Computational Fluid Dynamics (CFD) simulation using Abaqus

Setting up a simple Computational Fluid Dynamics (CFD) simulation in Abaqus.

Laminar flow through a cylinder is a very well documented CFD problem. This tutorial will go through the steps of making the model, assigning material properties, creating a mesh, setting up the boundary conditions and visualizing the results using the student version of Abaqus 6.14 (Student edition). The size of the mesh is kept to a minimum so that the simulation can be run on any machine. By following the instructions in this tutorial one should be able to make a simple model, run the simulation and visualize the result.

Making the geometry of the model

When the link to Abaqus student edition is clicked a screen similar to figure 1 appears. Select "With CFD Model" option.

Figure 1. Abaqus model database selection screen.

In the top left corner of the Abaqus screen, expand the Model-1 option and double click on Parts. A screen similar to figure 2 is seen. Leave the default options. Click on continue. This will bring up the options displayed in figure 3. A rectangular simulation box of dimension 33 x 16 x 0.2 is required for the current simulation. Click on create a rectangle option as shown in figure 3.

Figure 2. Creating a Part in Abaqus.
Figure 3. Creating a rectangular simulation box.

The bottom of the screen prompts the user for picking a starting corner for the rectangle – or enter X,Y. Enter 0,0 as the starting corner and hit enter. The user will be prompted to pick the opposite corner for the rectangle—or enter X,Y. Enter 33,16 and hit enter. Click on the red (X) option on the bottom of the screen as shown in figure 4.

Figure 4. Click option to create part.

The user will be prompted to Sketch the section for the solid extrusion. Click "Done" to continue on to the next screen. We have entered the X and Y dimension of the model. Once the "Done" button is clicked, a screen similar to figure 5 is displayed. Enter 0.2 as the value of depth. Click "OK" to see the rectangular model created.

Figure 5. Z dimension of the model.

The next part involves creating a circular hole that represents the cylinder. From the top menu bar go to Shape. Under shape menu, go to the cut option. Under the cut menu, go to the Circular Hole option. Select the Type of hole as "Through All". Select XY plane for the hole.Check the direction of the hole to make sure that the hole is cut through the model in the correct direction. The user will be prompted to select the first edge from which to locate the hole. Select the top X direction edge of the model. The cylinder will be located at a distance of 8 m from the top of the model. The user will be prompted to select the second edge from which to locate the hole. Select the extreme left edge in Y direction. The cylinder will be located at a distance of 8 m from the front of the model. Enter the diameter of the model as 1m.

The model will be partitioned in the center horizontal direction to control the meshing in the wake region. This partitioning will help in maintaining the size of mesh in the area of interest. Several approaches can be used to achieve this. As the user becomes familiar with using Abaqus and meshing techniques, mesh refinement study can be carried out to study the effect of mesh size on the accuracy of the results and the computational cost. From the main menu bar go to the Tools option. Under Tools, select Datum option. This will open the Create Datum GUI. Select the Plane radio button. Under the plane menu select 3 points option. Use figure 6 as a guideline to select the three points to create a datum plane. Hold the shift button when the three points are selected.

Figure 6. Creating a datum plane.

The datum plane created earlier will aid in partitioning the model. From the main menu go to Tools sub menu. Under Tools select Partition option. This will open up create partition GUI. Select the Cell radio button in this GUI. Select the use datum plane option. This will prompt the user to select a datum plane. Select the datum plane created in the preceding section. Select the Create Partition button. Select the Done button. Rotate the model to examine the partition just created.

Assignment of material properties to the model

In the main menu bar go to the Material sub menu and select the create option. This will open up the Edit Material GUI. Go to General tab and select Density. Enter a value of 1 $kg/m^3$ for density. Go to Mechanical tab and select Viscosity option. Enter a value of 0.01 $kg/ms$. Click OK button on the bottom left corner of the Edit Material GUI.

