Advanced Tutorial: Bending of an Aluminium Pipe (Marc)

This article is inspired by the original Bending of an Aluminium Pipe tutorial—which uses SimScale’s Standard FEA Static analysis type—and provides a step-by-step guide for performing a nonlinear structural simulation of an aluminium pipe bending process using the ‘Nonlinear Mechanical (Marc)’ analysis type. The objective is to analyze the deformation and stress distribution that develop in the pipe during bending, including nonlinear effects such as material plasticity, physical contact, and large deformations.

pipe bending tutorial marc with results overlapping for different time steps — Figure 1: Deformed shape and von Mises stress contour results for the aluminium pipe.

This tutorial explains how to:

Set up and run a ‘Nonlinear Mechanical (Marc)’ simulation.
Assign boundary conditions, materials, and other simulation properties.
Mesh the geometry using the SimScale standard meshing algorithm.
Analyze the results with the SimScale online post-processor.

The tutorial follows the standard SimScale workflow:

Prepare the CAD model for the simulation.
Set up the simulation.
Generate the mesh and run the simulation.
Inspect the results.

1. Prepare the CAD Model and Select the Analysis Type

Select the button below to copy the tutorial project, including the aluminium pipe geometry, into your workbench.

Import tutorial into workbench

The image below shows the interface after importing the tutorial project.

workbench view pipe bending — Figure 2: Imported CAD model of the aluminium pipe, rollers and stopper. This view appears after selecting the import link button.

If you are using your own CAD model, follow these instructions:

All solid geometry should be free of any interference, intersecting surfaces, and small edges. Fix these issues in CAD before importing the geometry into the SimScale platform. Refer to the CAD preparation guide for more details.

Before starting the simulation setup, verify the following:

Ensure the imported geometry consists of solid parts rather than sheet or surface elements.
Remove small fillets or round faces in CAD if they are insignificant for the analysis. This reduces the mesh cell count and computational solve time.

1.1. Create Simulation

To begin the simulation setup, select the ‘Create Simulation’ button located in the geometry dialog box. This action opens the simulation creation panel where analysis types are selected.

Pipe bending create simulation — Figure 3: Creating a new simulation with the geometry selected.

The simulation type selection panel appears, allowing the selection of the desired analysis type.

create simulation nonlinear mechanical marc — Figure 4: Analysis types available in SimScale. Select the **‘Nonlinear Mechanical (Marc)’** option for this tutorial.

Select ‘Nonlinear Mechanical (Marc)’ as the analysis type and click the ‘Create Simulation’ button to proceed.

Studies using the Nonlinear Mechanical (Marc) analysis type are nonlinear, accounting for nonlinear contact relationships and material properties. This analysis differs from a Dynamic analysis, which accounts for inertial forces.

2. Set Up the Simulation

This tutorial simulates the forming process of an aluminium pipe using a hydraulic bending machine to evaluate the mechanical stress and strain induced in the components. Figure 5 illustrates the model components and the process:

bending aluminum pipe model and process — Figure 5: Illustration of the model components and their function during the simulation.

The following modeling techniques are used to simulate the process:

Pipe deformation requires an Elastoplastic material model.
The contact areas between the pipe and the rollers change during the simulation, with contact forces driving the deformation; these interfaces are modeled as ‘Touching’ contacts.
A ‘Glued’ contact is assigned between the pipe and the stopper to prevent movement at one end of the pipe.
As shown in Figure 5, the rotating roller bends the pipe around the fixed roller; rotation is defined via a ‘Point displacement’ assigned to the small roller, using the large roller as the center.
Given that the geometry and boundary conditions are symmetric, only half of the model is simulated with a ‘Symmetry plane’ condition to optimize computational resources.

2.1. Contacts

With the analysis type selected, SimScale automatically detects several Glued contacts:

Between the small roller and the pipe.
Between the large roller and the pipe.
Between the pipe and the stopper.

The contact between the pipe and the stopper is kept as ‘Glued’ to ensure no relative motion between contact nodes. The other two relationships are manually updated to ‘Touching’ contacts to capture real interactions, such as separation and contact changes.

Refer to this documentation page for more information about Marc contacts.

SimScale automatically detects touching faces or edges and assigns ‘Glued’ contacts by default. In this case, three contacts are identified:

contacts items automatically created pipe bending marc — Figure 6: Automatically detected contacts.

Only the contact between the pipe and the stopper (‘Glued 3’) is required. Redefine the other two as ‘Touching’ contacts:

Navigate to the ‘Contacts’ node and select the interaction (e.g., ‘Glued 1’).
Change the ‘Connections’ setting to ‘Touching’ while keeping the default values.
Repeat this process for the second contact (‘Glued 2’).

pipe bending marc tutorial change contact type — Figure 7: Adjusting automatically identified contacts between the rollers and the pipe to allow for *Touching* contact modeling.

