Additionally, we can also choose pre-defined materials from various libraries under the Engineering Data Sources.
We can add these materials to the project and then assign them to the appropriate parts in the Mechanical interface.
But, what if we want to create our material?
Do we need to define the value of every material parameter when creating any new material?
Or is there a minimum set of material coefficients required to carry out a static structural analysis?
For any new material, we need at least two material parameters –
Elastic Modulus and Poisson’s Ratio – to perform static structural analysis.
The Elastic or Young’s Modulus characterizes the stiffness of a material when a force is applied to it.
It explains the relationship between stress and strain in the linear elastic region of a stress-strain curve.
The Modulus of Elasticity is the slope of stress vs strain.
The second important material parameter is Poisson’s Ratio.
It is a measure of the deformation of a material perpendicular to the loading direction.
It can be defined as the ratio of transverse or lateral strain to the axial or longitudinal strain.
With these two properties and geometry, we can fully describe the linear elastic behavior of any part.
However, what if we want to also include inertial loads for our simulation,
for example, gravity, that affects the entire body based on the mass?
In such cases, we also need to include density in the material definition.
With density and having the geometry that provides the volume,
we can derive the mass of the bodies for inertial loads.
Here is a process to create a new material and add the material parameters.
First, add the material in the list and then drag and drop the required parameters
on the material and specify the values along with correct units.
In terms of the inertial loads available for our simulation, Ansys Mechanical provides several.
Let us try to understand them one by one.
The simplest one is the Standard Earth Gravity.
It is used to model the gravitational effect on a body in the form of a force, or weight.
Gravity is a specific example of acceleration with a fixed magnitude of 9.8 m/s^2,
and it causes the body to move in the direction of gravity.
The next one is Acceleration to define an arbitrary acceleration field for a structure.
Think of being in a car that is undergoing constant acceleration,
and our frame of reference is moving with the car.
Thus, for applied acceleration loads, a body tends to move in the direction opposite to
the acceleration direction since we are in that moving reference frame.
So, we need to pay special attention to the direction.
Thus, Gravity and Acceleration are essentially the same types of load
except gravity has a fixed magnitude, and the sign convention differs
since Gravity is in a stationary frame of reference while Acceleration is in a moving frame of reference.
Then, we have Rotational Velocity for considering the structural effects of a part spinning at a constant rate.
For Rotational Velocity defined in a Static Structural analysis,
the spin softening effect is automatically included in the rotating reference frame.
For Rotational Velocity, the forces are generated along the radial direction,
so the relative movement is in the radial direction for an axisymmetric structure.
The Rotational Acceleration applies a constant rotational acceleration to the selected bodies.
For the Rotational Acceleration, the forces are generated in the perpendicular direction to the radial direction
and hence we see the relative movement in the circumferential direction.
In a static analysis, using rotational velocity or rotational acceleration does not mean that
we are calculating the actual rotation of the parts.
Here, we assume, by default, a rotating frame of reference.
It is as if we are rotating with the structure.
We can use a stationary frame of reference in rotordynamics analyses,
but it is outside the scope of this lesson.
Let us try to understand how these terms differ in Static vs Dynamic analysis.
First, let us see the governing equation of motion.
In the static analysis, acceleration and velocity terms are zero
as the loads and structural response don’t change with time.
So, we only have kx = F, where inertial loads are included in the F term.
While the part’s acceleration is zero, the structure may be in an acceleration field,
like gravity, so ma, or more precisely, mg = F is acting on the part
and appears on the right side of the equation.
Therefore, in a static analysis, inertial loads are treated as loading or part of {F}.
In the static analyses, we will not calculate a part actually moving –
in cases of Acceleration, Rotational Velocity, or Rotational Acceleration,
we should know that we are interpreting the results in a moving frame of reference.
Let’s now consider dynamic analysis – in this case, the loads and structural response change with time.
So, the acceleration term is unknown, and it is the second time-derivative of DOF.
Dynamic analyses are used to include and calculate these inertial effects,
meaning that the contribution [𝑚]{𝑥¨} is unknown and may change with time.
Unlike inertial loads, we can’t treat this term as known force {F},
so that is why it remains on the left side of the equation and is calculated by the solver.
We can think of this like a ball hitting a bat.
