CFD Online Discussion Forums

CFD Online Discussion Forums (
-   CFX (
-   -   Particle Simulation without recalculating airflow (

tischroe August 7, 2019 08:48

Particle Simulation without recalculating airflow
Good afternoon,

I'm working at a project where i'm calculating the erosion at a plate which is hit by particles. I use ANSYS CFX. The calculation is a steady state simulation with oneway-coupling between fluid and particles.

To study the parameters for the particles without investigating to much time i would like to calculate the fluid first and vary the parameters without modifying the solution of the fluid flow anymore.

Is there a opportunity in CFX to seperate the particle calculation completely (-> Start only the particle calculation based on the result of the fluid flow)? Or is the easiest way to calculate the fluid flow again with the previous result as an initialization but only over 1 iteration step, so that the solver calculates the particle data.


ghorrocks August 7, 2019 19:30

Have you looked at the tutorial example "Flow in a butterfly valve"? This appears to be exactly the sort of case you are looking at. That should be a good guide for how to set up this sort of model.

tischroe August 12, 2019 02:24

Tanks. I built up the setup like the tutorial.
Now I have to calibrate some parameters of my model to get the same results as my colleague in his experimental research.

For a fast calibration I would like to do parameter studies with the particles. The particles with one-way-coupling are calculated as a seperated step after the CFD-Calculation. I have calculated the flow already. So I wanted to know how I can start the particle calculation without wasting time with simulating the fluid flow after changing the particle parameters again and again.

Thank you for your replies.

tischroe August 30, 2019 04:59

Problem solved: Calculating Particles without recalculating Fluid
Maybe a short update how I solved the problem and saved a lot of time could help anyone:

In CFX-Pre the opportunity to insert Expert Parameters is given. In the menu for Expert Parameters is the point "Model Overrides". Here the points "solve energy", "solve fluids", "solve temperature variance" and "solve turbulence" were set to false.
At Solver Controls I chose only 2 Iterationsteps.
At the Solver Manager I added the calculated fluidflow as an initial solution.

Instead of calculating the fluid and the particles for 2,5 hours the program solved just the particle equations in about 10 minutes. I'm actually searching for suitable parameters of erosion models, so i have to do multiple particle simulations and it saved a lot of time.

All times are GMT -4. The time now is 01:36.