FreeCAD CFD Workbench with OpenFOAM v2106

1: FreeCAD 0.19.x AppImage: If you don’t have FreeCAD installed, you may refer to the latest FreeCAD installation tutorial from Solvercube LearnPress (registration not required for free articles). Also check out channel videos from Solvercube Channel.

2: OpenFOAM v2106: To install OpenFOAM, refer to the latest OpenFOAM installation tutorial from Solvercube LearnPress (registration not required for free articles). Also check out channel videos from Solvercube Channel.

3: ParaView 5.9.1: To install ParaView, refer to the latest ParaView installation tutorial from Solvercube LearnPress (registration not required for free articles). Also check out channel videos from Solvercube Channel.

Launch FreeCAD, and open one of the example models from the Start page. Right-click on the graphics screen to select Navigation styles  Gesture. Under this scheme, mouse operations are as follows:

You can also control the viewport using the Keyboard Navigation keys:

Note that FreeCAD GUI (Graphical User Interface) has many toolbar icons to boost productivity. I suggest reducing the toolbar icons size so that more icons be visible at once: Visit the Edit  Preferences…​ menu, and select Small (16px) for the Size of toolbar icons (from the Main window section).

Also, from the main GUI layout, relocate the View toolbar

from the default position (the forefront of the second row) to the rear end of the first row. It will leave more space spared for the workbench tools we are going to use in this tutorial.

0.1: Launch FreeCAD and go to the Tools  Addon manager menu. Locate the Plot addon and click the Install/update selected button to install it. When the the process is complete, shut down the Addon Manager by clicking Close, and then restart FreeCAD.

0.2: In the same manner, install the CfdOF addon and restart FreeCAD accordingly.

1.1: Start FreeCAD from a local work folder. Visit the Preferences panel (i.e. Edit  Preferences…​) and specify the local folder for the CfdOF solution data.

1.2: Also, I prefer to be working with the MKS (m/kg/degree) units — i.e. rather than the CAD-conventional mm-based system. Change the Number of decimals value to 5 accordingly.

To try out the CFD Workbench, we will create an S-shaped pipe of a constant circular cross-section (16" SCH 40). We then solve the internal flow field for the water transport, with turbulence modelling inclusive.

2.1: Select Part Design from the workbench selector (currently showing as ). Click the (Create a new document) icon in the toolbar area to start the Part Design module.

2.2: Let us close (or detach) the Report view panel from the layout for now — either using the View  Panels menu or by the panel’s close button. (It will come back anyway whenever FreeCAD needs to inform you of something.)

2.3: Click Create body under the Tasks tab in the Combo View panel; This area will be dubbed simply as the Tasks pane from now on — unless a specific task panel name is better mentioned.

2.4: Click the Model tab to switch to the modelling tree view. See that one (and only) Body object is added under the Unnamed document root. Click the (Create a new sketch) icon from the toolbar to invoke the Sketcher module.

2.5: First, we will create a circle with 381 mm of (inner) diameter to define the cross-section. Select YZ_Plane either from the graphics area or the list in the Tasks pane. Click OK to confirm the plane selection.

2.6: Click (Create a circle in the sketch), hover the mouse cursor towards the origin point — until the point colour turns to grey — to pick it as the centre of the radius. Then, click anywhere on the +X+Y quadrant to define the 2D circular wireframe.

2.7: Click the (Constrain diameter) icon from the toolbar (You may need to click the small triangle on the right of the (Constrain radius) icon). Select the circumferential edge to enter 0.381 m  — or 381 mm — for the Diameter in the Change diameter dialog, and then click OK. Confirm the sketch by clicking Close in the Task pane.

2.8: Make the viewport to fit to the geometry — either using the view control context menu (right click on an empty spot) or by pressing the V F key combination.

2.9: Now, we will create another wireframe to define the path profile. Click (Create a new sketch) again, select XZ_Plane, and then click OK. Adjust the graphics view so that the previous sketch projection (showing as a white line) be positioned in the lower-left corner.

2.10: Click the (Create a polyline) icon from the toolbar, and starting from the origin point, draw three (3) line segments (similar to the below example). Make sure each line segment be defined with either the horizontal () or vertical constraint () imposed. Finish creating the polyline by clicking the right mouse button.

2.11: We will then define two (2) 90° bends between line segments. Click (Create a fillet) from the toolbar, pick the first edge and then do the vertical one to insert the first fillet. You do not need to press and hold the Ctrl key as the filleting naturally expects two (2) consecutive inputs. With the ghost cursor still attached — i.e. you being in the filleting mode (if not, click again) — create the second fillet between the vertical and the last edges.

2.12: Finalise the profile sketch by assigning the following dimensional values:

2.13: When the profile sketch is complete, click Close in the Tasks pane to exit from the Sketcher. Adjust the viewport so that you can see the two (2) sketches in the graphics screen.

2.14: Now, with both Sketch and Sketch001 selected in the model tree, click the (Sweep a selected sketch) icon to build the pipe section. Click OK in the Tasks pane to confirm.

2.15: Save the current FreeCAD document to a local work folder before we proceed with the CFD Workbench.

Our preferred meshing tool for the CFD Workbench is the cfMesh software developed by Creative Fields Holdings Ltd. It has been incorporated since OpenFOAM v1712, thus you do not need to install it externally.