2.2. Connectors

Under the Connectors node, establish a remote point connection between the largest circular face of the small roller and a remote point. This defines a rotation using the ‘Point displacement’ boundary condition later in the setup. Create a new point under the ‘Geometry primitives’ node in the simulation tree as presented in the figure below.

pipe bending marc tutorial create point — Figure 8: How to create point *Geometry primitive*, it will later be used in the *Point displacement* boundary condition

Follow the steps outlined in Figure … :

Select the ‘+’ icon next to ‘Geometry primitives’ and select ‘Point’.
Enable ‘Face selection’ and select the largest circular face of the large roller.
Select its center coordinates by clicking the ‘Center picking’ option.
Rename the point to Center of Rotation or a preferred name.

Navigate back to the ‘Connectors’ node and select the ‘+’ icon to generate a ‘Remote point connection’. Leave the ‘Behavior’ as ‘Rigid (RBE2)’, select the created point under ‘Point’, and select the largest face of the small roller. This action links the face and the point through rigid body elements.

pipe bending marc tutorial create remote point connection — Figure 9: How to create a *Remote point connection* from the *Connectors* item

What is the difference between RBE2 and RBE3 elements?

In FEA, RBE (Rigid Body Element) connects a remote point to a set of nodes. RBE2 creates an infinitely rigid link where the remote point governs the movement of the surface, preventing local deformation. RBE3 acts as an interpolation element that distributes loads or mass without adding stiffness, allowing the connected surface to deform naturally.

2.3. Element Technology

Retain the default settings and proceed to ‘Materials’.

2.4. Assign Materials

This simulation assigns two different materials:

Steel for the rollers and stopper. This material is linear elastic as these components remain rigid.
Aluminium for the pipe. This material uses an Elastoplastic model to account for large deformations.

To create a new material, select the ‘+’ icon next to ‘Materials’ to open the materials library. Select the required material and click ‘Apply’ to create the material item:

steel material library — Figure 10: Selecting steel from the material library.

Create a ‘Steel’ material and assign it to the ‘Stopper’, ‘Small roller’, and ‘Large roller’. Other parameters remain at their default values:

pipe bending marc tutorial create steel material — Figure 11: Properties and assignment for steel. Adjusted properties define custom materials.

Repeat the procedure for the pipe using ‘Aluminium’. The ‘pipe’ body is automatically selected as it is the only remaining body without a material assignment.

Figure 10 displays the true stress-plastic strain curve for the material. Switching the ‘Behavior’ to ‘Elastoplastic’ enables permanent deformation calculation.

pipe bending marc tutorial al stress strain curve — Figure 12: Aluminium stress-strain plot. The solver follows this curve to calculate pipe deformation.

To model this nonlinear behavior, change the material ‘Behavior’ to ‘Elastoplastic’ and set the parameters as shown in Figure 13. The stress curve \( \sigma \) data is provided in the following steps.

pipe bending marc tutorial create aluminium material — Figure 13: Aluminium material properties for *Elastoplastic* behavior.

The solver requires the aluminium stress-strain curve shown in Figure 10 to predict deformation. Select the button below to download the material data CSV file:

Download Material Data

Select the ‘Table input’ icon in the material window (highlighted in Figure 10). This action opens the ‘Specify value’ window:

pipe bending marc tutorial specify value table — Figure 14: Specifying values for the material *Elastoplastic* curve.

Select the ‘Browse files’ button to upload the CSV file. The data table populates as follows:

pipe bending marc tutorial stress plast strain curve — Figure 15: Uploaded plastic material table data.

Click ‘Apply’ in the settings shown in Figure 15 to confirm the data, then select the ‘Check-mark’ icon to save the setup. This resolves the error message indicated in Figure 14.

2.5. Boundary Conditions

Refer to Figure 6 for an overview of the physical setup to inspect the boundary conditions defined in this section.

To define a boundary condition, select the ‘+’ icon next to ‘Boundary conditions’ in the simulation tree and select the required type from the dropdown menu:

pipe bending marc tutorial create boundary conditions — Figure 16: Creating a boundary condition.

A. Fixed Roller and Stopper

Define an ‘Imposed displacement’ boundary condition.

Face selection mode is active by default. To assign solid bodies, use the scene tree to switch to volume selection mode:

activate volume selection change render and selection mode — Figure 17: Activating volume selection to assign bodies to the fixed value boundary condition.

Assign the boundary condition to the ‘Large roller’ and ‘Stopper’ bodies. As shown in Figure 5, these must be constrained in X, Y, and Z (set to \(0\)).

pipe bending marc tutorial create imposed displacement — Figure 18: Applying fixed values to the large roller and stopper.

