|
[Sponsors] |
Particle Simulation without recalculating airflow |
![]() |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
![]() |
![]() |
#1 |
New Member
Join Date: Apr 2019
Posts: 5
Rep Power: 7 ![]() |
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. Thanks. |
|
![]() |
![]() |
![]() |
![]() |
#2 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,870
Rep Power: 144 ![]() ![]() ![]() ![]() |
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.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
![]() |
![]() |
![]() |
![]() |
#3 |
New Member
Join Date: Apr 2019
Posts: 5
Rep Power: 7 ![]() |
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. |
|
![]() |
![]() |
![]() |
![]() |
#4 |
New Member
Join Date: Apr 2019
Posts: 5
Rep Power: 7 ![]() |
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. |
|
![]() |
![]() |
![]() |
Tags |
particle, solver |
|
|
![]() |
||||
Thread | Thread Starter | Forum | Replies | Last Post |
Particle size and Mesh Size; Particle tracking; | Suman Sapkota | CFX | 11 | August 12, 2018 20:39 |
Water Droplets Entrained within Airflow / Nasal Spray Simulation - Basic Beginner | AllyB2106 | FLUENT | 0 | March 27, 2018 21:31 |
particles leave domain | Steffen595 | CFX | 9 | March 7, 2016 17:19 |
Pressure gradient in particle simulation | Mikka | Main CFD Forum | 0 | August 5, 2007 22:55 |
Pressure gradient in particle simulation | Mikka | Main CFD Forum | 0 | June 30, 2007 23:16 |