3.1: Select CfdOF from the workbench selector, and then click the (Create an analysis container with a CFD solver) icon from the toolbar. Make sure one (and only) CfdAnalysis object is added to the model tree.

3.2: Select the AdditivePipe object in the model tree to define the meshing scope, and then click (Create a mesh) from the toolbar. When the CFD Mesh panel opens, initiate your meshing task by clicking the Write mesh case button.

3.3: Give the Base element size value with 50.8 mm  — or 0.0508 m — and click Write mesh case again. Then, click the Run mesher button to generate a preliminary mesh. When the meshing job is complete, check the surface mesh distribution by the Load surface mesh button.

3.4: Note that the surface mesh visualisation is just a "triangulated" representation (i.e. NOT the real mesh elements). To examine the actual mesh structure, you better use ParaView by the Paraview button. We will refine the mesh after we assign boundary conditions, so for now, exit from the mesher by clicking Close.

The physics involved in this exercise is chosen arbitrarily with the flow Reynolds number (based on the pipe diameter) being at 3.8 x 10⁵. Relevant turbulence modelling parameters can be easily estimated using online tools such as one provided by CFD Online.

4.1: In the model tree, expand the CfdAnalysis branch to reveal the objects under it. First, double-click the PhysicsModel object to enable the Viscous and then the RANS turbulence options. Click OK to confirm.

4.2: Double-click the FluidProperties object in the model tree, and select Water from the Predefined fluid library. Accept the default values for the Density and the DynamicViscosity values, and then click OK to close.

4.3: Double-click the InitialiseFields object in the model tree. Enable Specify values for Velocity and leave the values of 0 m/s in the Ux, Uy, and Uz fields. Similarly, tick on the Specify value option for Pressure with the default value 0 Pa. For the turbulence parameters, feed the following values:

Click OK to confirm.

In this example, we will assign 1 m/s of inflow from the left end which exits through the right end.

5.1: Click (Create a CFD fluid boundary) to define the velocity inlet boundary. Rotate the view angle so that you can pick the left cross-sectional area using the left mouse click. With the selected surface highlighted in green, click the Add button in the Tasks pane.

5.2: Change the Boundary type to Inlet, and then enter the value of 1 (m/s) for the Ux field. Select the Intensity & Length Scale option for the Turbulence specification and feed the same values as for the initial field ones:

Click OK to confirm.

5.3: Similarly, we will assign the pressure outlet boundary condition, but this time, click the opposite cross-sectional area first and then click the (Create a CFD fluid boundary) icon. This will open the CFD boundary condition panel with the Boundary face list filled accordingly.

5.4: Change the Boundary type to Outlet and leave the remaining parameters as they are. Click OK to confirm.

5.5: We might continue on selecting all other faces to define a no-slip "wall" boundary condition. But doing so makes picking the same faces for boundary layer generation a bit tricky. Instead, we better handle this in the Boundary wall treatment section.

In this section, we make use the inherent mesh refinement functionality as a way to group target wall region(s) for assigning appropriate refinement strategy.

6.1: Select the main mesh object — i.e. the one labelled as AdditivePipe_Mesh in this example — and then click the (Create a mesh refinement) icon.

6.2: Pick the five (5) wall faces from the graphics, and then click the Add button in the Mesh refinement panel to add them to the References list.

6.3: Tick on the Boudanry layers option from the Mesh refinement panel and increase the Number of layers to 4. Leave the other as they are and click OK to close.

6.4: From the model tree, expand the AdditivePipe_Mesh entry and rename the MeshRefinement entry to a more intuitive name such as "WallFaces". Now, click the (Create a CFD fluid boundary), click Select from list, and then select the WallFaces for the Select Object list control. With all the five (5) faces selected, click OK. Turn the visibility off for the newly created wall object in the model tree.

With the boundary mesh generation parameters, we need to revisit the meshing task.

7.1: Double-click AdditivePipe_Mesh in the model tree. Initiate by clicking the Write mesh case button, and then click Run Mesher. When the meshing job is done, quickly check the surface mesh distribution by Load surface mesh.

7.2: You may launch ParaView to examine the actual mesh structure — i.e. either by the Paraview button (if it works) or by launching one manually (See Step 3.4). After a brief investigation, exit from ParaView. Also, exit from the meshing panel by clicking Close.

7.3: Note the FreeCAD changes the visibility status for individual objects as necessary. That said, you may turn on/off their respective visibility any time. It is also a good idea saving the FreeCAD document before we continue on to solving.

Now with the geometry and mesh ready, you can go on to solve the model using the OpenFOAM solver.

8.1: Double-click the CfdSolver object in the model tree and instantiate the case data by clicking the Write button. This constructs the 'case' folder in your work folder with the set parameters.

8.2: Click Run and monitor the residuals from the plotting window. Convergence seems to get stalled and wavy after around 500 iterations (possibly due to flow transient). Stop the run after around 1000 iterations.

Unfortunately, the Analysis control panel is not fully implemented for handling solved data yet. You have to navigate to the case folder and complete the remaining post-processing tasks.

9.1: Click the Edit button to open the case root directory.

9.2: Open a terminal by right-mouse-clicking to select Open in Terminal from the context menu. For partition-decomposed cases, you first need to reconstruct the solution data using the reconstructPar command.

Then, launch ParaView by entering:

9.3: Spend some time to investigate the result by plotting pressure contours, velocity vectors, etc.