-
-
January 3, 2024 at 11:51 am
christian.scheffler
SubscriberHi all,
I have an issue regarding the propagation of a free surface jet in ANSYS CFX.
The trajectory length of the jet does not fit to the analytic value of the horizontal throw.
There seems to be a kind of damping or energy loss.
What might be the problem?Settings are:
1st phase = Jet: Water, 2nd phase: Air
Steady State
Advection Scheme: High resolution
Isothermal 25°C
Laminar flow
Morphology: Continuous Fluid
Buoyant: Gravity y-direction: 9.81m/s
Fluid Models: Multiphase Free Surface Model: Standard (i.e. Homogeneous Model not activated)
Fluid Specific Models: Fluid Buoyancy Model: Density Difference
Fluid Pair Models: Interphase Transfer: Free Surface
Fluid Pair Models: Momentum Transfer: Drag Coefficient 0.44
Fluid Pair Models: Surface tension not activated
Solver Control: Advanced Options: Multiphase Control - Volume Fraction Coupling: Segregated
Inflow: Normal velocity 4m/s, 1.0 water, 0.0 AirCould somebody help??
-
January 3, 2024 at 2:01 pm
Rob
Forum ModeratorI assume you've resolved the jet and converged the solution. Where is the drag/viscosity term in the theoretical correlation?
-
January 4, 2024 at 9:32 am
christian.scheffler
SubscriberConvergence more or less, at least the Pressure and Momentum RMS residuals for the water fraction are below 1e-4. Do you consider this as a problem?
I set the drag coefficient to 0.0 and it seems to have a great influence; however, there is still a difference to the analytical solution.
Regarding your question: No, there is no drag force considered in the simple analytical throw trajectory equation.I would like to understand which parameters influence the solution.
Any ideas?I will try to test air with very low density and pressure and see if the orgin of the "loss" problem could be there. -
January 4, 2024 at 10:04 am
Rob
Forum ModeratorI didn't think there was a drag coefficient for the VOF model? Convergence isn't good, but I don't use CFX so am unsure how bad it is. The person I'd usually ask isn't back in yet, but another colleague looks to be in.
We can't model vacuum, but see what dropping the gas density and viscosity does.
-
January 4, 2024 at 10:52 am
Rob
Forum ModeratorOK, having spoken to someone who covers CFX. You're using the drag coefficient to adjust momentum exchange between the two fluids so as the analytical model has no drag the result will be different.
Convergence isn't good either.
-
January 4, 2024 at 2:26 pm
christian.scheffler
SubscriberI tested air pressure/density at 20000m level -> no visible influence.
Convergence is almost below 1e-4 RMS for all momentums. But I am not sure if RMS assessment is correct for such a large area where only a small number of cells contain the water jet.
Any ideas how to improve convergence for the steady state analysis? Timescale settings? Note: The distance of the jet in x is about 1m, that means a travel duration of about 0.25s for one fluid particle.I will test to increase jet size in order to minimize interface losses between the two fractions air/water and increase the cell number trying to improve convergence.
Reducing the drag coefficient from 0.44 to 0.0 seems to had the biggest impact.
Any other ideas are welcome.
-
January 4, 2024 at 4:09 pm
Rob
Forum ModeratorCheck the fluid model too - you're dragging air with the jet, hence the significant difference when you reduce the drag coefficient.
How well refined is the mesh in the jet? Reducing the time scale should help improve convergence too.
-
January 5, 2024 at 9:08 am
christian.scheffler
SubscriberNow the free surface jet and the analytic solution is more or less equal. The model needed the following changes compared to the above settings:
- use openings for left and right wall instead of wall left and outlet/wall right
- setting a physical timescale of 0.05
This improved significantly the convergence.
Neither one of the settings alone did the trick.
The timescale value (time step) is just a guess, I didn’t calculated it based on the Solver Theory Guide. But it is certainly a better option to calc it according to 1.273, 1.274, 1.275 (2023R1). Just to mention it here: the jet velocity is 4m/s, the dimension of the jet in x about 1m, the cell size 1.5mm x 1.5 mm x 1.0 mm. The jet width is resolved by about 10 cells.
-
- The topic ‘Multiphase flow – Free surface jet deviation to analytic solution’ is closed to new replies.
- How do I get my hands on Ansys Rocky DEM
- Non-Intersected faces found for matching interface periodic-walls
- Unburnt Hydrocarbons contour in ANSYS FORTE for sector mesh
- Help: About the expression of turbulent viscosity in Realizable k-e model
- Script Error
- Facing trouble regarding setting up boundary conditions for SOEC Modeling
- convergence issue for transonic flow
- Running ANSYS Fluent on a HPC Cluster
- Point exception in erosion calculation
- Errors with multi-connected bodies using AQWA
-
1987
-
896
-
599
-
591
-
408
© 2025 Copyright ANSYS, Inc. All rights reserved.