Have you ever wondered how products are engineered to be successful and reliable?
In many cases, the first design that engineers develop is not the most optimal.
Through trial-and-error or incremental improvements,
the engineered product can become reliable or more cost-effective or both.
Numerical simulation provides the ability to compare multiple designs virtually,
without needing to build and test physical prototypes.
Therefore, simulation proves to be a powerful tool providing insights about the design
and helps the engineer in developing reliable designs in a faster and cost-effective manner.
All of this is achieved using Workbench design points,
which allow the engineer to examine how changes to the geometry, material properties,
or loading conditions affect the system's response.
In fact, once a parametric model is set up,
automated design optimization and reliability studies are just a few clicks away!
In this video, we’ll focus on the use of Workbench design points using parametric models.
The video consist of a short lecture followed by a walk-through example using Ansys Mechanical.
Ready, let’s get started.
Imagine if you need to build and test a physical prototype for each set of design parameters you wished to explore
wouldn’t that be expensive and time-consuming?
Workbench allows us to create multiple design points and perform “what-if” studies to see how outputs depend on input parameters.
For example, you can easily evaluate different geometric configurations to see which set of dimensions minimize the peak stresses.
Looking at the effect of various operating conditions on the product performance
or getting insight into material selection can be addressed with what-if studies.
Let’s start by noting that a “design point” is a collection of input and output parameters.
Input parameters include geometric dimensions, such lengths and radii, in your design.
They can also include analysis inputs,
such as the magnitude of pressures and forces or material properties such as elastic moduli.
Output parameters are generally information about your geometry or results from an analysis.
These include but are not limited to system mass, peak stress on a part,
or maximum deformation of your assembly.
Note that we can also have derived parameters,
meaning that a parameter is dependent on the value of another parameter.
It is easy to define parameters in Ansys SpaceClaim and Ansys Mechanical.
Click on the P symbol that appears next to the dimension or use Groups in SpaceClaim to create the parameters.
In Mechanical, click on the square field in the details view to create parameters.
CAD parameters can come from 3rd-party CAD packages such as Creo and SolidWorks using the direct CAD associativity feature,
which is a topic outside of this lesson.
In this video, we will be using SpaceClaim to define CAD parameters.
Once the input and output parameters are defined,
a “Parameters Set” is attached to the analysis system on the project page.
By double clicking on the “Parameter Set,” we can open the Parameter Workspace.
What-if studies can be created in the Parameter Workspace by defining design points in the Table of Design Points.
Recall that each design point is a set of parameter values representing a single configuration.
Therefore, we can evaluate multiple scenarios using several design points.
Creating different physical prototypes costs both time and money.
On the other hand,
virtual prototyping through design points not only is easier and more cost-effective to perform,
but we can investigate effects such as changes in operating or loading conditions that may be hard to reproduce or to control in real life.
Let’s look closer at the table of design points.
The current project is designated as design point 0, or DP0 in the Table of Design Points.
Additional design points can be created by duplicating existing design points or by entering new input parameter values.
By default, Workbench does not retain all analysis files for each design points after they are solved.
Except for the current design point, only the output parameter values are saved.
In some cases, we might want to review the results interactively for specific design points.
In that case, we would need to retain data, which is easy to do in the table of design points.
Just check the Retain Data column in the table of design points.
Once multiple design points have retained data,
we can switch back and forth between these multiple designs within the project.
To view the design associated with a given design point, we set it as the current design point.
Only design points with retained data can be set to current,
and only one design point can be set to current at a time.
Design points can be updated in the Parameter Set where we can update the table of design points at once
or select individual design points to update or from the Project page to update the whole project.
Once the design points are updated and solved,
the outputs will be populated in the DP table
and can be investigated to find out which design is optimal based on the input parameters' variations.
The results of the DP study can be plotted using
Parameter Chart which illustrates the relationship between a selected parameter and each of the design points, and
Parameters Parallel Chart which illustrates the relationship between all parameters and each of the design points.
What-if analysis using the table of design points is the first step in our effort to understand our design.
It is worth noting that automated optimization tools,
such as Design Exploration or optiSLang, are also available but are outside of the scope of this lesson.
Now, let's see how to set up, solve and postprocess parametric model in our walkthrough example in Ansys Mechanical.
In this demo,
let’s look at a parametric study of an Aluminum bracket.
This bracket is subjected to loads and boundary conditions which result in stresses and deformation in the bracket.
The objective of this parametric study is to check if the change in the design of bracket
helps to decrease the peak stresses without changing the mass of the bracket.
The bracket design is varied using 2 geometric properties.
The parameter “outer_add” will add material on the outer portion of the bracket,
whereas the parameter “inner_cut” will remove material from the inner portion of the bracket.
