Hey, Everyone!
Welcome to this Ansys How-To Video.
Engineers perform Modal analysis to obtain natural frequencies and mode shapes of a given structure.
When analyzing the results of some assemblies or structures, we sometimes come across modes with zero frequency.
We call such modes Rigid body modes.
And the mode shape of a rigid-body mode is simply rigid translation or rotation without distortion.
So how should we evaluate such rigid-body modes?
Are they valid modes that we should consider, or do they directly indicate a mistake in the model?
The answer to such questions totally depends on the purpose and the application of the simulation.
There are some situations where rigid body modes are expected, and there are times they are undesired and should be eliminated.
In this video, we will explore different cases where we evaluate and treat rigid body modes.
Now, let us get started!
As we mentioned earlier, we may or may not want rigid-body modes.
Let’s first start with the case where rigid-body modes are undesired.
Imagine that you need to perform modal analysis on a circuit board structure.
What you expect from the modal analysis is a series of natural frequencies and mode shapes that describe the dynamic characteristics of the system.
However, when you check the modal results, you find that the first several frequencies are zero.
And the mode shape shows something not realistic at all.
It seems all the deformation is localized on one electronic component, and it’s not connected to the rest of the circuit board.
Something must be wrong here.
Usually, this kind of rigid-body mode indicates insufficient constraints to the model.
It could be a lack of properly-defined connections between different parts that allows those parts to undergo rigid-body motion.
As we see in this circuit board example, there’s no connection between this square component and the board.
A typical cause is improper contact definition, so it’s always a good idea to check the initial contact status using the Contact Tool before solving.
For more details, please see our video on “Checking Initial Contact Conditions Prior to Solving”.
Doing so will save a lot of time, as the initial contact checks are much quicker to perform than a regular model analysis.
As you can see here, the contact pair highlighted in red indicates an open contact, which needs to be addressed.
Now, let’s move on to the case when we may expect rigid-body modes in our modal solution.
In engineering, there are some applications that do not require boundary conditions.
For example, aircraft fly in the air, satellites orbit in space, boats drift in the ocean, to name a few examples.
The goal of conducting modal analysis for such systems is to find out the dynamic characteristic of the system when they are unconstrained.
And we call such modal analyses free-free modal analyses.
In a free-free modal analysis, the first six natural frequencies are expected to be zero or close to zero.
Note that usually if the frequency is in the range of 1e-3 Hz, we view it as being essentially zero.
The first six zero natural frequencies represent the six rigid body modes in three translational directions and three rotational directions.
As you can see, for this toy airplane, the first 6 modes present rigid body motion of the entire structure.
Note that the motion of the six rigid-body modes don’t have to be aligned with the global Cartesian coordinate system,
as long as they are orthogonal to each other.
Besides the free-free modal analysis, there’s another situation where engineers may expect rigid-body modes, that is for checking if Grounding exists in a system.
So what is Grounding?
Grounding refers to a system that has some artificial internal constraints, preventing it from moving freely.
You can think of the term “Grounding” a way to say that there’s some loose connection between the system and the ground behind the scenes.
And it is a side effect of some numerical methods used in the finite element simulation.
If grounding exists, it means the modal results of the current system are not accurate, because grounding can affect the stiffness matrix of the structure.
The way to identify grounding in a system is to first suppress all the supports, or boundary conditions, and run a modal analysis.
We expect to obtain only 6 rigid-body modes with zero or near-zero frequencies.
If a rigid-body mode has non-zero frequency, this may mean that grounding exists in the system.
And the higher frequencies with constraints will be affected, too.
In Ansys Mechanical, one common source of Grounding is Bonded contact with relatively large, non-uniform gaps.
Also, some MPC formulation options for bonded contact can lead to Grounding.
The solution to eliminate grounding is to switch between different contact formulations provided in Ansys Mechanical to make sure we have zero frequency values for rigid-body modes.
Now let’s have a look at a model where rigid body modes and grounding are addressed.
