Hello everyone!
While performing any analysis, we always come across a question asking whether or not the simulation results obtained are accurate.
Many new users may assume that any calculated result must be correct.
But is this the right assumption?
This makes validating and verifying the model one of the most important steps for any simulation, and this is something new users may take for granted.
In this video, we will focus our attention on establishing good practices for a new analyst performing Stress Analysis.
We will also go through some of the most important aspects which must be reviewed while setting up your simulation model.
So, let's get started!
We all desire accurate simulation results, and, generally speaking, this takes two forms:
Numerical Accuracy and Correct Model Representation
In Numerical Accuracy, we answer the question of whether the mesh is fine enough to get a mesh-independent solution.
While in Correct Model Representation, we focus on the question of whether the model is accurately representing our understanding of the physical system.
Numerical Accuracy has been covered in detail in another video lesson and is not the subject of the present lesson.
So, let's focus on the Correct Model Representation.
In order to check whether or not the numerical model is capturing the physical system, we need to answer some of the very fundamental questions.
Is the simulation addressing our objective?
And are our initial assumptions valid?
Let's understand this with a simple example.
In the case of an automobile crash test, we can observe that the system is dynamic but, what if we consider it as a static system?
In such cases, there may be a big discrepancy.
Usually, these questions need to be addressed in the planning stage before setting up the simulation, but it is always a good practice to double-check, especially to see if certain assumptions we made earlier are correct.
Another fundamental question which we need to address is do we have a ballpark figure of the response we expect?
While performing an analysis, we should always have a rough idea of the deformation or stress we expect to be generated in the system.
If we haven't obtained this information from physical testing or field measurements, we should do some rough, back-of-the-envelope calculations whenever possible.
Doing so always proves to be very helpful; otherwise, we will have no idea whether or not our simulation results are completely off.
So, let's begin with our first check we perform after obtaining results, which is verifying the Deformation.
In Ansys Mechanical, users can view animations of deformed shapes while analyzing the deformation results.
It is a very good practice to verify these animations and ensure that the structure is deforming in the manner which we expect.
It is important to note here that, while analyzing the simulation results of a linear analysis, the animations generated are, by default, exaggerated so that the user can get a proper understanding of the deformed shape of the part.
But users can change the deformation scaling between actual scale and other scale factors to better view the deformation shape.
Also, the deformation magnitude should be compared with a rough estimate or idea we should have established, as noted earlier in this lesson.
By verifying the deformation results, we can also identify whether or not our applied loads and supports are correct, especially to identify common problems like over constraining the model.
Let's now focus on our next check which is the Reaction Forces.
It's very good practice to verify whether the reaction forces observed make sense or have we achieved the expected force balance i.e., whether the applied force is equal to the reaction force?
Verifying the reaction forces is a very useful check as it helps us to get an idea about the global equilibrium of our model.
Another important check is understanding the load path in our model, right from the location of load application to the reaction forces from the boundary conditions or supports.
This is an important exercise as it helps us to validate whether our simulation model is capturing the actual or expected load path in our system.
Let's now proceed to our last check associated with our Initial Assumptions.
While analyzing the stresses and deformation values obtained in the solution results, it is very important to verify whether these values are large enough to require a nonlinear analysis?
Linear, or a small deflection analysis, assumes that the final deformed shape is essentially the same as the original geometry, and that is why the default behavior is to exaggerate the deformed shape when reviewing the results, as the deformation may be imperceptible.
If we check the actual deformation by using true scaling or review the deformation magnitude and see that it is relatively high, then we may consider the need to perform a large-deflection analysis.
We must also verify whether the equivalent stress values are exceeding the yield stress value of the material used.
In such cases, we can change the design of our part, if possible, to avoid yielding or we can also account for it using a plasticity material model.
Finally, do check for error messages and warnings before and after we obtain the solution.
These messages can highlight important items that we need to address or consider.
Let's now see how to implement some of these points with the help of a walkthrough example in Ansys Mechanical.
