Documentation

This result control item allows calculating forces and moments in the course of the simulation by integrating the pressure and skin-friction over a boundary. It is possible to select a set of boundaries to calculate the overall force and moment on them.

It can be added under *Result Control* in the simulation setup tree entry.

The *Center of rotation* is commonly defined as the center of mass of the structure. In some simulation projects, it may be convenient to define different coordinates for the center of rotation. For example, if a part is attached to the ground at a specific point, you can use the coordinates of this point to obtain the resulting moments.

*Write interval* controls how often the force and moment values should be output/written. The value is the number of *time steps* between the outputs.

Values of force and moment are printed in the solver log. The plots are updated while the simulation is running. The figure below shows a sample plot of forces and moments:

Alternatively, it is possible to calculate force and moment coefficients instead of force and moment values. In addition to the previous parameters, the user should supply lift, drag, and pitch directions, as well as freestream velocity magnitude, reference area, and reference length. The results are available in the simulation log and as plots.

Multiphase flow simulation, as the name suggests, models two fluids of different densities and their interaction with each other in the flow domain. This is done through a phase fraction variable \(\phi\) that takes a value of *0* for one fluid and *1* for the other.

Depending on the case, one might be interested in computing the cumulative force of both or only one of the fluids on the object they interact with. For example, in the simulation of a boat sailing on a water surface represented by the following figure, one could calculate the net drag force on the boat due to both water and air, or only one of them.

Find below the procedure to compute this cumulative force and how to separate forces using the phase fraction.

To post-process your results locally, ParaView should be installed on your computer. Depending on your operating system, the appropriate version of ParaView can be downloaded from here.

**Step 1: Download and Open the Results**

Once a simulation is completed on the SimScale platform, the results can be downloaded to your local system. See Post-processing via a 3rd-party solution for a detailed description of how this can be done. By default, ParaView loads the entire data set. However, the interest now lies only in computing the forces on certain specific faces of the body. Therefore, before opening the case, please make a list of these faces.

- Start a new session on ParaView.
- Click on
*File*–*Open*, select the*case.foam*, and press ‘**OK**‘. - In the
*Mesh Regions*section in the*properties*tab (see figure), select only those faces on which the force needs to be computed. - Click on ‘
**Apply**‘. The case should now be loaded on ParaView. - From the time navigation panel, go to the time-step at which you are interested to compute the forces.

ParaView works as a sequence of filters applied to objects in its pipeline.

- Select ‘
**case.foam**‘ in the pipeline browser. This sets the active object for the filters. - Click on ‘
**filters**‘ and choose ‘**Generate Surface Normals**‘ from the list. A new object called*GenerateSurfaceNormals1*will be created in the pipeline. - Several parameters can be used to adjust the result of this filter. See this for a detailed description. Once finalized, click on ‘
**Apply**‘. ParaView computes the result and automatically sets*GenerateSurfaceNormals1*as the new active object.

**Step 3: Calculate the Forces**

In Step 2, we computed the normals on the faces of interest. These normals are scaled according to the area of the respective faces. Since we already have the pressure data on these faces, we can now easily compute the net force on each face.

- Click on ‘
**Filters**‘ and pick ‘**Calculator**‘. A new object*Calculator1*is created in the pipeline. - If need be, change the
*Result Array Name*to something relevant, such as ‘Forces’. - Force is computed as \(prgh . \vec{n}\), where \(prgh\) is the static pressure, and \(\vec {n}\) is the surface normal. Depending on what you want to calculate:
- For total force, due to both phases, enter “p_rgh * Normals” in the text box.
- For force due to only one phase, enter
- “p_rgh * Normals * alpha.phase1” for the phase which corresponds to \(\phi\) = 1.
- “p_rgh * Normals * (1 – alpha.phase1)” for the phase which corresponds to \(\phi\) = 0.

- Click on
**Apply**. The force value is now available for each face.

For example, in the figure below, we are calculating the forces generated by *alpha.phase1* onto the boat:

Note

The reason why density is not required as input is because we already know the static pressure. Therefore, simply multiplying with the area is sufficient to compute the force.

**Step 4: Integrate the force over the faces**

The result of Step 3 is local to each face. To get the net force on all faces, this result needs to be integrated.

- Click on ‘
**Filters**‘ and then choose ‘**Integrate Variables**‘. - Click on ‘
**Apply**‘.

A spreadsheet view opens up. The *Forces* tab displays the net force value (in Newtons) in the three coordinate directions.

Last updated: May 26th, 2021

We appreciate and value your feedback.

Sign up for SimScale

and start simulating now