Welcome to this video to discuss selecting the geometry and level of detail to include in simulations.
Numerical simulations provide an efficient way for engineers to evaluate and gain insight into their designs.
However, the first step is to identify the geometry and level of detail to include.
For example, if we were to design a brake pad for a car, can we have just the geometry of the brake pad?
Or do we need to model the entire braking system?
Do we even need to include the entire geometry of the car or even the geometry of the road?
The objective of the analysis determines the level of geometric detail we need to include for an efficient yet accurate solution.
We do not want to model an entire world just to evaluate the performance of a brake pad,
but we may not be able to simulate the brake pad in isolation accurately if interactions with other parts need to be considered.
In this video, we will explore the thought process and workflow for the specific case of performing stress analyses.
Ready? Let us go!!
Before getting started with any analysis, we need to address some important questions, such as how much geometry should we include?
To understand this question, we need to first identify the critical parts of interest and to determine the load path of the analysis.
Considering the load path will help us understand where the loads are coming from,
what the system is attached to, and whether we need to include additional geometry.
For example, do we need to include the rest of the airplane attached to the landing gear if we are only interested in performing stress analysis of the landing gear?
For the landing gear, where are the loads coming from, and do I need to represent such geometry, like the runway?
On the other hand, instead of considering additional parts, not in our CAD model,
we may want to ask if the CAD geometry we already have has more parts than we need for the simulation.
If we are only interested in the performance of a component or sub-assembly, can we simplify other parts that are not of interest?
For example, if we are interested in the behavior of the shock absorbers in this landing gear assembly,
can we simplify or even remove other parts, like the tires?
If not required, suppressing unnecessary components and sub-assemblies from our analysis will save us time in setting up and solving the analysis.
When we suppress or ignore parts that interact with our main geometry, we represent their effect with boundary conditions.
Going back to the example of the landing gear, we may constrain the bottom of the tires in the vertical direction if the plane is resting on the runway.
We could simplify this further since the load distribution from the tires to the axel is straightforward, so we may be able to suppress the tires and just constrain the axel.
A force applied to the top of the landing gear can represent the weight of the plane,
although we need to have appropriate support to prevent lateral movement, as the landing gear is not free to move side-to-side.
We make these decisions based on the load path and the relative stiffness of the parts.
For example, the runway is very rigid compared to the landing gear,
so representing the effect of the ground with support may be a suitable approximation in a static analysis.
However, if there are flexible parts that affect the distribution of loads, we may need to consider including such parts –
what is nice, however, is that we can mesh such parts with a coarse mesh and still obtain an efficient solution.
Let us now focus our attention on geometric details of specific parts and how they are related to our objectives.
For example, when we are doing a stress analysis of a component in the assembly,
we may wish to exclude small details like imprinted, decorative letters or the details of teeth, etc.
We can also get rid of the small and sliver faces by merging them into bigger patches.
Minimizing the geometric details on the model can help us to reduce mesh size significantly and make the analysis run more quickly.
Let us use a simple example of a brake lever of a bike and address the questions we just discussed in the process of performing stress analysis.
Here, we are looking at a bike brake lever geometry in Ansys SpaceClaim.
This is the lever part, where the hand can push it down to slow down or stop a bike.
This is the casing part, which is mounted on the handlebar through this hole.
The lever and casing parts are linked by this bolt.
When the hand pushes down the lever, it rotates around the bolt.
And at the same time, the brake cable is pulled which engages the brakes on the tires.
We can see that the cable is connected to the lever from this hole and passes through the casing part to this cap nut.
In this simulation, we are interested in reviewing the stresses and deformation of the aluminum lever part when the brake is engaged.
Now, let us consider what geometry to model and decide on the level of details to include in this simulation.
First, regarding the casing part.
We know it is fixed on the handlebar and the lever part can rotate around it through the bolt.
The casing is assumed to be much stiffer than the lever, so we will be excluding this part in our simulation.
In SpaceClaim, we can go to the Structure Tree, right-mouse-click the part, and select “Suppress for Physics”.
We can also hide the part from display by unchecking this box.
“Suppress for Physics” and “Hiding” the part can also be done by directly selecting the part and right-mouse-clicking with these two options.
Accordingly, the cap nut and the check nut attached to the casing part can be omitted, too.