The next step will be creating a section. From the main menu bar go to Section option and select the Create option. This will open Create Section GUI. Leave everything at default Fluid-Homogeneous option. Click the Continue button on the bottom left corner of Create Section GUI. This will open Edit Section GUI. Leave everything at default values in the GUI. Click the OK button on the bottom right corner of Edit Section GUI.

Once the section is created, the next step will involve assigning this section properties to the model. From the main menu bar go to Section sub menu. Under the Section menu bar select Assignment Manager option. This will open the Section Assignment Manager GUI. Click on the Create button. This will prompt the user to select the region for section assignment. Select the entire model and click OK on the bottom left corner of Edit Section Assignment GUI. This will change the color of the model on screen to green. The green color indicates that the material properties have been assigned to the model.

Creating mesh for the model

Once the material are assigned to the model, the next part will be meshing the model. In the module sub menu bar select the Mesh option. Once the mesh option is selected, from the top menu bar select the seed menu and click on Part option. This will open the Global seeds GUI. Set the Approximate global size of the model to be 1. Next, select the Seed menu from the top menu again and this time select the Edges option. The user will be prompted to select the regions to be assigned local seeds. Select the edges on the cylindrical region of the model. Since we are interested in the flow around the cylindrical option, we want the mesh in this region to be such that it captures the details of the flow. In the Local Seeds GUI, enter the Approximate element size to be 0.1. Also, follow the same procedure for the edges that connect the cylinder to the inflow and outflow region and set the Bias for these edges to be single. Also, for these edges enter minimum size to be 0.1 in the region near the cylinder and maximum size to be 1 in the region near the inflow and outflow. This will maintain an adequate mesh size. Once seeding of edges is accomplished, the next step would be meshing the model. From the main menu, go to Mesh and select the part option. The user will be prompted if it is OK to mesh the part? Select Yes option. The mesh will be generated once this option is selected. The user can try different option to generate the mesh. There are several different approaches that can be used to generate mesh. With experience, this procedure should be straight forward.

Assembling the model

Once the mesh is generated, double click the Assemble button under Model Database on left hand top corner. This will activate the assembly module. From the main menu go to Instance option. Under the Instance menu select the Create option. This will open the Create Instance GUI. Select the part you just created. Click OK on the bottom left corner of the Create Instance GUI.

Creating Step

Double click the Step button under Model Database on left hand top corner. This will open the Edit Step GUI. Set the time period to 350. Leave all the other options to default setting.

Assigning Boundary Conditions

In the model database toolbar, double click on the BCs tab to open the Create Boundary Condition toolbar. Select the CFD Step in the Step option. Click the fluid radio button. Select the Fluid inlet/outlet option for the inflow and outflow. Follow figure 7 to set the inflow, outflow, symmetry, and top-bottom boundary conditions as follows:

Inflow:V1=45, V2=0,V3=0 Outflow: Specify Pressure=0 Top-Bottom:V1=45, V2=0,V3=0 Sides:Symmetry boundary condition by specifying V3=0

Figure 7: Boundary conditions

Running CFD Simulation

In the model database toolbar, under the Analysis option, double click on the Jobs Tab. This opens up the Create Job GUI. In the Name option, give an appropriate name to the job, select the model that was created for the CFD job. Click continue on the bottom left corner of the GUI. In the Edit Job GUI, give a description of the job in the Description menu. Click OK. Right click on the CFD job that was just created and select the Submit option. Once the job is submitted, monitor the job by right clciking on the job and selecting the monitor option.

Visualizing Results

Once the job has completed, or even when the job is running, the user has the option to open the odb file and visualize the results. It is assumed that the user has the ability to visualize the data in Abaqus. Figure 8 displays the velocity contours from the job created using the above instructions.

Figure 8: Velocity plot

Animation of Velocity profile displaying vortices

Figure 9 displays the animation of velocity contours generated from the Abaqus CFD outout. Contours generated due to the obstruction of flow can be easily seen.

 Figure 9: Animation of velocity plots displaying vortices formed due to flow separation.