What is a “Vortex Across a Pressure Boundary?”

In Flow Simulation,  a vortex is a region in the fluid domain which causes a swirl in a region where there is asymmetric drag in the flow field. The vortex itself is an expected phenomenon and is not problematic. When that vortex is allowed to generate across a theoretical boundary, within a CFD analysis, this can cause the results to deviate from reality in the immediate vicinity of the boundary. It can also cause the solver to fail to produce results. For that reason, it is important to note where this is happening in an analysis and take steps to avoid it.

Figure 1: The Flow Simulation solver will show this warning when a vortex is occurring across a pressure boundary.


How can this be fixed?

The vortex itself is generating because of the local solid geometry near the pressure boundary of a CFD setup. If the flow through the boundary is not symmetric, a low-pressure region can generate in front of the boundary and allow fluid to pass the wrong direction through the boundary as intended. The fix for this is to “build out” the model geometry. This means that the solid model needs to have more of the real life geometry added to the setup so the flow field can be allowed to have the vortex and then transition into a unidirectional flow.

Solution 1: Add Geometry

An example of a vortex across a boundary would be directly from the first Flow Simulation tutorial in SOLIDWORKS (the tutorials can be found under ‘Help’, ‘SOLIDWORKS Simulation’, ‘Flow Simulation Online Tutorial’ once the Flow Simulation add-in is turned on). The ball valve, as it is setup in the tutorial, has two lids that are positioned closely to the ball of the valve. In situations where the ball valve is not set completely open the flow through the valve is forced to be asymmetric as it passes through the pressure outlet.

The asymmetric flow out the pressure boundary allows fluid to backflow through the theoretical pressure boundary and creates the vortex that is seen in below.

flow simulation
Figure 2: Asymmetric flow through a ball valve shows a vortex occurring on the pressure outlet boundary.


Since the issue only exists on the outlet side of the model; that is the only side that needs to be “built out”. In this example, a straight pipe is placed off the end of the valve extending the fluid region and moving the pressure boundary further away. In this way, the flow can have a vortex and then be allowed to transition into a unidirectional flow as it might in real life. Figure 3 below shows that the vortex downstream from the valve remains but is now allowed to fully form before leaving the fluid domain.

flow simulation
Figure 3: A straight pipe added to the end of the ball valve shows how the pressure boundary can be moved away from the vortex that is being formed.


Solution 2: Release to Pseudo-External Environment

Solution 1 is possible when it is reasonable to assume there is more piping after the valve that can be put into place. This is not always true. Solution 2 examines how to handle the valve’s behavior when releasing into a larger reservoir. An entire tank could be modeled to resolve this vortex across boundary warning or this could be modeled as an external analysis but that would make the Flow Project take prohibitively long to solve if the valve is the only thing being analyzed. In this case, it may be suitable to model only a portion of the tank where fluid plume flows into. This setup is shown in Figure 4.

Figure 4 shows a small modeled enclosure attached to the ball valve.


Only a part of the tank is modeled so on 5 of the 6 internal surfaces, a pressure boundary is defined that will represent the undefined fluid volume in the rest of the tank. The face immediately adjacent to the valve is not applied with pressure so as to represent the tank wall. The result is that the fluid plume generates in the now open region beyond the valve allowing, again, for the vortex as the valve to generate and then dissipate as shown in Figure 5. In this case, however, a warning for vortex crossing the pressure boundary will still likely generate but will impact the results at locations away from the valve exit and the fluid plume.

Figure 5: The fluid plume generates in the pseudo-external environment created attached to the valve


Where possible create a solid model where a vortex will not cross a pressure boundary or move the pressure boundary itself away from the region of interest in the fluid domain.

Author:  Ryan Dark
Ryan has been in the GoEngineer technical support team since February 2008 where he most notably provides support for all FEA and CFD software offered by SOLIDWORKS. His most recent accolade is the title of Elite Application Engineer awarded by SOLIDWORKS Corp.



GoEngineer delivers software, technology and expertise that enable companies to unlock design innovation and deliver better products faster. With more than 30 years experience and thousands of customers in high tech, medical, machine design, energy and other industries, GoEngineer provides best-in-class design solutions from SOLIDWORKS, Stratasys, CAMWorks, Altium and Product Lifecycle Management (PLM). For more information, visit goengineer.com.

Categories: SOLIDWORKS Flow Simulation, SOLIDWORKS Simulation, Tips & Tricks, Usability

Last comment By: FlowJoe   Wed, 22 Mar 2017 13:45:00 +0000
By: FlowJoe
There is a specific testing standard for valves, so one would need to set up the virtual simulation model exactly how it would be tested in a real-world scenario. This is also true in general and not specifically for the valve industry. Solution 1: Add Geometry would be the preferred option, but with the addition of geometry on the inlet side as well. Refer to ISA-75.01.01-2007 Flow Equations for Sizing Control Valves. For the fan industry, Solution 2: Release to External Environment would be the preferred option. Refer to AMCA 210-07 (2007) Laboratory Methods of Testing Fans for Certified Aerodynamic Performance Rating for additional information.
By: FlowJoe  Tue, 21 Mar 2017 14:28:00 +0000
By: FlowJoe
The Flow Simulation software includes a pressure boundary condition type called "Environmental Pressure," which does not really exist. There are really only two types of pressures that are measurable: Static pressure is measured through a hole in the body, where the velocity is zero hence the static part of the name, with a pressure gauge such as a manometer or Bourdon gauge; and Total pressure, or Stagnation pressure, is measured by a Pitot tube that is placed inline with the flow so it results in a combination of Static + Dynamic pressure. (Subsequently, if the ambient static pressure is additionally measured, you can determine the velocity of the fluid, which is what airplanes do to find its airspeed.) Static pressure is typically used for internal flows and on walls of aerodynamic bodies, and Total pressure for external flows in the free stream. Environmental pressure in the software is meant to try to help solve the problem of foreshortening the computational domain. I don't think that the user is doing this knowingly but figures that since s/he designs this widget that focus will be solely on that widget, without considering how it might need to be physically tested to get reliable results (see previous comment). You would never place a pressure tap in an area where there is a recirculation, you would not obtain consistent measurements. Environmental pressure exactly is a hybrid approach to handling this issue by considering the pressure boundary on a (mesh) cell-by-cell basis by using Static pressure when the fluid is leaving the computational domain and Total pressure when it is entering, or recirculating back into, the domain. So remember this fact when you are specifying your boundary conditions that if flow is entering the domain, say at an "Inlet," that you really did want to specify a Total pressure! An Environmental Pressure condition is typically specified at an outlet, but the outlet should be far enough away from any recirculation that a Static Pressure condition would suffice; so the Environmental pressure condition is a "just in case." Note that pressure in Flow Simulation is always Absolute pressure, as opposed to Gage pressure, and when calculating the Pressure Differential, it should be similar pressure parameters, such as [Total P in] - [Total P out] or [Static P in] - [Static P out].
By: FlowJoe  Wed, 22 Mar 2017 13:45:00 +0000
You are not authorized to view this page No results found! Suggestions: Check spelling, try a different search, or browse topics below.