CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Running, Solving & CFD

DPMFoam - Serious Error --particle-laden flow in simple geometric config

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

Like Tree5Likes

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   January 28, 2016, 05:11
Default
  #21
New Member
 
Muhammad Usman
Join Date: Nov 2015
Location: Germay
Posts: 15
Rep Power: 10
msman is on a distinguished road
I have used the same geometry for other solver and its works.

Files are attached herewith where i have made modifications according to my case
Attached Images
File Type: jpeg Geometry.jpeg (25.5 KB, 71 views)
Attached Files
File Type: zip kinematicCloudProperties.zip (2.8 KB, 14 views)
msman is offline   Reply With Quote

Old   February 2, 2016, 11:17
Default drag model in KimematicCloudProperties
  #22
New Member
 
Muhammad Usman
Join Date: Nov 2015
Location: Germay
Posts: 15
Rep Power: 10
msman is on a distinguished road
Hi again,

can anyone explain the meaning of some terms used in KimematicCloudProperties dictionary

type patchInjection; //Type of injection
parcelBasisType fixed; // ?
patchName upperInlet; // start patch for injection
U0 (18.7939 -6.8404 0); // ?
nParticle 1; // 1 is for steady state condition? right?
parcelsPerSecond 1390885; // number of particles entering per second
sizeDistribution // ?
{
type normal; // ?
normalDistribution
{
expectation 650e-6; // ?
variance 25e-6;
minValue 500e-6;
maxValue 800e-6;
}
}
flowRateProfile constant 1; // ?
massTotal 0; // ?
SOI 0; // start of injection
duration 60; // ?

Kindly rectify my mistake

Your kind help is highly appreciated

Thank you

Last edited by msman; February 2, 2016 at 15:43.
msman is offline   Reply With Quote

Old   February 2, 2016, 14:27
Default
  #23
Member
 
Ananda Kannan
Join Date: Feb 2014
Location: Göteborg, Sweden
Posts: 55
Rep Power: 12
ansubru is on a distinguished road
Hi!!

I will try and answer the terms you have marked with a question mark -

Hi again,

can anyone explain the meaning of some terms used in KinematicCloudProperties dictionary

type patchInjection; //--> Type of injection (you can have either patch injection where you define a surface in the geometry from where particles are injected or other types, have look at injection types.
parcelBasisType fixed; // --> Don't really concern yourself about this, leave it as FIXED
patchName upperInlet; // start patch for injection (the name of the patch where injection is initiated)
U0 (18.7939 -6.8404 0); // Particle velocity at injecton
nParticle 1; // This is a condition for parcels, if you change this to say 100, it means one parcel represensts 100 particles, if this value is 1 then you are treating the system as particle based and not parcel based
parcelsPerSecond 1390885; // number of particles entering per second (correct ))
sizeDistribution // If you want a specific particle size distribution you specify this condition (refer size distribution types in OF guides online)
{
type normal; // Type of distribution can be normal, rossin-ramler etc. (read more in OF guides)
normalDistribution // (read about normal distribution to understand what these terms) mean
{
expectation 650e-6; // ?
variance 25e-6;
minValue 500e-6;
maxValue 800e-6;
}
}
flowRateProfile constant 1; // --> type of flow rate profile again for most laminar flow cases this would be 1, else you will have to change them
massTotal 0; //--> This is used to fix the number of particles that should be injected into the system (or you can use it to control the rate of particles injected per time-step).. play around with it to better understand
SOI 0; // start of injection (correct)
duration 60; // --) Total duration of the injection, in this case the particles are injected until 60 secs of simulation time



I would advice you to thoroughly understand the tutorial case, before proceeding. Everything you need is there, and you should also dig into the source code for the 'lagrangian' function in openfoam (Openfoam x./src/lagrnagian..)

Regards

ansubru
BlnPhoenix and rmn_990 like this.
ansubru is offline   Reply With Quote

Old   February 2, 2016, 14:33
Default
  #24
Member
 
Ananda Kannan
Join Date: Feb 2014
Location: Göteborg, Sweden
Posts: 55
Rep Power: 12
ansubru is on a distinguished road
Hi again!!

