CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Fluent Multiphase

DDPM (dem) model specifying collisions with boundaries

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

Like Tree1Likes
  • 1 Post By grasingerm

Reply
 
LinkBack Thread Tools Display Modes
Old   May 22, 2014, 11:37
Default DDPM (dem) model specifying collisions with boundaries
  #1
New Member
 
PA
Join Date: May 2014
Posts: 6
Rep Power: 3
grasingerm is on a distinguished road
I am trying to start with a simple discrete element model in fluent. I ran an unsteady model with unsteady particle tracking and the DEM collision model active. I used the adaptive collision mesh. I used the default collision parameters for the collision pairs (spring constant = 1000, coeff of resititution = 0.9), and specified the wall boundary conditions as "reflect" for the DPM phase. After injecting a single particle I can track it, step by step, until it collides with a wall. At this step Fluent hangs and eventually crashes. I wish I could provide some error messages to the thread, but none are given from the solver.

Any advice on setup and/or parameters that may need changed in order for the solver to not crash when a collision takes place?
grasingerm is offline   Reply With Quote

Old   June 2, 2014, 11:47
Default Convergence issues
  #2
New Member
 
PA
Join Date: May 2014
Posts: 6
Rep Power: 3
grasingerm is on a distinguished road
So the reason Fluent was hanging / crashing before was because the solution for particle motion was not converging for a time step in which a collision occurred. Some ways in which I was finally able to achieve convergence:

* reduced the time step by an order of magnitude. Instead of working in hundredths of a second I tracked the particles in thousands of a second. Fluent allows you to track particles at a different time step than the fluid motion time step. I took advantage of this.
* soften collisions
- reduced spring constant by an order of magnitude. the default is to use a spring constant of 1000. By reducing it to 100 a solution for particle motion when a collision occurred converged much quicker.
- reduced coefficient of restitution from 0.9 to 0.5
grasingerm is offline   Reply With Quote

Old   June 18, 2014, 18:17
Default
  #3
Member
 
Amir
Join Date: Sep 2012
Posts: 44
Rep Power: 4
Amir1 is on a distinguished road
Hi there,

Would you mind elaborating a little bit more on:

1. Where can I change the coefficent of restututio?
2. How can I make sure which restitution number and spring or dash coefficents work better?

Thanks a lot,
AK
Amir1 is offline   Reply With Quote

Old   June 19, 2014, 10:09
Default
  #4
New Member
 
PA
Join Date: May 2014
Posts: 6
Rep Power: 3
grasingerm is on a distinguished road
1) In the models section make sure the Eulerian-Eulerian model is active and the Dense Discrete Phase Model box is checked.

2) double click "Discrete Phase - On" in the models section. Uncheck "Accuracy Control" under the Numerics tab. Check "DEM Collision" under the physical models tab.

3) create an injection. make sure you define a phase domain and collision partner when you set the injection properties.

4) click "DEM Collisions..." in the Discrete Phase Model dialog box

5) you can set the properties of any of the collision pairs. The coefficient of restitution is actually labeled "spring-dashpot: eta" under the spring-dashpot contact law. The default is 0.9 but it will help convergence if it is lower. Same goes with the spring constant. The default is 1000, but if you are having convergence issues either lower your tracking timestep or try lowering the spring constant.

6) make sure you set a collision partner at the walls. you can do this by editing your wall boundary conditions for the "mixture" phase and editing the properties under the DPM tab. note that the "DEM Collision Partner" names are arbitrary. Those names only reference collision properties that you have set, not necessarily what specific material or particles are going to collide. For instance, if you set the wall's collision partner as "dem-anthracite", when a discrete particle with the collision partner "dem-aluminum" collides with the wall, the contact laws it will use are set under the dem-anthracite dem-aluminum contact pair settings.