Both parameters can be accessed from the Workbench project page under Parameter Set.
Since we need to maintain the mass of the bracket in each design change,
one of these parameters should be dependent on the other parameter.
P2 can be defined as the ratio of the area of two faces multiplied by P1.
Select P2 parameter in Parameter set.
In the properties panel,
specify Expression as 0.913* P1.
Let’s quickly review the setup of this model.
The material for this bracket is specified as Aluminum Alloy.
An element size of 1 mm is specified to generate a relatively fine mesh in the model.
A load of 200 N is acting in the negative Z direction on the hole located at one end.
The 2 holes on the other end are fixed using Cylindrical supports to prevent them from deforming in the radial direction,
while allowing them to deform along axial and tangential directions.
A frictionless support is also defined on the side face to restrict it from moving along its normal direction.
In addition to monitoring the Equivalent Stress for the entire body,
the Equivalent Stress is separately monitored in the cutout portion as well
as on the top side of the bracket where higher stresses are observed.
Also, the deformation along the direction of loading is also being monitored.
Now let’s parameterize the mass of the bracket to ensure that it remains constant for each design change.
In the Model tree, click Geometry.
In Details panel, expand Properties and click the box located next to Mass.
You will now see a “P” symbol indicating that this output result is converted into a parameter.
If you go to the Parameter set on Workbench project page,
this parameter will appear as an output parameter.
Next, in the details of Equivalent Stress defined for the entire body,
create a parameter for Maximum stress value.
Go to the Parameter set on Workbench project page and rename it as “Stress Total”.
Similarly,
create parameters for Maximum stress value from the other 2 Equivalent Stress results.
Rename the 2 output parameters as “Stress Cut” and “Stress Top”.
Lastly, go to the Directional Deformation result and create a parameter for the Minimum Deformation value.
Rename this output parameter as “Uz”.
Now let’s perform a parametric study by increasing the thickness of the outer portion of the bracket
and understand the resulting stresses.
Let’s increase the thickness by a total of 5 mm by incrementing the value of P1 in each design point by 1 mm.
Before updating the design points,
let’s retain the data for each design point to view the design associated with a given design point.
We are now ready to update all the design points.
All the design points get solved in few minutes and we can analyze the results of the output parameters.
First, if we look at the parameter P3 which reports the mass for each design point,
we can see that the mass is remaining constant for each design change as expected.
If we look at the total stress values,
we can notice that the maximum stress is increasing as the outer thickness increases while the inner thickness reduces.
The stress values reported in the cutout region and top region provides some interesting information.
We see that the peak stresses are occurring in the cutout region and increase with decrease in the thickness of the cutout region.
The peak stress on the top of the bracket is less as compared to that in the cutout section.
Also, there is not much variation in the stress values for each design change.
Another way to interpret these results is by plotting charts.
Let’s add a parameter chart.
Set the bottom X axis as outer_add parameter and the Y-axis left as Uz.
The chart tells us that even though the analysis is linear and the change in dimension for the
six design points is incremented by the same amount, the change in deformation is not linear.
We see that the first 1mm has less effect on Uz but increases in each design point.
Now, let’s plot “Stress Cut” and “Stress Top” in a single chart.
We can see that the maximum equivalent stress on top face decreases and then increases.
Looking at stress output, we see this is due to the stress distribution change from the change in geometry.
The chart of “Stress Total” verses outer_add parameter also tells us that
even the peak stress is not behaving in linear fashion with change in geometry.
We set up the model once and just run it, and it runs 6 cases automatically,
giving us insight that the geometric changes aren't linearly related to the stress or displacements,
even though this is a linear analysis.
We see that the initial design is the best,
so if presented with this design change,
we can say with more confidence that the design change won't be favorable to the structural response.
This completes the demonstration on how to set up, solve and postprocess parametric model in Ansys Mechanical.
In Ansys Workbench, multiple design points and comparison studies for input and output parameters can be easily done.
This serves useful for What-if analysis to see how results vary as per the inputs,
understanding the performance of our design over a range of specified conditions.
Input parameters define the geometry and the boundary conditions while output parameters are the results of the analysis.
Features can be easily parameterized for the model in CAD software,
specifically in SpaceClaim and in Mechanical by just a click of checkbox.
A design point is a single set of parameter values representing one design.
By varying the input parameters and calculating the corresponding outputs,
multiple design points can be created and analyzed using the table of the design points.
The design points can be compared with the help of Parameter Chart and Parameter Parallel Chart.
Ansys does offer automated optimization and robust design methods,
though this is outside the scope of this lesson,
it is worth noting these tools extend the benefits and advantages of parametric models for obtaining optimal designs.
I hope you have found this video informative.
Thank you for watching and check out our other courses to discover more useful learning resources.