Looking at your geometry, I can see some potential regions where you might have numerical inconsistencies. Your geometry is too open-ended. I don't know if this is correct, but you could try and close the pores (they seem to open in the sides).. ensure that the pores have just an opening in the center and the remaining portions are fully sealed (mainly around the circumference)

Regards

ansubru
ansubru is offline   Reply With Quote

Old   February 8, 2016, 11:57
Default what should be particle boundry condition for 2D case
  #25
New Member
 
Muhammad Usman
Join Date: Nov 2015
Location: Germay
Posts: 15
Rep Power: 10
msman is on a distinguished road
Hi again,

thanks ansubru for you kind help. I am about to successfully simulate my first part of the project.

These open pores shown in last figure are completed sealed.

Now I wanna know about the boundry condition for particle located in kinematicCloudproperties dictionary. Usally for velocity and pressure the Bcs for 2D case are like so

walls
{
type empty;
}


but i am not sure what should be the bc for particles and also I couldn't find from langrangian tutorials too. currently I am using

walls
{
type stick;

}

Is it correct or should I also need to use it "empty" for particles?
msman is offline   Reply With Quote

Old   February 8, 2016, 12:03
Default
  #26
Member
 
Ananda Kannan
Join Date: Feb 2014
Location: Göteborg, Sweden
Posts: 55
Rep Power: 12
ansubru is on a distinguished road
Hi again!!

The properties of the Lagrangian phase are specified in the kinematiccloudproperties file. Generally you can specify, stick or rebound or escape depending on your system. Generally particles would rebound from walls, but if you specifically want to capture them ( for some special reasons) then you can use stick. The conditions are specie based on what the system requires.

Regards

ansubru
ansubru is offline   Reply With Quote

Old   July 21, 2016, 11:44
Default PatchInjection
  #27
New Member
 
christos panagopoulos
Join Date: Apr 2016
Posts: 7
Rep Power: 10
panachristos is on a distinguished road
Hallo,

patchInjection injects the parcels randomly over the patch, which is a randomness to my results that i do not want. So, is there any way to modify patchInjection so that it distributes the parcels over the patch under a certain pattern??

If not possible is there any other model to be used instead? manualInjection is not an option for me since i have thousands of particles.

I am looking forward to give me any suggestions on how to solve this.

Regards,
Christos
panachristos is offline   Reply With Quote

Old   December 19, 2017, 20:47
Default
  #28
Member
 
Robert
Join Date: Sep 2016
Posts: 32
Rep Power: 9
dussa is on a distinguished road
Hi,

I see that this thread has not been used in a while, but hopefully someone can help me out.

I am trying to simulate a solid particle and fluid system, where the fluid is more dense than the particles causing them to float. I have just now tried taking the DPMFoam/Goldschmidt case and changing only the fluid and particle density (I also reduced the domain size and number of particles injected to speed up the simulation). I also removed the inlet velocity for further simplicity.

When the simulation is with air the particles fall to the bottom of the geometry as expected and quickly lose most of their kinetic energy forming a layer with very little movement.

When I try this with the case altered by using water (rho = 1000 kg/m3) and reducing the particle density (rho0 = 750) I find that the particles move in a very erratic manner, and do not simply float from their injection location to the top of the fluid domain. They seem to be attracted to the walls, and away from the centre of the fluid domain as you can see in the attached images after 1 second of physical time.

Does anyone know why this could be? I have seen some posts talk about additional forces that need to be included if a dense fluid like water is used, but I am not sure which ones would be required here. If someone coudld point me in the direction of where I can look at what contact models, fluid-particle forces models etc are available that would be much appreciated.

Kind regards,
Robert
Attached Images
File Type: jpg injection.jpg (36.2 KB, 15 views)
File Type: jpg 1second.jpg (42.6 KB, 17 views)
File Type: jpg sideView.jpg (52.6 KB, 30 views)
dussa is offline   Reply With Quote

Reply

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
Inviscid Drag at subsonic, subcritical Mach # Axel Rohde Main CFD Forum 1 November 19, 2001 12:19
SIMPLE method for 2-D flow N.Natiq Main CFD Forum 0 June 2, 2001 08:26
flow over a 2D cyl using SIMPLE T Main CFD Forum 1 January 27, 2001 07:32
fluid flow fundas ram Main CFD Forum 5 June 17, 2000 21:31
momentum under-relaxation for compressible flow with SIMPLE Mihai ARGHIR Main CFD Forum 0 April 7, 2000 04:58


All times are GMT -4. The time now is 20:41.