B. Symmetry Plane

The geometry includes only half of the pipe and components to optimize computational resources. To apply a ‘Symmetry plane’ condition, create a ‘Plane’ under the ‘Geometry primitives’ node by selecting a reference point at the surface of a symmetric face and setting the normal (e.g., \(n_x = 1\)).

pipe bending marc tutorial create plane — Figure 19: How to create a *Plane* in the *Geometry primitives* item

Define a ‘Symmetry Plane’ boundary condition, assign the ‘Small roller’ and ‘Pipe’, and activate the plane created previously under ‘Planes’. The ‘Large roller’ and ‘Stopper’ are excluded as they are already fixed.

pipe bending marc tutorial create symmetry plane boundary condition — Figure 20: Applying a *Symmetry plane* boundary condition to save computational resources.

How does a symmetry plane work in Marc?

In Nonlinear Mechanical (Marc), a symmetry plane acts as a rigid plate constraining planar nodes and serving as a barrier for contact interactions.

C. Moving Roller Rotation

For the small roller, define a ‘Point displacement’ boundary condition. Fix the ‘Displacement’ values to prevent translation and select the Center of Rotation under ‘Assigned points’.

pipe bending marc tutorial create point displacement — Figure 21: Applying a *Point displacement* to the *Center of rotation* point created earlier.

An equation defines the linear ramping of the angular motion in the \(r_x\) direction. Figure 19 illustrates the simulated motion from \(0^\circ\) to \(180^\circ\):

pipe bending marc tutorial start and end small roller positions with angle — Figure 22: Start and end position of the rotating roller.

A positive \(180^\circ\) rotation is required. The corresponding equation is \( \phi(t) = 180 \times t \). Select the ‘Formula’ icon in the boundary condition settings (highlighted in Figure 18) to enter the formula shown in Figure 20.

pipe bending marc tutorial specify value equation — Figure 23: Specifying the rotation angle value.

Select ‘Apply’ and the ‘Check-mark’ icon to save the setup.

2.6. Numerics and Simulation Control

The ‘Numerics’ parameters control solver precision; retain the default settings. In ‘Simulation control’, set the ‘Maximum time step length’ to \(0.05\ s\), change the ‘Write control method’ to ‘Output steps’, and set the ‘Number of output steps’ to \(20\).

pipe bending marc tutorial change simulation control — Figure 24: Simulation Control settings.

2.7. Result Control

‘Result control’ defines the output fields. In addition to the defaults, a ‘Contact result’ field is required.

A. Solution Fields

Select the ‘+’ icon next to ‘Solution fields’.
Select the field type and create a ‘Contact result’ field.
Change the ‘Contact result type’ to ‘Pressure’.

pipe bending marc tutorial create solution field — Figure 25: Creating a solution field for results visualization.

B. Volume Calculation

Volume calculations report field statistics over a part. Define a ‘Volume calculation – Min-max’ item for the ‘von Mises stress’ over the ‘Pipe’ as shown in Figure 24.

pipe bending marc tutorial create volume calculation — Figure 26: Volume calculation settings for **‘von Mises stress’**.

3. Mesh

This tutorial uses the standard mesh algorithm with default general settings:

Global mesh settings pipe bending — Figure 27: Mesh settings for the standard algorithm.

Apply local refinements to optimize resources. An ‘Extrusion mesh refinement’ improves the mesh in thin sections. Follow the steps in Figure 26 to define the refinement.

Add mesh refinement extrusion refinement pipe bending — Figure 28: Adding an **‘Extrusion mesh refinement’** item.

Assign the refinement to the pipe faces (Figure 27). Set ‘Sweep sizing type’ to ‘Number of elements along sweep’ at \(2\), use ‘Quad dominant’ as the ‘Surface element type’, and set a ‘Maximum edge length’ of \(4 \times 10^{-3}\ m\).

pipe bending marc tutorial mesh create extrusion refinement — Figure 29: *Extrusion mesh refinement* settings assigned to the pipe.

pipe bending marc tutorial final mesh — Figure 30: Visualization of the generated mesh.

4. Start the Simulation

Create a new run by selecting the ‘+’ icon next to ‘Simulation Runs’:

pipe bending marc tutorial create simulation — Figure 31: Creating a new simulation run.

Important

When you create a simulation run, the following warning message will appear:

warning message simulation — Figure 32: Ignore this warning message for this tutorial. Select **‘Run anyway’** to proceed.

For this tutorial, the run will be successful, so the warning message can be ignored by clicking the ‘Run anyway’ button.

5. Post-Processing

Once the run is successful, open the online post-processor using the ‘Solution Fields’ node or the ‘Post-process results’ button (Figure 31).

pipe bending marc tutorial access solution fields — Figure 33: Accessing the online post-processor.

5.1 Deformations

By default, ‘Displacement Magnitude’ is selected for ‘Coloring’ under ‘Parts Color’. Select ‘Von Mises Stress’ instead, right-click the legend and select ‘Use Continuous Scale’ to improve result visualization (Figure 32).