For this lesson, we have two simplified parts with a non-uniform gap in between to illustrate the concepts of rigid-body modes in a modal analysis.
The simplified geometry is for demonstration purposes.
We would like to run a modal analysis to check if contacts are correctly configured for this model with non-uniform gaps.
So, let’s proceed with this example.
First, drag and drop a Modal analysis system on the project page.
Rename it to “Original model”.
Then, right-click on the geometry cell, Import Geometry, Browse, and pick the file named SampleModel.
Then, double click on the model cell to open Ansys Mechanical.
We will set the units to the (mm, kg) for this simulation.
If we expand the geometry, we can see the materials for both parts are structural steel.
We will leave it as it is.
Then, go to Connections, expand the connections and contacts, we can see the bonded contact is automatically created between the two parts, we will leave it as it is.
The two parts touch each other only in the center and are bonded there.
However, the bonded contact is defined over the entire surface where the majority of the region is separated by a non-uniform gap.
We would like to check if contacts are correctly configured in this model.
To do this, let’s generate the mesh first, so for that, right click on Mesh and select “generate mesh.”
There should be a fixed boundary condition on the bottom surface, but, we will omit all the boundary conditions defined in this model and run a modal analysis first.
We are expecting 6 models at zero Hz or near zero Hz.
Go to Analysis settings, specify Max Modes to find as 20, and solve using the default settings.
Highlight Solution, let’s check the Tabular Data for the calculated frequencies.
Note that the frequencies of mode 4-6 are quite large, not close to zero Hz as we expected.
Something is not setup correctly, and by examining the model, we notice the bonded contact has non-uniform gaps.
Let's try MPC contact formulations.
Go to Workbench, Duplicate the modal analysis, rename system B to “MPC”, then, double click on the model cell to open Ansys Mechanical.
Go to connections, expand Contacts, highlight contact region, and change contact formulation to MPC.
Then solve.
Let’s check the frequencies.
Now we can see the first 6 modes are all at zero or near zero Hz.
We can see that the MPC contact formulation works much better for this model with a non-uniform gap.
If we compare other modes, we can see differences as well.
The difference tends to be more significant if the mode is associated with deformation in the contact region.
Let’s go to solution information, Solution output, change it to participation factor summary.
What we note here is that, when we have rigid-body motion, the evaluation of participation factors becomes less meaningful due to the dominance of the rigid-body modes.
Now, Let’s add the fixed boundary condition back and run the model again.
Go back to the original modal analysis, right click on Modal, Insert a Fixed Support.
Pick “Face” selection filter and select the bottom surface.
Click Apply for the Geometry Scoping to define the Fixed support.
Solve the modal analysis.
Go to the other modal analysis with MPC contact defined, add the same fixed boundary condition.
Then solve.
Let’s Compare the frequencies after the support has been added for these two modal analysis.
The original modal analysis results are off from the true values.
For example, if we look at mode 3, we can see an obvious difference in values
We can also check the mode shapes for mode 3, go to the "MPC" model, select Solution, right click over mode 3, Create mode shape results.
Evaluate all results.
We can see mode 3 is in the direction of contact, so this explains why we see a bigger difference for this mode.
To summarize this lecture, evaluation of rigid body modes depends upon the situation.
For free-free modal analysis, obtaining up to 6 rigid body modes is expected because the purpose here is to calculate the modes when the system is fully or partially unconstrained.
Another situation is when we are performing a Grounding check for a system.
What we do is temporarily suppress the constraints to see if we get the expected rigid body modes.
In either case, if any rigid-body modes have non-zero frequencies, we should check and correct the model setup, such as reviewing the contact definitions.
On the other hand, if rigid-body motion is not desired, our goal is to make sure that sufficient boundary conditions or appropriate contact settings are included in the system, so that zero frequencies are eliminated.
I hope you have found this video informative.
Thank you for watching and please check out our other courses to discover more useful learning resources.