Fill out the form to download

Required field
Required field
Not a valid email address
Required field


Tutorial: Bending of an Aluminum Pipe

This is a tutorial on how to set up a simulation of the bending process of an aluminum pipe.

aluminium pipe displacement post processing
Figure 1: Displacement results on the aluminium pipe.


This tutorial teaches how to:

  • set up and run a static simulation
  • assign topological entity sets in SimScale
  • assign boundary conditions, material and other properties to the simulation
  • mesh with the SimScale standard meshing algorithm

We are following the typical SimScale workflow:

  1. Preparing the CAD model for the simulation
  2. Setting up the simulation
  3. Creating the mesh
  4. Run the simulation and analyze the results

1. Prepare the CAD Model and Select the Analysis Type

First of all click the button below. It will copy the tutorial project containing the geometry of the aluminum pipe into your own workbench.

The following picture demonstrates what should be visible after importing the tutorial project.

imported cad workbench aluminium pipe stopper roller
Figure 2: The imported CAD model of the aluminium pipe, rollers and stopper.

If you are using your own CAD model make sure to follow these instructions:

All solid geometry should be free of any interference, intersecting surfaces, and small edges. Issues such as these should be fixed in CAD before bringing the geometry into the SimScale platform. More specific preparation details are mentioned here.

Before starting to set up the model, check the following:

  • Please make sure that the imported geometry consists of solid parts and not sheet/surface elements.
  • If the geometry has small fillets or round faces which are insignificant for the analysis, then it is recommended to remove this geometry in CAD. This will dramatically reduce mesh cell count and therefore solve time.

1.1. Create the Simulation

create simulation
Figure 3: Creating a new simulation.

Hitting the ‘Create Simulation’ button leads to the following options.
Choose ‘Static’ as analysis type and click on the new ‘Create Simulation‘ option to get started:

create simulation list static analysis
Figure 4: Static analysis type selection from the simulation library.

2. Assigning the Simulation Properties

Initially, make sure the ‘Non Linear analysis‘ is toggled on:

non linear static analysis
Figure 5: Enabling the non linear analysis.

2.1. Creating Contacts

SimScale will automatically detect any touching faces within the geometry, but sometimes assignments are needed for faces that SimScale won’t automatically detect. We are adding a bonded contact between the stopper and the pipe.

  • Click on the ‘+‘ icon next to the Contacts in the simulation tree – this is not the same as a physical contact.
bonded manual contact static analysis
Figure 6: Creating a bonded manual contact.
  • Select the ‘Bonded‘ under the Manual Contact creation.
  • Change the Position tolerance to ‘Off‘.
  • Assign the following faces:

Proceed to the Physical Contacts assignment.

  • Click on the ‘+’ icon next to the Physical Contacts.
physical contact static analysis nonlinear
Figure 7: Creating a physical contact.
  • Apply ‘1e-12‘ to the Penalty Coefficient.

2.2. Model & Element technology

Leave those two panels as default, and proceed to the Materials.

2.3. Define the Materials

Two different materials are used for this simulation.

steel material library
Figure 8: Choosing Steel from the material library.

The Steel is assigned to the Stopper, the Small roller, and the Large roller:

steel assignment
Figure 9: Properties and assignment for Steel.

Finally we need to create Aluminium:

aluminium material library
Figure 10: Choosing Aluminium from the material library.

The pipe is modeled as aluminium. The material behavior needs to be changed to plastic, and this csv needs to be imported as the stress-strain data. 

Changing the material behavior to plastic allows permanent deformation, where the elastic behavior will cause the body to rebound to its original shape:

aluminum assignment properties material pipe
Figure 11: Properties and assignment for Aluminium.

2.4. Initial and Boundary conditions.

For this simulation, the initial conditions can be left untouched. Apply a fixed value boundary condition to the small and large roller:

fixed value boundary condition static simulation zero displacement
Figure 12: Applying a fixed value on the large roller and stopper.

A symmetry plane will be applied to the flat faces of the pipe.

symmetry boundary condition pipe static simulation
Figure 13: Applying a symmetry boundary condition on the two pipe faces.

