Hello Everyone
If you look at a butterfly or starfish,
apart from their pretty colors,
a unique feature that stands out is their symmetry.
Similarly, engineered systems like buildings, airplanes,
or cars have a symmetrical shape.
Designers usually take advantage of symmetry when they create models.
Only half of a symmetric model needs to be modeled,
and modeling tools such as mirror or copy of the section can be used to generate the entire model.
Can analysts also take advantage of symmetry while analyzing symmetrical structures?
The answer to this question is Yes.
In this video we will discuss when it is beneficial to impose symmetry boundary conditions
to make the analysis more computationally efficient and accurate.
On the other hand,
we will point out the situations when symmetry boundary conditions should not be used.
This video will consist of a short lecture followed by a walk-through example using Ansys Mechanical.
Ready, let’s get started!
A commonly asked question is:
How can we utilize symmetry in our analyses?
Some analyses may require large amounts of memory and computational time to obtain a solution.
If the geometry, material orientation,
loading and expected response are all symmetric about the same planes,
we can take the advantage of planar symmetry
and only model a portion of the actual structure to reduce the analysis run time and memory requirements.
Also, a finer mesh can be used in a symmetry model resulting in a more accurate solution
than a coarsely meshed full model with similar number of nodes and elements.
In solid mechanics,
the general rule for a planar symmetry boundary condition is that
the component of displacement normal to the plane of symmetry should be set to zero.
This makes sense if we think of the symmetry plane like a mirror,
as the deformation shouldn’t move into the mirror or overlap onto itself.
For line and surface bodies,
another requirement is that rotations into the plane must also be constrained,
using the mirror analogy,
a structure shouldn’t rotate into the mirror.
Although, there are several types of symmetry boundary conditions available in Ansys Mechanical,
we will focus our attention in this video on the Symmetry Region feature, which is used for planar symmetry.
The Symmetry Region can be defined based on either the global or a local coordinate system,
where we specify the symmetry normal direction.
It’s worth noting that, for 3D solid bodies, instead of a Symmetry Region,
a Frictionless Support can be applied on faces lying on the symmetry plane
since a Frictionless Support also constrains translations normal to the face.
However, Frictionless Supports can’t be used as a replacement for Symmetry Regions for line or surface bodies
since in-plane rotations will not be constrained with a Frictionless Support.
Note that the magnitude of any applied forces lying on planes of symmetry must be properly adjusted.
For example, in a half-symmetry model,
only half of the magnitude of force should be applied if the surface crosses the plane of symmetry
since we only have half of the geometry modeled.
Note that no adjustment of magnitude is needed for Pressure, Gravity, or Temperature loads.
After solving, the results from the symmetry model can be visually expanded about the symmetry planes to show the “full” model,
which is useful when presenting your results to others not familiar with the finite element method.
So, why should we use the symmetry boundary condition?
A big reason is that analysis can be more accurate.
Since the size of the geometry is reduced,
a finer mesh density can be used compared to a ‘full’ model,
which will result in a more numerically accurate solution compared to a full model with the same number of nodes and elements.
The results of the quarter symmetry model can be visually expanded to represent the full model results.
In Mechanical,
visual expansion of the symmetry model results is a beta feature that needs to be turned on under Options, Appearance, Beta.
In the details view under Symmetry in the Tree Outline,
the number of repeated symmetry segments need to be defined along with the small overlap value in the symmetry normal direction.
If there are two planes of symmetry, then two graphical expansions would need to be defined for each symmetry plane.
Let’s get back to the last question about Symmetry Region or planar symmetry.
When shouldn’t we use the Symmetry Region?
If any of the four requirements such as geometry, material orientation,
loading and expected response are not symmetric, a Symmetry Region shouldn’t be used.
For example, in a dynamic analysis like modal analysis a symmetric structure can have non-symmetric modes,
and using symmetry makes us miss these modes.
Another example is linear buckling analysis where using a symmetry model will omit non-symmetric buckling modes.
However, for typical stress analyses utilizing a symmetry region is usually beneficial when all of these four requirements are met.
