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

Particle deposition using DPM in fluent

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   February 11, 2020, 06:27
Default Particle deposition using DPM in fluent
  #1
New Member
 
Shahid Khan
Join Date: Jan 2020
Posts: 10
Rep Power: 2
shahidkhan is on a distinguished road
Hello everyone.
I am trying to simulate velocity distribution and particle deposition using DPM model in fluent.
Particle size- 1micron
Particle density- 2000kg/m3
number of particles to be injected- 10000.
I am using injection type as surface and choosing inlet surface for injection.
For outlet- 'escape' boundary condition
For wall- 'trap'.


First question- How can I give number of particles to be injected? I am not able to get it.
Second question- In boundary conditions, for inlet it is automatically taking as escape which is wrong I guess?
Third question- After simulation how to see where particles are deposited in post-processing?

P.S- I am attaching screenshots for reference.
Screenshot (149).jpg

Screenshot (150).jpg

Screenshot (151).jpg
shahidkhan is offline   Reply With Quote

Old   February 11, 2020, 06:36
Default Issues
  #2
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 539
Rep Power: 16
vinerm is on a distinguished road
There are multiple issues with the setup.

1. An anthracite particle, and I am assuming you have not modified the material properties, with 1 \mu m diameter has a mass close to 10^{-16} kg. The mass flow rate you have supplied is 4 order less. Increase it to at least equal to 1 particle. You may want more.

2. You can modify escape to some other condition; whatever you like

3. You have various options to see particles; you may look at concentration of particles or their tracks.

With a particle size of 1 \mu m, you may not expect much disturbance to the flow, therefore, you can run one-way coupled simulation; it will save time. However, calculate Stokes number and check if it is really below 1. If it is not, then keep it two-way coupled; the way you have it now.

Number of particles are decided by the faces on the surface that you use for the injection. If you use some other method of injection, then you have better control, but number of particles are not really that important. These are only representative particles. Real number of particles is decided by its diameter, density, and mass flow rate given in Injection panel, which is 1e-20 right now.
__________________
Regards,
Vinerm

PMs only for private content
vinerm is offline   Reply With Quote

Old   February 11, 2020, 07:51
Default
  #3
New Member
 
Shahid Khan
Join Date: Jan 2020
Posts: 10
Rep Power: 2
shahidkhan is on a distinguished road
Quote:
Originally Posted by vinerm View Post
There are multiple issues with the setup.

1. An anthracite particle, and I am assuming you have not modified the material properties, with 1 \mu m diameter has a mass close to 10^{-16} kg. The mass flow rate you have supplied is 4 order less. Increase it to at least equal to 1 particle. You may want more.

2. You can modify escape to some other condition; whatever you like

3. You have various options to see particles; you may look at concentration of particles or their tracks.

With a particle size of 1 \mu m, you may not expect much disturbance to the flow, therefore, you can run one-way coupled simulation; it will save time. However, calculate Stokes number and check if it is really below 1. If it is not, then keep it two-way coupled; the way you have it now.

Number of particles are decided by the faces on the surface that you use for the injection. If you use some other method of injection, then you have better control, but number of particles are not really that important. These are only representative particles. Real number of particles is decided by its diameter, density, and mass flow rate given in Injection panel, which is 1e-20 right now.

1. Based on what you said I am giving flow rate. I have changed the density in boundary conditions. Attaching a calculation
photo please look into it.

2. Which condition should I give as that is my inlet for particles as well as flow? Attaching screenshot for reference.

3. Is there any tutorial through which I can understand how to run a one-way coupled lagrangian simulation?

4. Which injection type will be suitable for that? Attaching a screenshot for reference.

I am attaching the screenshot of how I want my particle deposition to look like at the end.

IMG_20200211_170234.jpg

Screenshot (153).jpg

Screenshot (154).jpg

Screenshot (155).png
shahidkhan is offline   Reply With Quote

Old   February 11, 2020, 08:51
Default Suggestions
  #4
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 539
Rep Power: 16
vinerm is on a distinguished road
1. First calculation is correct and not the second one. It was not very clear, however, I am assuming \pi has been taken into account.

2. For inlet, you should use what you know; it could be velocity or mass flow rate or pressure. For DPM at inlet, it should either be reflect or escape. That depends upon whether particles can exit from inlet side due to some forces or not.

3. For one-way coupled, you just run the simulation with DPM Interaction Disabled in the DPM Model Window. Once the simulation converges, you can postprocess the results. Refer any Fluent DPM tutorial

4. Type of injection depends upon information availability. I'd suggest you use surface injection from the inlet, provided particles enter from the inlet in the real system.
__________________
Regards,
Vinerm

PMs only for private content
vinerm is offline   Reply With Quote

Old   February 12, 2020, 03:28
Default
  #5
New Member
 
Shahid Khan
Join Date: Jan 2020
Posts: 10
Rep Power: 2
shahidkhan is on a distinguished road
Quote:
Originally Posted by vinerm View Post
1. First calculation is correct and not the second one. It was not very clear, however, I am assuming \pi has been taken into account.

2. For inlet, you should use what you know; it could be velocity or mass flow rate or pressure. For DPM at inlet, it should either be reflect or escape. That depends upon whether particles can exit from inlet side due to some forces or not.

3. For one-way coupled, you just run the simulation with DPM Interaction Disabled in the DPM Model Window. Once the simulation converges, you can postprocess the results. Refer any Fluent DPM tutorial

4. Type of injection depends upon information availability. I'd suggest you use surface injection from the inlet, provided particles enter from the inlet in the real system.

I did what you said and ran the simulation.
I gave the trap condition on the walls and escape for the outlet. Now I need to see where particles are deposited on the walls. I am not able to find any tutorial for that.

This is how I want to see- (attaching image for reference)Screenshot (155).png
shahidkhan is offline   Reply With Quote

Old   February 12, 2020, 08:04
Default Transient
  #6
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 539
Rep Power: 16
vinerm is on a distinguished road
For such an outcome, you have to use transient tracking. Trap boundary condition means the particles are mixed with the continuous fluid as soon as they touch the boundary. You don't want that. Set reflect boundary condition with rather small restitution coefficient. Run Unsteady Particle Tracking from DPM panel.
__________________
Regards,
Vinerm

PMs only for private content
vinerm 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
Particle tracking error alchem OpenFOAM Bugs 5 May 6, 2017 17:30
Particle mass in DPM in Fluent Abhiroop Fluent Multiphase 0 August 1, 2016 05:08
Hooking a DPM Particle Heat and Mass Transfer UDF to FLUENT subhankar_bhandari Fluent UDF and Scheme Programming 0 August 19, 2010 04:09
Hooking a DPM Particle Heat and Mass Transfer UDF to FLUENT subhankar_bhandari FLUENT 0 August 19, 2010 04:01
DPM particle size distribution in Fluent Pete FLUENT 5 July 7, 2008 13:22


All times are GMT -4. The time now is 09:11.