I am creating an internal fluid flow simulation.  The model is am testing is a Y pipe junction, with three inlets (2 lines coming in at 45 degrees, one in straight) and one outlet (in line with the straight inlet line).  Like this...... in ->- out

I know the inlet volume flow rates, the inlet pressure, environmental pressures.  This Y pipe model is part of a larger system, so there are no ends open to the environment.

What is the best way of approaching modeling something like this?  Should I use the wizard, or simply add boundary conditions to the ends of the pipes?  I am not sure how  and what is the most efficient way to approach this, in terms of being able to accurately include all of my know flow rates and pressures in the sim.

Ultimately, I am looking to examine mixing (likely with flow trajectories), and also shear forces.

Let me know if you need to know anything else.  Thank you!

Categories: Simulation, Flow Simulation

Last comment By: Joe Galliera   Fri, 16 Feb 2018 22:51:06 GMT

Hi Heather,

While the geometry is a bit different than you describe this video (GoEngineer - Flow Simulation: An Introduction to Fluid Mixing) shows a Flow Project boundary tree with the sorts of pressure and flow definitions you would need to have an analysis complete.  It also goes into some of the plot outputs that visualize fluid mixing.

This video shows more of the actual setup of a fluid mixing problem through the Project wizard (GoEngineer - Flow Simulation: Fluid Mixing Transient Analysis) which may be more helpful with picking particular settings for a fluid mixing analysis.

By: Ryan Dark  Wed, 14 Feb 2018 16:53:59 GMT

There are many ways of starting a Flow Simulation project (including New from a Template, and Clone Project), but the Wizard is most likely the place for you to start.

Select units that you are familiar with using (inches or mm, LPM or GPM, Pa or psi, m/s or ft/s), physics to include (internal, gravity, etc.), fluid type, wall conditions (adiabatic i.e. isothermal, roughness), and ambient conditions (sets the state of the fluid and initial values for all cells).

Then the software should be able to automatically capture the fluid region from your water-tight solid volume. Define your boundary conditions, where one will have to be a pressure condition (most likely the outlet) but depends on what you are trying to accomplish with the study.  Define the other ends appropriately (and based on what you know), which I think is where you question lies.  Just do it like how you would perform a physical bench test, but in a much more controlled virtual environment on the computer.

Based on your description, I would define the outlet as a Pressure condition; internal pipe flow is measured by a pressure tap, so use a static pressure.  (Environmental Pressure condition is equivalent to a Static Pressure when the fluid is leaving the volume at that boundary.) Make sure the outlet boundary is far enough away from the mixing so that the flow has fully redeveloped in the pipe and has regained a linear pressure drop; you may have to extend the pipe further from what the existing model might have.  Again in a physical test, you would do the same to measure the outlet pressure at a location further downstream.

Define your known Volume Flow rates to the 3 inlets, and the software will calculate for you the pressure required to achieve these rates. Define inlets at least 6 diameters upstream of where they will come together and start mixing. A useful hack is that you could make two copies of the fluid that you are using, say Water, Water2 and Water3, and define each inlet as a separate fluid so that you can track the mixing from each inlet.

Create Surface Goals of Static Pressure for the Inlet lids individually (or better select all 3 and choose option to "Create goal for each surface"), and for Shear forces, you can define another Surface Goal of all the internal pipe surfaces collectively.  Shear stress, Force (wall pressure times surface area), and Frictional force might all be interesting to you.

Without knowing your geometry, I suggest to choose an automatic Global Mesh level of say 6 to start with.  If this is too fine or coarse, you could make other changes and maybe set some local mesh controls.

What version of SOLIDWORKS are you using?  I am currently running 2018 Sp1.0.

By: Joe Galliera  Fri, 16 Feb 2018 22:51:06 GMT