For the walkthrough, we will use a simple drone model that is hovering, balancing its own weight with the thrust generated by its motors.
Our geometry consists of a quarter-symmetric model of the main chassis and an arm, that is subjected to a force load from the motor thrust.
A drone often has numerous parts such as batteries, PCBs, and camera modules, therefore, a point mass is used to account for their weight in our simplified representation since we are most interested in the deformations of the drone arm.
Weak springs are also employed to limit the rigid body motion of the model.
The results of stress and deformation will be monitored, and the deformation is compared with a simple hand calculation.
Without further ado, let's get started.
Go to the project page and pick file > Open
Select the Workbench project archive file drone_quarter_symmetry.wbpz
Save the project to the desired location.
We will keep the filename as specified.
Double click on the model cell to open Mechanical.
The model has been partially setup so let's do a quick review.
Expand the Geometry and selecting each part, we can see the material assignment is Aluminum Alloy.
Click on Point Mass.
We are using a .25 kg point mass to account for the portions of the drone mass that is not modelled with geometry.
In this quarter symmetric portion, we are simply accounting for one quarter of the mass.
Click on Geometry and expand the properties tab.
We can see that the total mass is 0.3107 kg.
Expand the symmetry region, and notice we have two symmetry regions specified.
Expand the connections branch and then expand contact.
We can see the contact which is generated.
Ansys automatically detects contact between parts and assigns bonded contact by default.
Click on the circular beam connection.
This represents the bolt that is connecting the arm to the chassis of the drone.
Normally a bolt will have some pretension from torqueing it.
For this workshop we will omit the pretention.
Let's now apply the loads and boundary conditions.
We are considering a situation of the drone hovering in air, balancing its weight with the thrust from the motor.
So, for the simulated hover case, the force 'F' will be equal to m*a, where 'm' is the mass and is equal to 0.3107 kg and 'a' is equal to the acceleration due to gravity, which is 9.8066 m/s^2.
This equals a force of 3.0469 N.
Please note that this does not include the mass of the beam connection in the calculation since the mass property under geometry does not include the mass from beam connections.
Click on Static Structural, select the two holes at the end of the arm where the motor will mount.
Right click, insert, force.
Specify the magnitude of 3.0469 N.
Click on direction and select one of the two holes and click apply.
Change the direction by toggling between red and black arrows to point the force vector in the global - Y direction.
Please note the force is distributed over the faces of the two holes and it is not 3.0469 N per hole.
To insert the standard earth gravity, go to Static Structural, insert, standard earth gravity.
Change the direction to the positive Y global axis.
As you might have already observed, there is no boundary condition restricting the model from a rigid body motion in the Y direction.
For this, Weak Springs are used.
Weak springs are small spring elements with extremely low stiffness that are adequate to limit the rigid body motion but, should have no net effect on the analysis.
We will verify this assumption when we look at the results.
To use these, go to analysis settings and turn on the Weak Springs.
Now the model is ready to be solved.
Right-click on Static Structural and solve.
As now the model is solved, right-click on Solution, insert, deformation, and total deformation.
Right-click and evaluate all results.
Let's see the results in the normal plane to the arm.
To do that, select the face of the arm, go to display tab and click on 'look at' icon.
Go to result tab, edges, show undeformed wireframe for a better comparison between the deformed and undeformed model.
We can observe that the maximum deformation value is 3.79 mm and has occurred in the main chassis.
To get a clear picture of the deformation, we must check the directional deformation results.
To do that, right click on solution, insert, deformation, directional deformation.
Change the orientation to Y axis.
This will include the sign, unlike the total deformation, hence a proper comparison can be made with our hand calculation.
Right-click and evaluate all the results.
Change the deformation scale from true to auto to clearly see how the model is deforming.
With the help of this animation, we can conclude that the behavior of the model is correct and is adhering to the rules of fundamental physics.
Let's check the relative displacement between the tip and base of the arm.
Go to result, probe, and select near the screw holes at tip of the arm and at the base of the arm.