As far as finding which contact laws work best (spring constant, coefficient of restitution, friction, etc.) you're going to have to try different things and see, I imagine every model will be different. Obviously you want contact laws that match the physics of the problem you are trying to solve, but if you are having trouble getting a solution to converge, you can try making your particle tracking time step lower, reducing the spring constant, or reducing the coefficient of restitution.
grasingerm is offline   Reply With Quote

Old   June 20, 2014, 14:08
Default
  #5
Member
 
Amir
Join Date: Sep 2012
Posts: 44
Rep Power: 4
Amir1 is on a distinguished road
Thanks a lot for your message. I will check it and will let you know.

Have a great weekend
Amir1 is offline   Reply With Quote

Old   July 18, 2014, 15:15
Default
  #6
Member
 
MarkClarence
Join Date: Jul 2014
Posts: 32
Rep Power: 3
Clarence91 is on a distinguished road
Hi,
I am using the Lagrangian model...and DPM with DEM. I have never worked with DEM before.
When i try to run the case it gives me an error popup "OUT OF MEMORY" and in the fluent dialog box I see:

DEM: Memory allocation for collision mesh failed.
Collision mesh width is very small which will give rise to a
huge collision mesh. Consider inspecting your injection setup.
Maybe the number in parcel is not what you want.
Error: Out of memory


Can you help me with this?
Clarence91 is offline   Reply With Quote

Old   July 19, 2014, 14:34
Default Adaptive collision mesh
  #7
New Member
 
PA
Join Date: May 2014
Posts: 6
Rep Power: 3
grasingerm is on a distinguished road
Under...

Discrete Phase Dialog Box -> Physical Models Tab

You have "adaptive collision mesh" checked. I had similar issues with it running out of memory for some models so I have unchecked that box in the past and picked a constant value for the collision mesh size. It is important that if you do this, you choose a collision mesh size that you know is fine enough that your model will not miss any collisions.

In the Fluent documentation: "By default, Adaptive Collision Mesh Width is enabled. This adjusts the width of the collision mesh to the largest parcel diameter multiplied by the Edge Scale Factor."

So another way to increase your collision mesh size (and therefor save memory), would be to increase the edge scale factor, or increase your parcel size. There is a parcel tab under the injection dialog box. I don't know if you can specify a size, but you can specify a fixed mass or number of particles for each parcel. If you decide to specify either of those yourself, I'm sure increasing the particles per parcel, or mass per parcel, will increase the parcel size and increase the collision mesh width.
grasingerm is offline   Reply With Quote

Old   July 19, 2014, 14:49
Default
  #8
Member
 
MarkClarence
Join Date: Jul 2014
Posts: 32
Rep Power: 3
Clarence91 is on a distinguished road
Thanks of the reply. I will work on this and let you know.

By the way, can I find any DEM tutorials anywhere?
Clarence91 is offline   Reply With Quote

Old   July 21, 2014, 11:03
Default
  #9
Member
 
Amir
Join Date: Sep 2012
Posts: 44
Rep Power: 4
Amir1 is on a distinguished road
Hi Clarence,

I have some nice papers on DEM. I can share with you if you are interested.
Also take a look at Fluent Theory Guide. It's concise and helpful.

Regards,
Amir
Amir1 is offline   Reply With Quote

Old   July 21, 2014, 11:24
Default
  #10
New Member
 
PA
Join Date: May 2014
Posts: 6
Rep Power: 3
grasingerm is on a distinguished road
Clarence,

I found this to be a decent tutorial to start with. Of course, you need an ANSYS Customer Portal account to access it.
Clarence91 likes this.
grasingerm is offline   Reply With Quote

Old   July 21, 2014, 11:38
Default
  #11
Member
 
MarkClarence
Join Date: Jul 2014
Posts: 32
Rep Power: 3
Clarence91 is on a distinguished road
Amir,

Can you share papers with me? (markclarence1991@gmail.com)

I saw the FLUENT theory guide it explains about the terms in the DEM menu but not how to use them in different cases.
Clarence91 is offline   Reply With Quote

Old   July 21, 2014, 13:29
Default
  #12
Member
 
Amir
Join Date: Sep 2012
Posts: 44
Rep Power: 4
Amir1 is on a distinguished road
Just sent you some useful papers. As I mentioned these articles gives you whats behind these numbers and what models you should select with which valuse.