The ball may start with a constant acceleration but contact with the bat will change the magnitude
and direction of the ball’s acceleration, which needs to be computed by the solver.
With this understanding, let us perform a simple static analysis.
For this lesson, we have the geometry of a very simplified wind turbine blade to illustrate the concepts of inertial loads.
We simplified the geometry for demonstration purposes, as the actual assemblies are more complex
and can have dozens to hundreds of parts with contact.
The wind turbine would be attached to a shaft, which is not modeled here,
and fixed support is applied to the wind turbine as an approximation.
Then a rotational velocity of 1.5 rad/s is applied.
We assume a rotating frame of reference when reviewing the results.
Imagine that we are rotating with the turbine blade.
So, let’s proceed with this example.
First, drag and drop a Static Structural System on the Project Page.
Then right-click on the geometry cell, Import Geometry, Browse, and pick the file named Rotor_Blade.scdoc.
Then, double click on the model cell to open Ansys Mechanical.
We will set the units to Metric (mm, kg, N, s) for this simulation.
If we expand the geometry, we can see the material for the Blade is Structural Steel.
We will keep it as is.
Then, go to Coordinate Systems, right-click, insert Coordinate System.
For this workshop, a cylindrical coordinate system will be defined,
so that the axial, circumferential, and radial displacements can be reviewed after solving the case.
In details of Coordinate Systems, change the type to Cylindrical.
Select the “Face” selection filter and select the end surface of the blade connecting to the shaft and click Apply.
For the Principal Axis, choose Axis as Z and Define by Global Y-Axis.
Now the cylindrical coordinate system is defined.
Let’s generate the mesh, so for that right-click on Mesh.
For the Element Size, specify 50 millimeters under the Mesh Details.
Now, right-click on Mesh, and Generate Mesh.
Now, we will set up the model with boundary conditions and inertial load.
First, right-click on Static Structural, Insert a Fixed Support.
Pick the “Face” selection filter and select the end surface of the blade.
Click Apply for the Geometry Scoping to define the Fixed support.
Right-click on Static Structural again and Insert the Inertial Load of Rotational Velocity.
Now, pick the “Body” selection filter.
Select all geometry and click Apply.
Then, set Define By to “Components” and set 1.5 rad/s for the Y-component.
Now, we are ready to solve the model.
Right-click on solution and Solve.
As the solution is done, let’s first check the stresses in the blade.
Right-click on the solution, insert, stress, equivalent.
Evaluate the results to view the stresses that developed on the blade.
Now let’s check the displacement.
For that, right-click on Solution, Insert Directional Deformation, choose X-Axis.
Here, for the Coordinate System, choose the cylindrical coordinate system that was created earlier.
This will give us radial displacement.
Repeat this for Y and Z direction to get circumferential and axial displacement respectively.
We can hold the Shift button and select the X, Y, and Z directional deformations that
we just inserted and then right-click to Rename based on Definition.
This will make it easier to identify each result object.
Right-click and evaluate all results to view all directional deformations.
For a simple disc with rotational velocity, we may expect uniform radial motion,
but deformation, in this case, is not purely radial since this is not an axisymmetric structure.
Due to its geometric shape, the blades bend circumferentially in the rotating frame of reference.
We also notice there is an out-of-plane deformation component, too, due to the shape of the blades.
So, let’s summarize the key learning points.
Defining proper material properties is essential for carrying out a finite element analysis,
of which the bare minimum are Elastic modulus and Poisson’s ratio.
But if inertial loads are taken into consideration, then the density also needs to be defined.
We discussed various inertial loads including Standard Earth Gravity, Acceleration, Rotational
Velocity, and Rotational Acceleration, providing the foundation for our understanding of realistically representing inertial loads.
Remember that some inertial loads may need to be interpreted in the context of a moving reference frame.
We also discussed how the equation of motion varies for static and dynamic analysis.
For Static analysis, we assume acceleration and velocity terms as zero,
so we are left with [K]{x} = {F}, and the inertial loads are included in the {F} term.
For Dynamic analysis, acceleration is unknown and is defined as the second time-derivative of DOF.
I hope you found this video informative to understand the inertial loads.
Don’t forget to visit courses.ansys.com to discover more useful courses.