Setting Up a Basic Simulation in Ansys Mechanical
This blog is designed to help beginners understand the step-by-step workflow required to set up a structural analysis using Ansys Mechanical within Workbench. Whether you're analyzing a single part or working with a larger assembly, the process begins by defining materials, importing or creating geometry, generating a mesh, and applying the appropriate structural boundary conditions. Each of these steps is essential for building a valid simulation that accurately reflects real-world behavior. This guide walks through the basic setup and organization of a Workbench project to give new users a solid foundation for running structural simulations with confidence.
This example will use the following CAD file:
Getting to Know Workbench
Ansys Workbench serves as the graphical front end to set up, organize, and connect simulation modules. Each type of analysis (structural, thermal, fluid, etc.) is handled through a module that you can drag from the Toolbox into the Project Schematic.
When you drop a module (e.g., Static Structural) into the schematic, it creates a set of cells, each corresponding to a different stage of your simulation setup:
-
Engineering Data: Define materials and the material properties you'll need for your simulation
-
Geometry: Import, adjust (clean) or create your CAD model
-
Model: Open Ansys Mechanical to assign materials and define setup
-
Setup: Apply mesh controls, boundary conditions and loads
-
Solution: Solve the model
-
Results: View and post-process simulation output
Each of these cells plays a critical role in building your simulation systematically. We'll go through each of these steps individually in more detail.
Defining Materials in Engineering Data
To begin, double-click the Engineering Data cell to open the material editor. A new tab should open up in the Workbench interface.
Here, you'll find:
-
A material list on the left
-
A property editor at the bottom
-
A tabular data viewer for temperature- or time-dependent properties on the top right
By default, "Structural Steel" is included. To add more materials:
-
Click the "Engineering Data Sources" button in the top lefthand corner (see below)
-
Browse the available material libraries (e.g., Granta Sample Materials) for the materials you are interested in using for your simulation
-
Select a material and click the yellow “+” to add it to your project
- Toggle off "Engineering Data Sources" to return to the list of materials you have available to see all the materials you've added.
Alternatively, we can also choose to create new materials if the material we want is not available from the libraries. To create your own material:
-
Click the box on the materials list page which says "Click here to add a new material". Give this new material a name.
- Once the material has a name, we'll need to assign it's respective properties. The properties we need to add will depend on the type of analysis we would like to run. For example, a linear static structural model (that is to say, an analysis where we do not expect the stresses to exceed the Young's Modulus of the material we're using) does not require us to insert any type of plasticity data. By the same token, if we are only interested in the structural response of our model and will not be accounting for any kind of thermal gradient, we also do not need to insert any types of thermal properties (such as thermal conductivity etc). To help filter out some of these properties, we can click on the "Filter Engineering Data" button. This will remove properties for other types of physics that we do not need (such as those required for a thermal analysis), but will keep all others that could feasibly be applied. The minimum properties we need to add for a static structural model are the Elastic properties, usually given by the Young's Modulus and Poisson's Ratio for an isotropic material. We can add this by clicking on adding the "Isotropic Elasticity" model under "Linear Elastic", then entering the material information in the yellow boxes.
For this example, we’ll use the "Copper Pure, C10100, hard" material from the Ansys Granta Materials Data for Simulation (Sample) library.
Importing Geometry via Discovery
Now that we have our material properties assigned, we can move the the Geometry cell to define our CAD model. In this example, we'll be using a pre-built CAD model. To bring in your CAD:
-
Right-click the Geometry cell → choose New Discovery Geometry
-
In Discovery, go to
File → Import External Geometry File -
Load the Solid Assembly.SLDASM CAD file.
Once loaded, you can make geometry adjustments as needed. If not, we can proceed directly into Mechanical. In this example, we will not be adjusting our CAD model in any way. However, this blog goes through geometry preparation in more detail. Additionally, more helpful blogs for other tangent topics discussed in this example (contacts, meshing, etc) can be found on our blog page here.
Launching Mechanical and Assigning Materials
Back in Workbench, double-click the Model cell to launch Ansys Mechanical.
Once inside:
-
Expand the Geometry branch to view your parts
-
Select parts and assign materials via the Details pane
-
For example, select 3.1-1\Solid and 3.2-1\Solid in the tree and assign them the “Copper” material under the Assignment row. The other bodies can be left as “Structural Steel”
-
Reviewing Contacts and Connections
Under the Connections branch, you'll find automatic contact definitions generated by Mechanical. They are added using a slider value calculated by Mechanical based on the feature sizes of your CAD model. These settings, including the slider value, can be adjusted by clicking on the "Contacts" folder in the tree, then adjusting the settings in the Details pane. Once created, these define how individual parts interact (bonded, frictional, etc.). Without contacts, the software will not be able to understand how individual bodies interact with one another in an assembly, or what type of contact exists between them (ie bonded, frictional etc). To learn more detailed information about contacts, such as the different contact types, how they're enforced by the software and how to troubleshoot problematic connections, please see our blog "Contact Modeling in Ansys Mechanical For Beginners".
