hey everyone welcome to this ncs how-to video engineers perform model analysis to obtain natural frequencies and most 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 the 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's get started [Music] 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 model analysis on a circuit board structure what do you expect from the model analysis is a series of natural frequencies and most shapes that describe the dynamic characteristics of the system however when you check the model results you find that the first several frequencies are zero and the most shapes are showing 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 modes indicates insufficient constraint 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 the circuit board example there's no connection between this square component in the board a typical cost here is improper contact definition so it's always a good idea to check initial contact status using 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 check are much quicker to perform than the 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 do expect rigid body modes in our model solution in engineering there are some applications that do not require boundary conditions for example aircraft fly in the air satellites orbit in space both drift in the ocean to name a few examples the goal of conducting mode analysis for such system is to find out the dynamic characteristics of the system when they are unconstrained and we call such modal analysis free free modern asses in a free free mode 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 one times ten to the minus three hertz 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 six modes represent 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're orthogonal to each other besides the free free mode 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 constraint preventing it from moving freely you can think of the term grounding a way to say that there is some loose connection between the system and the ground behind the scenes and 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 model analysis we expect to obtain six rigid body modes with zero or near zero frequencies if a rigid body mode has nonzero frequency this may mean that grounding exists in the system and the higher frequencies with constraints will be affected too in aces 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 too the solution to eliminate grounding is to switch between different contact formulations provided in this mechanical to make sure we have zero frequencies 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 model analysis the simplified geometry is for demonstration purpose we would like to run the model assets 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 modern asset system on the project page rename it to original model then right click on the geometry cell import geometry browse and pick the file name sample model then double click on the model cell to open aces mechanical we will set the units to the millimeter kilogram 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 lists 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 model analysis first we're expecting six models and zero hertz or near zero hertz go to analysis settings specify max modes to find as 20 and solve using the default setting highlight solution let's check the tabular data for the calculated frequencies note that the frequencies of mode four to six are quite large not close to zero hertz as we expected something is not set up 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 model analysis rename system b to npc then double click on the model cell to open ncs mechanical go to connections expand contacts highlight contact region and change contact formulation to npc then solve let's check the frequencies now we can see the first six modes are all at zero or near zero hertz 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 information 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 factor 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 model analysis right click on model 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 this modal analysis go to the other modal axis with mpc contact defined add the same fixed boundary condition then solve let's compare the frequencies after support has been added for these two mode analysis the original mode analysis results are off from the two values for example if we look at most three we can see an obvious difference in values we can also check the mode shapes for most three go to the npc model select solution right click over mode 3 create more ship results evaluate all results we can see most 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 on the situation for free free mode analysis obtaining up to six 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 modal 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