Best, Amir
Amir1 is offline   Reply With Quote

Old   July 23, 2014, 12:54
Default
  #13
Member
 
MarkClarence
Join Date: Jul 2014
Posts: 32
Rep Power: 3
Clarence91 is on a distinguished road
Hello grasingerm,
I tried to follow the steps you mentioned above but I have a problem still. Mine is a 2D problem and I am not able to DEFINE-->PHASES in fluent...so simultaneously for the injections I cant define any PHASE DOMAIN.
And I dont know why Iam getting this when I start calculations :
Advancing DPM injections ....
Injecting 80 particle parcels with mass 3.2e-23 at t = 0

Deleted 20 particles in injection pp1mm with total mass 8.000000e-24 kg

Deleted 20 particles in injection pp0.15mm with total mass 1.600000e-23 kg

Deleted 20 particles in injection np1mm with total mass 2.400000e-23 kg

Deleted 20 particles in injection np0.15mm with total mass 3.200000e-23 kg


Do you have any idea about this?

((I have four different injections in my case.))
Clarence91 is offline   Reply With Quote

Old   August 8, 2014, 19:13
Default
  #14
Member
 
MarkClarence
Join Date: Jul 2014
Posts: 32
Rep Power: 3
Clarence91 is on a distinguished road
I could fix this error.
FLUENT allows only minimum parcel mass limit below which Fluent terminates those parcels and kill them. I decresed the total flow rate, then it worked.

By the way is there a way to know the parcel diameter ? If so how can we calculate it?
Clarence91 is offline   Reply With Quote

Old   August 27, 2014, 15:03
Default
  #15
Member
 
Amir
Join Date: Sep 2012
Posts: 44
Rep Power: 4
Amir1 is on a distinguished road
I think parcel diameter (radius) can be found by multiplying the number:

The radius of the DEM parcel is that of a sphere whose volume is the mass of the entire parcel divided by the particle density.
Amir1 is offline   Reply With Quote

Old   August 27, 2014, 17:40
Default
  #16
Member
 
MarkClarence
Join Date: Jul 2014
Posts: 32
Rep Power: 3
Clarence91 is on a distinguished road
Yeah I could get this information from UserGuide of Fluent.

Weird thing in my problem is: I see number of particles to be something like 300-400 in each parcel, which will define that parcel diameter is less than particle diameter right? but thats not the case in my problem.

Particle diameter is 1e-3(which I set) and finally parcel diameter is 1.56e-6, which is impossible if no.of particles in each parcel is >1 ((((even though if each parcel consists of 1 particle then both the diameters should be equal))))

I don't understand whats going on with my problem!!!
Clarence91 is offline   Reply With Quote

Old   July 3, 2015, 16:01
Default Dem
  #17
New Member
 
Marcos
Join Date: Nov 2013
Posts: 9
Rep Power: 3
marcoscp2 is on a distinguished road
Little late, I know...

I would suggest using only one particle per parcel when using DEM. It solves a lot of problems.

Just out of curiosity: how is DEM working with Eulerian-Eulerian model? Is it good? Why don't you use KTGF?
marcoscp2 is offline   Reply With Quote

Reply

Tags
dem, dpm, fluent 14.5

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Is it possible to model natural convection in a 2D horizontal model in fluent caitoc FLUENT 1 May 5, 2014 13:32
Error finding variable "THERMX" sunilpatil CFX 8 April 26, 2013 07:00
Eulerian model with DDPM Lucaaa FLUENT 2 February 20, 2013 09:56
2 stage axial turbine model convergence issues sherifkadry CFX 2 September 7, 2009 20:51
Kato-Launder model sam Main CFD Forum 13 September 21, 2006 10:15


All times are GMT -4. The time now is 17:19.