Let’s now see how to set up, solve, and postprocess symmetry model in our walkthrough example in Ansys Mechanical.
For this walkthrough session,
let’s consider a model of a flange joint.
A flange joint consists of 2 flanges connected with nuts and bolts.
If we take one sixth sector of the model and copy it around its central axis,
we can generate the complete model.
So, this flange joint model can be considered as a symmetric model.
Let’s look at the loading on this flange joint.
Let us assume that the fluid flowing through the inner region of the joint is exerting a uniform pressure on the flange.
Next, let us also assume that a uniform force is acting on the top face of the top flange.
Let’s also assume that all bodies of this flange joint are made up of Structural steel
which exhibits isotropic material properties.
The geometry, material orientation, loading,
and expected response all exhibit symmetry about the same planes.
Thus, we can take advantage of symmetry and model only one sixth sector of the full model.
This will not only help to reduce the analysis run time and memory requirements but also get more accurate results.
To model this one sixth sector of the joint as a symmetric model,
we could make use of the Cyclic Region symmetry type.
Recall that a Cyclic Region allows us to solve for repeating sectors and still get a non-symmetric response.
Cyclic Region is a repeating pattern,
so it allows for twisting.
However, Symmetry Region is a mirror about the 2 planes,so there is no twisting.
Hence, for this example,
as we are expecting symmetric behavior for each sector,
we will use Symmetry Region instead of Cyclic Region.
Now that we have finalized on the type of symmetry that we would be using for this analysis,
let’s create the one sixth sector of the flange joint.
Let’s start with the flange model having bolt connections simplified in the form of beam elements.
Open a new session of Ansys Workbench.
Drag and drop Static Structural system on the Project page.
Right click on the Geometry cell and import the flange model.
Now double click on the Geometry cell to open the imported geometry in SpaceClaim.
We first need to create the symmetry planes for splitting the geometry.
Select the X axis from the Global coordinate system and click the Plane tool.
This will create a plane along YZ plane.
The plane is passing through the bolt locations and we would not like to create the section which cuts the bolt locations.
So let’s rotate this plane.
As there are 6 bolt locations,
the angle between 2 bolts is 60 degrees.
We need to create a plane that is in the middle of the 2 bolt locations.
So, we need to rotate the plane by 30 degrees.
Using the Move tool,
we can rotate this plane.
Press S to exit the Move tool.
Now, we need to create another symmetry plane located at an angle of 60 degrees from the previous plane.
Select the Move tool again and select the plane.
Press Control key (Ctrl) and drag the plane along the curved red colored axis.
Then type in 60 degrees.
We now have the 2 symmetry planes for splitting the geometry.
Select the Split Body tool.
Then select both the flange bodies and select any one plane for splitting the selected bodies.
Now select the Cutter tool from the tool guides and select the second plane for splitting the geometry.
The 60 degree symmetry sector is now separated and ready for further use.
The remaining bodies are not of interest and can be suppressed.
The symmetry model can now be transferred to Ansys Mechanical for performing the simulation.
Close the SpaceClaim window and double-click on Model cell to open Mechanical.
As mentioned earlier,
all bodies are assumed to be made up of Structural Steel.
Let’s proceed to defining the contacts.
It can be seen that one contact has been automatically created between the 2 flanges.
Let’s change its properties.
First, let’s change the contact type from Bonded to Frictional Contact.
Set the Frictional Coefficient as 0.1.
Leave the other settings to their default values.
We need to create contacts for connecting the beam element,
which represents the bolt,with the flange.
Insert a Manual Contact Region.
For Contact geometry,
select one of the end vertices of the beam.
And for the Target geometry,
select the annular face on the flange located on the same side of the vertex selected earlier.
Let’s keep the contact type as Bonded.
Change the Formulation to MPC and Constraint Type to Distributed,
All Directions.
Select Radius option for Pinball Region and specify a radius of 6 mm
so that the annular face falls within the pinball region for contact detection.