We can see the relative displacement between them is around 3 mm.
If we assume the arm is a cantilever beam fixed at the base, we can perform a hand calculation to give a displacement of about 1.3 mm.
This helps us see that a deformation of around 3mm from our simulation is reasonable, given that the base of the arm really is not fixed, but, rather can rotate because of the elasticity of the rest of the drone chassis.
We can also see that the drone has moved only in the positive Y direction, meaning that the forces are not perfectly balanced.
This can be explained.
Go to solution information, click on the text output, type ctrl-F to find, and type mass summary into the dialog box.
The mass reported in the solver output is the actual mass the solver recognizes, based on the mesh and additional entities, such as Beam Connections.
The solver does not utilize the solid model geometry but only the mesh in its calculations, so it's good practice to check the mass in the solver output.
Usually, small discrepancies can be explained if, for example, the mesh is coarse and does not capture curvature properly or if additional entities, like Beam Connections, have been added to the model.
Let's go back to the Geometry tab.
Here we can see the weak springs defined in the model.
To see the reaction forces developed in them, right click on solution, insert, probe, force reaction.
Change the boundary condition to Weak springs.
Right-click and evaluate all results.
Here we can observe small reaction forces in the weak springs, which is due to the small imbalance between the force of the motor we applied and the computed gravity force on the structure.
Recall that the force calculation for the motor did not account for the mass of the bolt, but, the computed acceleration body force from the solver did, hence, there is a slight force imbalance which is taken up by the weak springs.
The weak spring reaction forces are still small compared to our applied forces and hence the results are acceptable.
Now right click on solution, insert, stress, Equivalent (von-Mises) stress.
Right-click and evaluate all results.
Let's check the areas where we obtain maximum stress.
To do that, turn on the Maximum probe in Display tab.
We can see that the maximum stress is obtained at the bolt area in the chassis.
We can continue to scope stress results to different regions or faces of the assembly to get a better understanding of the stress distribution, as well as check that the stresses are reasonable and below the yield of the material.
Now let's investigate the vector plots to see what they can reveal.
Right-click on Solution, insert, stress, vector principal.
Scope it to the arm by clicking on geometry, select arm and click on apply.
Right-click and evaluate all results.
In the Results tab, pick on Vectors, then solid form, adjust vector display slider to increase scale a bit for better visualization.
The arrows show the magnitude and direction of the maximum, middle, and minimum principal stresses.
Notice how the top of the arm has compressive stress (blue) and the bottom has tensile stress (red) that aligns with the planar surface of the arm top and bottom respectively.
This is expected and is a good check as we expect similar behavior from a classic tip loaded cantilever beam.
We can also see that the stresses are tensile from arm to chassis in the contact area.
Let's turn on the wireframe to see how it looks inside.
We can observe that even though the stresses are small, they are tensile pointing out of the arm into the chassis.
This shows that the load path is not only through the screw hole, but also through the bonded connection.
If the arm was not actually glued to the chassis of the drone, we may wish to change this contact behavior to frictional rather than bonded.
In this case, we would expect to see the tensile stresses aligned with the drone arm and not pointing out of the arm into the chassis.
I hope that this example provided you with various elements that you can check in your analysis to make sure you are on the right path and with that said, the workshop demo is completed.
Let's summarize.
Validating and verifying the model setup is a critical step in performing an accurate analysis.
There are several basic questions that one should ask such as:
Are the initial assumptions valid?
Do the results violate/invalidate any of our initial assumptions?
Are the results adhering to physics fundamentals?
Do we have a ballpark figure of the response we expect?
If yes, are the results reasonably accurate?
Are the stress and deformation results comparable to hand calculations or our expectations?
Do the reaction forces make sense?
Is the simulation achieving the expected force balance?
Does the load path make physical sense?
With the verification of these key factors, we can have higher confidence that our simulation model will provide accurate results.
I hope you have found this video informative.
Thank you for watching and do check out our other courses to discover more useful learning resources.