CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > CFX

Particle Simulation without recalculating airflow

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   August 7, 2019, 08:48
Default Particle Simulation without recalculating airflow
  #1
New Member
 
Join Date: Apr 2019
Posts: 5
Rep Power: 3
tischroe is on a distinguished road
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.
tischroe is offline   Reply With Quote

Old   August 7, 2019, 19:30
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,467
Rep Power: 128
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
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.
ghorrocks is offline   Reply With Quote

Old   August 12, 2019, 02:24
Default
  #3
New Member
 
Join Date: Apr 2019
Posts: 5
Rep Power: 3
tischroe is on a distinguished road
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 is offline   Reply With Quote

Old   August 30, 2019, 04:59
Smile Problem solved: Calculating Particles without recalculating Fluid
  #4
New Member
 
Join Date: Apr 2019
Posts: 5
Rep Power: 3
tischroe is on a distinguished road
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.
tischroe is offline   Reply With Quote

Reply

Tags
particle, solver

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
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


All times are GMT -4. The time now is 21:32.