For simple models (including this example), leaving the default bonded contact is sufficient.
Meshing Your Geometry
Before any simulation can be solved in Ansys Mechanical, the geometry must first be converted into a mesh. A mesh is a network of smaller, discrete elements that the software uses to approximate the behavior of the model under various loads and conditions. This process is at the heart of finite element analysis (FEA). By breaking a complex geometry into simpler parts (elements), Ansys can numerically solve the governing equations of physics for each element and compile those results into a full-system response.
A good quality mesh is critical to achieving accurate and stable results. Poor meshing can lead to longer solve times, convergence issues, or even incorrect outcomes. Factors like element shape, size, and refinement in critical areas all influence the quality of your results.
While this blog provides a basic overview of mesh setup and the tools available in Ansys Mechanical, we won't dive deeply into meshing theory or advanced techniques here. For those interested in a more detailed discussion (including when to use tetrahedral vs. hexahedral elements, mesh quality metrics, refinement strategies etc) be sure to check out our dedicated blog - Understanding Mesh Methods in Mechanical: A Comprehensive Guide.
To define meshing controls, we can right click on the Mesh branch of the tree. For our example, we'll walk through the process of adding a few different controls to help give an overview of this process.
-
Left click on the Mesh branch of the tree and go down to the details window. Set the Global Element Size to 3 mm
-
In the details window, open the Sizing tab and turn off Adaptive Sizing
-
Right click on the Mesh branch and insert a "Method". An object will appear under the Mesh branch. Click on this object and change the Method row to the Multizone option. Next, scope this method to the bolt/cylinder bodies as shown below.
-
Right click on the Mesh branch and insert another "Method". Here, we will use the Patch Conforming (Tetrahedral) method for the remaining 2 bodies.
- Generate your mesh by right clicking on the Mesh branch in the tree and selecting "Generate Mesh", or by clicking the "Generate" button in the ribbon under the Mesh tab.
Applying Structural Boundary Conditions
Once your geometry is meshed, the next essential step in any simulation is defining boundary conditions. These are the constraints, loads, and environmental inputs that tell Ansys how your model is expected to behave. Boundary conditions are how we simulate real-world physical effects like forces, pressures, temperatures, supports, and displacements. Without them, the model has no reference for how it should respond, and the simulation cannot proceed.
Applying boundary conditions correctly is just as important as having a good mesh. A model that is under-constrained may exhibit unrealistic rigid body motion, while one that is over-constrained may falsely resist deformation. The accuracy and reliability of your results depend heavily on how well your boundary conditions represent the actual use-case of the component or system.
This blog introduces the fundamentals of boundary condition setup in Ansys Mechanical, using simple examples to illustrate the process.
-
Right-click on Static Structural → Insert → Fixed Support. A fixed support will constrain all 6 structural degrees of freedom (Translation and Rotation in X, Y and Z) on whichever surfaces you apply it to.
-
Apply to the bottom 2 surfaces of the bottom block
-
-
Right-click Insert → Displacement
-
Apply a -2.5 mm in the Y-direction on both cylinder inner faces. Leave the X- and Z-directions as Free
-
-
Add Gravity via Insert → Standard Earth Gravity
- Set the direction that the gravity will act it to the -Y direction
Solving and Post-Processing
After setting up your mesh and applying all relevant boundary conditions, the next step in the workflow is to solve the model and interpret the results. Solving refers to the process where Ansys calculates how the system will respond under the defined conditions by numerically solving the governing equations of the selected physics. Depending on the complexity of the model, the solver may take anywhere from a few seconds to several hours to complete.
Once the solve is finished, the focus shifts to post-processing. This is where you extract meaningful information from the results, such as stress, strain, temperature distribution, deformation, or frequency response. Post-processing helps you understand how your design performs and whether it meets the intended criteria. It also allows you to identify areas of concern, such as high-stress regions or unexpected deformation patterns.
Once your setup is complete:
-
Right-click the Solution cell → choose Solve
-
Monitor progress under Solution Information
After solving, we can add post-processing items such as:
-
Stress
-
Strain
-
Total or Directional deformation
You can adjust units and isolate individual parts to make contour results easier to interpret. You can also animate results to see how the model deforms as the solution is solved.
Wrapping Up the Structural Workflow
At this stage, you’ve walked through the complete workflow for setting up and solving a structural simulation in Ansys Mechanical. From importing your CAD geometry and defining materials, to creating a quality mesh and applying structural boundary conditions, each step plays a critical role in ensuring accurate and reliable results. Once solved, you’ve also seen how to post-process the results to evaluate performance indicators such as stress, strain, and deformation.
This foundation forms the core of any mechanical simulation, and mastering it will prepare you for more complex analyses down the line. Whether you're validating a single part or preparing to simulate an entire assembly, these structural modeling skills are essential for building confidence in your design and accelerating the product development process.
For reference, the finished Workbench project can be downloaded from here. Please note, this project was created using version 2025 R1 with Service Pack 3, so you will not be able to open it if you are using an older version.