# Linear static analysis of a crane¶

Note

The content of this tutorial is not up to date with the current live version of SimScale. The tutorial setup and the results are still valid! Please do not get confused if styles like buttons and entity names have changed in the meantime.

In the following you find a step-by-step instruction for the linear static analysis of a crane structure.

Import tutorial case into workspace

## Step-by-step¶

### 1) Import tutorial project¶

• To start this tutorial, you have to import the tutorial project into your ‘Dashboard’ via the link above.
• Alternatively, you can also add the tutorial project from the ‘Public Projects’ library by searching for ‘tutorial’.
• Clicking on the project, then clicking on ‘Actions’ and ‘make a copy’ option to add it to your ‘Dashboard’. This process is illustrated by the figures below.
• Once the project is in your ‘Dashboard’, simply move the mouse over to the upper right corner click on the blue icon to open it in your workbench as shown in figure below.

• Once the ‘Work bench’ is open you will be in the ‘Mesh creator’ tab.
• The Mesh Creator tab is the place where you upload CAD models and create meshes for them.
• The geometry is already available under the ‘geometry’ tree item.
• After a few moments, the CAD model is displayed in the viewer like shown in the figure below
• You can interact with the CAD model as in a normal desktop application

The CAD model displayed in the viewer

### 3) Create a mesh¶

• In order to create a mesh click on the “mesh geometry” button.

• For a solid mechanics simulation you should either use the Fully automatic tetrahedralization or the

Parametrized tetrahedralization algorithm (see Fully automatic/ Parametrized tetrahedralization). The first one is always helpful if you have limited information about your geometry properties or if you aim for a first quick solution. In this tutorial we choose the parameter dependent Parametrized tetrahedralization.

• The crane structure is approximately ten meters long. We choose 0.2m as Maximum mesh edge length and 0.02m as Minimal edge length and thus force the algorithm to create element edges within these limits. We create a first order mesh and select moderate fineness for the NETGEN3D fineness parameter. Furthermore it is recommended to keep the Activate NETGEN3D optimization option true.

Meshing parameters for the Parametrized tetrahedralization

• After setting all parameters save your selection and start the meshing operation. Use the notifications panel on the lower left to check the status of the meshing process. As soon as the mesh is finished it is loaded into the viewer and you can interact with it in the same way as with the geometry before.
• Use the operations log to get some general informations about the mesh e.g. number of nodes and elements in the mesh. For the suggested configuration your mesh should have around 38000 nodes.

Mesh visualization in the Viewer

### 4) Specify the simulation properties¶

• Switch to the Simulation Designer and add a new simulation.
• In a first step you have to choose the general simulation type. You can get some information about the different types on the right. In this tutorial we want to calculate the displacement and stresses of the crane structure due to a lifted load without considering dynamic effects or thermal conditions. Hence we choose Static from the Solid mechanics selection.

Simulation type choice

• This will create a tree entry that needs to be completed.
• In the model section you can now assign a mesh to your simulation design. Choose here the previously created mesh. After you have saved your selection the mesh should be displayed in the Viewer on the right.
• You can choose if you want to take geometric nonlinearities into account and apply a gravitational load on the whole domain in the Model section. In order to specify a gravitational load you have to determine the magnitude and the direction of the gravity field. We choose a linear calculation and apply a gravitational load of 9.81 m/s² in the -y direction (direction vector: 0 -1 0).
• The material is specified in the Materials section. You can add a new material by clicking on Add new material and assign a name to it. Currently linear elastic and plastic materials are supported. In this tutorial we choose Linear elastic. Thus one has to determine a Young’s modulus (unit Pa = N/m²) and a Poisson’s ratio. Furthermore the density is used to enable gravitational loading. As the default values are typical for steel one can use them for the crane structure.

General properties for the simulation of the crane structure

• Use the Boundary conditions section and apply loads or constraints respectively. A new boundary condition can be added with the Add new ... boundary condition Buttons.
• As the crane should be fixed on the one end add a new constraint boundary condition. With Fixed value one can prescribe a specific displacement, fix the boundary to zero or leave it unconstrained ( not fixed). We choose fixed and zero (0) for all three directions.
• In order to apply the boundary condition on the desired geometrical entities, we choose Pick faces (preselected) and pick the three faces at the end of the crane structure. The selected faces are now highlighted in red.
• You can simply assign the boundary condition to these faces by clicking on Assign selection from viewer.

Fixed boundary of the crane

• Now that the structure is fixed we apply the load.
• Therefore add a force boundary condition in the Boundary Conditions section. We simplify the load caused by a lifted body by a negative pressure (force F boundary condition: Pressure) on the lower face of the box at the end of the crane opposite to the fixed boundary condition.
• The load is assumed to take the value 10000N. As pressure is a distributed loading type it is necessary to apply the load using N/m² as unit. So we divide the load by the area of the face (0.25 m²) and get a value of 40000 N/m².
• The assignment to the lower face of the box is carried out in the same way as before for the displacement boundary condition. Please make sure, that the fixed faces are not selected anymore (Select none) and save the boundary condition at last.

• In the Numerics section you can choose the linear equation system solver. In this tutorial we use the direct solver Spooles that behaves well for most problems. The iterative solvers may have advantages considering memory usage and calculation time though.
• If you followed the settings of this tutorial so far especially

considering the mesh fineness it is possible to select one computing core for the calculation in the Simulation Control section.

• For finer meshes it may be necessary to choose a larger instance in order

to provide memory and reduce calculation time. In that case please check the informations for a professional account in Upgrade to Professional. The Maximum runtime is a control limit if the simulation does not converge for example.

### 5) Start a simulation run¶

• At last create a simulation run that holds the current configuration of your simulation and simply start your calculation by clicking on the Start button.
• The Notifications area on the lower left provides information on the status of your current run. Once the calculation has finished you get a notification E-mail as well.