Fill out the form to download

Required field
Required field
Not a valid email address
Required field

Documentation

Bending of an Aluminum Pipe

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

pipe bending simscale tutorial

Geometry

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

Geometry Preparation

All solid geometry should be free of any interferences, 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 defeature and remove this geometry in CAD. This will dramatically reduce mesh cell count and therefore solve time. 

Example Case

This is a jig used to bend aluminum tubing. It consists of a small and large roller, a stopper, and the aluminum pipe.

labeling the stopper, small roller, large roller, and aluminum pipe
Labeling the components in the simulation.

Reference project link:

Analysis Type

Once the geometry is in the platform, create a new simulation by selecting the “+” icon next to “Simulation”. Select Static for the type of analysis. Make sure to toggle on “Nonlinear analysis”.

creating a static simulation
Selecting the ‘Static” analysis type.
changing the static simulation to nonlinear
Toggling Nonlinear analysis.

Meshing

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

automatic mesh options in simscale
Creating a standard mesh.

We are going to add 3 refinements to the mesh. The first will be a local element sizing on the pipe. To select all the faces, toggle 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.

creating a local element size
Creating a local element size on the faces of the pipe.

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

hiding components within the simscale geometry tree
Hiding every component except for the 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.

adding refinement to the edge of the large roller
Creating a local element size on the contact face of the large roller.

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

adding refinement to the edge of the small roller
Creating a local element size on the contact face of the small roller.

You can now generate the mesh.

Simulation

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 going to add a bonded contact between the stopper and the pipe. To add a bonded contact, click the plus next to Contacts in the simulation tree – this is not the same as a physical contact. 

creating a bonded contact in simscale
Creating a bonded contact between the stopper and the pipe.

After creating the bonded contact, we need to make a physical between the two rollers, and the pipe.

creating a physical contact second example
Creating a physical contact between the two rollers and the pipe.
creating a physical contact in simscale
Creating a physical contact between the two rollers and the pipe.

Materials

The SimScale platform comes with many default materials. Select steel for the small and large roller, as well as the stopper.

asisgning steel as a material within simscale
Assigning steel as the material for the stopper and rollers.

Select Aluminum for the pipe. 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.

assigning aluminum as a material
Assigning aluminum as the material component for the pipe.

Initial Conditions:

For this simulation, the initial conditions can be left untouched.

Boundary Conditions

Apply a fixed value boundary condition to the small and large roller:

creating a fixed boundary condition within simscale
Applying a fixed boundary to the large roller and stopper.

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

creating a symmetry plane boundary condition
Applying a symmetry plane to faces on the tube.

Apply a rotating motion boundary condition to the small roller. It is rotated about the x-axis with a non-linear value of (pi/180)*130*t rad. 

creating a rotating motion boundary condition within simscale
Applying a rolling motion to the small roller.
rotating motion table
Table defining the value of the rotating motion.

Result Control

Create additional solution fields for contact pressure and signed vonMises stress.

creating a solution field within simscale
Creating a solution field for Signed von Mises stress.
creating a solution field within simscale
Creating a solution field for contact pressure.

We have also added two volume calculations. The volume calculations will allow us to graphically see the stress in the pipe over time.

creating a volume calculation within simscale
Creating a volume calculation for von Mises stress.
creating a volume calculation within simscale
Creating a volume calculation for Signed von Mises stress.

Numerics  

The numerics can be left alone.

Simulation Control

A few changes need to be made to the simulation control that can be seen here:

simulation control within simscale
Changing the ‘Simulation interval’ and ‘Maximum time step length’ in ‘Simulation control’

Changing the simulation interval to 1 second with a time step length of .05 seconds will give us 20 data points through the simulation. Everything else in the simulation control menu can be left alone.

You are now ready to run the simulation.

Results

Review & Interpretation of Results:
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.

fully displaced aluminum tube
Max displacement of the aluminum showing the von Mises stress.

An animation of the entire simulation can also be shown:

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

For additional post-processing, check out this documentation page.

Congratulations! You finished the tutorial!

Note

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

Contents
Data Privacy