We can just suppress and hide them.
Now let us move to the bolt connection between the lever and the casing part.
Look at the bolt and the nut – we can see that both have threads.
These threads can dramatically increase the number of nodes and elements in the model, which will increase the simulation time.
If we were interested in the threaded portion of the bolt, we may wish to retain such detail,
but, in this simulation, recall that the lever is the part of interest.
Thus, keeping details such as the thread of a bolt is not helping with our objective.
So, we can remove the threads to simplify the geometry for meshing purposes.
We can then have frictional contact between the lever and the bolt.
Or, in this case, we can further simplify the geometry by replacing the bolt and the nut with a boundary condition that allows rotation.
This means we can suppress the bolt and the nut in SpaceClaim, and the boundary condition will be applied later in Ansys Mechanical.
Another boundary condition we need to include is the stiffness of the cable.
In this model, we can use a spring with assigned stiffness to represent the cable.
The spring connects this hole and the bottom area of the cap nut.
We need to create a coordinate system on the cap nut bottom area so that we can use it in Ansys Mechanical for defining the location of the spring.
Thus, we will select the inner circular edge here and then click on Origin.
This coordinate system will be passed to Mechanical.
Now let us consider how we should apply the load from the hand to the lever.
What we need to consider is the size of the area we apply this load,
because depending on different hand sizes, the area of the applied load can be different.
In SpaceClaim, we can project the correct hand size to the lever.
We can create hand faces with a given dimension, then click on the Project tool in Design Tab from the Menu.
Here, select the finger faces to project on the lever.
Now, we are done in SpaceClaim.
You can see that while we started with a complicated assembly,
we ended up with a single component through careful consideration of the behavior of the brake system.
Let us open Ansys Mechanical to complete the setup of the model and run the solution.
First, let us include Aluminum material from Engineering Data.
Then double click Model to open Mechanical.
We select Aluminum as the material for the lever part.
Next, we need to add the spring for cable force.
We can right-mouse-click on the Connections, then click on “Insert”, “Spring”.
We will set the spring to be Body to Ground, meaning one end of the spring is attached to this hole area,
and the other end is attached to the ground, which is the reference coordinate system point.
So, for the Reference part, we can select the created coordinate system from SpaceClaim.
And for the Mobile part, we just scope this to the hole area.
In this simulation, we assume the stiffness of the spring is given as 20 N/mm.
For mesh, we can add a sizing control.
Select the entire body and set the element size to be 1 mm.
Remember that we removed the bolt and the nut between the lever and the casing,
so we need to add an appropriate boundary condition here.
In Mechanical, we have an option to add Cylindrical Support.
Here, we can select the inner area of the hole and set the radial and the axial direction to be fixed,
and the tangential direction to be free, meaning it can only rotate along the axis.
Note that we are performing a linear, or small deflection, analysis in this demonstration,
so there will not be actual rotation about this Cylindrical Support.
Next, let us add the load to the lever.
Assume that the force from the hand is 15 N.
For results, let us insert an Equivalent Stress contour plot.
Now, we can hit the Solve button.
The model runs fast and here are our stress results with deformation.
This concludes the demo, now let us summarize what we learned in this video.
Deciding which geometry to include in the numerical simulation and the level of geometric detail is an important first step,
as that provides a balance of computational efficiency and accuracy.
This decision is determined by the physics and objectives of the analysis.
For stress analysis, we want to consider the relative stiffness of the parts and the load path
to help us determine if a part can be suppressed and replaced with a boundary condition or force –
or if we need to keep the part if its flexibility will affect the outcome of our analysis.
A second step is to determine the level of geometric detail included in our parts –
there may be small features, like tiny holes or threads or decorative features that are away from our regions of interest
and do not affect the outcome of the simulation but may increase the computational time
due to the finer mesh needed to resolve such small geometric details.
As a rule of thumb, the further away you are from your regions of interest, the less geometric detail you may need, a coarser mesh may be used,
and the results tend to be less sensitive to applied loads and boundary conditions.
Thus, if applying boundary conditions or loads directly on your part of interest is not appropriate,
consider adding the additional parts interacting with your critical part to provide the proper flexibility or load distribution.
I hope that you find this video informative.
Thank you for watching and do visit our channel to discover more useful learning resources.