Reporting and Plotting the Pressure Drop

Create reports of average pressure at the inlet and outlet boundaries, and use the reports in a field function that gives the pressure drop.

Experimental measurements are available for the pressure drop across the flow restrictor when the flowrate is 28.09 liters/s. These can be compared to the prediction of pressure drop for this simulation to give some estimate of the accuracy of results. To do this, it is necessary to create reports of average pressure at the inlet and outlet boundaries, and to use these reports in a user-defined field function that gives the pressure drop. This field function can be plotted while running the simulation to estimate convergence.

The upstream static pressure was measured at a distance of two pipe diameters before the restrictor, and the downstream static pressure was measured at a distance of six pipe diameters after the restrictor. The inflow boundary corresponds to the upstream measurement, but a section plane must be created at the point of the downstream measurement. The section plane is created first:

  1. Right-click the Derived Parts node and select New > Section > Plane Section

    The Create Plane Section dialog appears in place above the object tree.

  2. In the Input Parts box, select Fluid.
  3. In the Plane Parameters box, set Y origin to -0.239014 m, the X normal to 0 m, and the Y normal to 1 m. The other parameters can be left as they are.
  4. In the Display box, select No Displayer as shown below.


  5. Click Create, and then Close.

    A new part that is called Plane Section is added to the object tree inside the Derived Parts node.

Create the reports that are used to extract the static pressure:

  1. Right-click the Reports node and select New > Metrics > Surface Average.
  2. Rename the Surface Average 1 node to Upstream Pressure.
  3. Select the Upstream Pressure node and set Scalar Field Function to Pressure.
  4. Click the right side of the Parts property. In the dialog that appears, expand the Regions and Fluid nodes and select the Inflow boundary as shown below.


  5. Click OK.

A similar report is created for the downstream pressure:

  1. Right-click the Reports node and select New > Metrics > Surface Average.
  2. Rename the Surface Average 1 node to Downstream Pressure.
  3. Select the Downstream Pressure node and set the Scalar Field Function to Pressure and the Parts to Plane Section.

    The completed Properties window appears as shown below.



Two new field functions corresponding to these reports have been automatically added to the object tree.

  1. Open the Automation > Field Functions node and scroll down to see the new nodes:


Examination of the properties for these nodes shows that the relevant field function names are DownstreamPressureReport and UpstreamPressureReport respectively. These function names are used to create an expression report for the pressure drop:

  1. Right-click the Reports node and select New > User > Expression.
  2. Rename the Expression 1 node to Pressure Drop.
  3. Select the Pressure Drop node.
  4. Click (Custom Editor) to enter the Definition property as:

    $UpstreamPressureReport - $DownstreamPressureReport

  5. Click OK.


  6. Click (Custom Editor) for the Dimensions property. In the Pressure Drop - Dimensions dialog, set the Pressure dimension to 1 as shown below.


  7. Click OK.
  8. Finally, set the Units to bar.

    The Properties window for the Pressure Drop report appears as shown below.



A monitor and plot is created from this report.

  1. Right-click the Reports > Pressure Drop node and select Create Monitor and Plot from Report.


    The resulting monitor and plot can be seen in the object tree:



  2. Right-click the Plots > Pressure Drop Monitor Plot and select Open from the pop-up menu. The empty plot is displayed.
  3. Save the simulation.