Apply a rotating motion boundary condition to the small roller.

rotating motion boundary condition roller static simulation
Figure 14: Applying a rotating motion on the small roller.
  • It is rotating around the x-axis, so set the Rotation axis as below.
  • Then click on the icon next to the Rotation angle:
rotation formula table
Figure 15: Applying the formula for the rotation.
  • For a non-linear value of (pi/180)130t rad, set the following formula.
  • Then confirm your definition by clicking ‘Apply‘.

2.5. Numerics and Simulation Control.

The numerics can be left in their default state.
Fill in the simulation control settings as below:

simulation control panel
Figure 16: Simulation Control settings.

2.6. Result Control

Solution Fields

Create additional solution fields for contact pressure and signed von Mises stress

stress result control solution field
Figure 17: Creating a solution field for the stress results visualization.

Change the Stress type to ‘Signed von Misses stress’.

signed von mises solution field stress result control
Figure 18: Setting the stress to signed von Mises.

Then add a ‘Contact’ the same way, and leave the panel in its’ default state:

contact pressure results control solution field
Figure 19: Creating a contact pressure solution field.

Volume Calculation

Two volume calculations will now be added. The volume calculations will allow to graphically see the stress in the pipe over time.

min max volume calculation pipe stress results control
Figure 20: Adding a new volume calculation for stress visualization on the pipe.
von Mises stress volume calculation min max pipe
Figure 21: Volume calculation settings for von Mises stress.
  • Change the Field Selection to ‘Stress’.
  • Select the ‘Von Mises’ Stress type.
  • The Component selection will be automatically changed to ‘Von Misses stress’.
  • Assign this calculation to the Pipe. Select it from the Geometry tree like before.

Repeat for a ‘Signed von Mises’ Stress type and Component selection.

signed von Mises stress volume calculation min max pipe
Figure 22: Volume calculation settings for signed von Mises stress.

3. Mesh

The standard mesh will be used, and each setting can be left alone.

standard mesh algorithm mesh settings pipe
Figure 23: Mesh settings for the standard mesh algorithm.

Three mesh refinements are going to be added.

The first will be a local element sizing on the pipe. To select all the faces, toggle on the face select and the box select options at the top. Hiding the other parts can make it easier to ensure only the desired parts are selected.

activate box selection faces local element refinement mesh pipe
Figure 24: Selecting faces of the aluminum pipe and applying a local element refinement.

The slashed out eye symbol indicates the part is hidden. In this scenario, only the pipe is shown.

hide parts assignment local element refinement
Figure 25: Hiding the unnecessary faces of the aluminum pipe.

The second mesh refinement is another local element size that is applied on the face of the large roller that contacts the aluminum pipe.

large roller local element refinement face selection maximum edge length
Figure 26: Selecting faces of the large roller and applying a local element refinement.

The final mesh refinement is a local element size applied on the face of the smaller roller that is in contact with the tube:

small roller local element refinement face selection maximum edge length
Figure 27: Selecting faces of the small roller and applying a local element refinement.

The resulting mesh will have about 53.2k nodes and look like this:

final mesh of model
Figure 28: Visualization of the mesh.

4. Start the Simulation

Create a new run by clicking on the ‘+‘ icon next to the Simulation Runs on the simulation tree like below:

new run simulation tree
Figure 29: Creating a new simulation run.

Now you can start the simulation and after about 91 minutes you can have a look at the results.

5. Post-Processing

Click on the ‘Solution Fields’ under the finished run in order to be redirected to the Post Processor.
Within the results tab, the scalar von Mises stress can be toggled globally.

Also, the displacement should be applied. After 1 second, the displacement of the tube is shown, with the color map of the stress.

gif showing the tube displacement
Figure 30: Displacement of the pipe over 1 second.

Analyze your results with the SimScale post processor. Have a look at our post-processing guide to learn how to use the post-processor.
Congratulations! You finished the tutorial!


If you have questions or suggestions, please reach out either via the forum or contact us directly.

Data Privacy