|
[Sponsors] |
February 11, 2020, 06:27 |
Particle deposition using DPM in fluent
|
#1 |
Member
Shahid Khan
Join Date: Jan 2020
Posts: 35
Rep Power: 6 |
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 |
|
February 11, 2020, 06:36 |
Issues
|
#2 |
Senior Member
|
There are multiple issues with the setup.
1. An anthracite particle, and I am assuming you have not modified the material properties, with 1 diameter has a mass close to 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 , 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 PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority. |
|
February 11, 2020, 07:51 |
|
#3 |
Member
Shahid Khan
Join Date: Jan 2020
Posts: 35
Rep Power: 6 |
Quote:
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 |
|
February 11, 2020, 08:51 |
Suggestions
|
#4 |
Senior Member
|
1. First calculation is correct and not the second one. It was not very clear, however, I am assuming 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 PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority. |
|
February 12, 2020, 03:28 |
|
#5 |
Member
Shahid Khan
Join Date: Jan 2020
Posts: 35
Rep Power: 6 |
Quote:
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 |
|
February 12, 2020, 08:04 |
Transient
|
#6 |
Senior Member
|
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 PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority. |
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
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 |