Similarly, create a contact on the other end of the beam (use the Duplicate option).
Since we’ll be using Symmetry Region for defining symmetry,
we first need to create local coordinate systems with the same orientation on the symmetry faces.
Right click on the Coordinate Systems tree and insert a new coordinate system.
Select any side face of the flange located on the symmetry plane to create the local coordinate system.
To ensure that 2 of its axes are parallel to the selected face,
go to principal axis section and change the “Define By” option to Geometry Selection.
Select any straight edge on that face to match the axes with the face.
Similarly, create another coordinate system on the other symmetry plane of the model.
Now comes the main feature that needs to be defined for simulating this symmetric sector.
Right click on the Model tree and insert Symmetry.
Right click on Symmetry and insert Symmetry Region.
Select the 2 faces of the flanges located on one of the symmetry planes.
Next, select the coordinate system that was created on this symmetry plane.
The Symmetry Normal should match the axis of the local coordinate system in the direction normal to the symmetry plane,
which in this case is the Z axis.
So select the Symmetry Normal as Z Axis.
Similarly, create a Symmetry region for the other symmetry plane.
Let’s define loads and boundary conditions for this symmetric model.
Let’s first add a bolt pretension load on the beam.
Generally, pretension load is applied in 2 load steps.
In the Analysis Settings,
change the Number of Steps to 2.
Now add a Bolt Pretension load.
Select the edge of the line body as the scoping geometry.
In the Tabular Data panel,
specify Preload as 1000 N in first loadstep.
Then, lock the second loadstep.
Details on bolt pretension loading can be found in a separate course.
Next, add Pressure load
and select the inner cylindrical faces and apply a pressure of 1 MPa in the second loadstep.
Add a Force load on the top face of the top flange.
Select the “Define By” option as “Components”.
Then go to the tabular data and specify 500 N along the Y direction in the second loadstep.
Lastly, let’s constrain the bottom face of the bottom flange using Frictionless Support.
The model is now ready to be solved.
Before doing so, let’s add a couple of results,
mainly Total Deformation and Equivalent Stress.
The solution completes in a few seconds,
and you can check out the deformation and stress contours in the model.
While presenting the results of any symmetric model,
it can be helpful to expand the results to show the full geometry.
This can be quickly done using the Beta Functionality of Symmetry.
To enable beta features,
go to the Workbench project schematic.
In the Tools menu, select Options.
In Appearance section,
enable Beta Options.
Since this model is repeating in a circular pattern,
we need to create a cylindrical coordinate system for expanding the results of symmetry model.
Add a new coordinate system and change its type to Cylindrical.
The z axis of this coordinate system should align with the axis of the symmetric model.
First select any circular face to position the cylindrical coordinate system on the axis of the model.
Now, add rotation around X axis and specify rotation angle of 90 degrees.
Click on the Symmetry folder in the Model tree.
In the Graphical Expansion 1 section,
specify number of repetitions as 6.
Select the Type as Polar.
Specify the sector angle as 60 degrees.
Lastly, select the cylindrical coordinate system.
You can now visualize the results of the full model.
If you recall from the lecture,
we use symmetry to make the analysis more efficient and accurate.
Let’s look at the results of the symmetric model and full model for a finer mesh resolution (0.4mm element size).
It can be seen that for a particular mesh resolution,
the symmetric model solved about 10 times faster than the full model.
Thus, you can obtain a more numerically accuracy result on a symmetric model by using a finer mesh,
yet the solution can still be faster compared to a full model!
This completes the demonstration of how to use Symmetry Region in Mechanical.
Let’s summarize
It’s advantageous to use symmetry when the
geometry, material orientation, loading,
and expected response all exhibit symmetry
about the same planes.
Using Symmetry Regions can give more accurate
and more computationally efficient solutions.
However, the Symmetry Region
should not be used when
all four symmetry requirements are not satisfied
such as in modal or linear buckling analyses
where non-symmetric modes are needed to be calculated.
I hope you have found this video informative.
Thank you for watching
and check out our other courses
to discover more useful learning resources.