[grasingerm]

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]

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

[Amir1]

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

[grasingerm]

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.

[Amir1]

Thanks a lot for your message. I will check it and will let you know.

Have a great weekend

[Clarence91]

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?

[grasingerm]

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.

[Clarence91]

Thanks of the reply. I will work on this and let you know.

By the way, can I find any DEM tutorials anywhere?

[Amir1]

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

[Clarence91]

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.

[Amir1]

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

[mroue]

Dear Amir,

Could you also please share the papers with me at mroue@hotmail.co.uk. Thank you

[Amir1]

Hi, Just sent you some papers you asked.

Good Luck, Amir

[Amna]

hello Amir

could you please send DEM helping material on this id : amnaamanat73@gmail.com

Actually i m simulating a fluidized bed using DDPM model with DEM collisions & i dont know how to set the normal or tangential collision parameters in DEM tab.

it'll be really nice of you if you let me know this .

thankx

[roopesh99]

Originally Posted by Amir1

Hi, Just sent you some papers you asked.

Good Luck, Amir

Hi Amir,
I am using ANSYS Fluent DDPM-DEM. Can you share the idea/papers about setting the value spring constant and damping etc.

[Amir1]

Hi,

Just sent you some files.

GL, Amir

[Dawood Al-Mosuli]

Hello All,
I am a beginner to use ANSYS Fluent DDPM-DEM to simulate transient flow in a downer fluidized bed column. I faced three main problems:
1- Because the DEM time step (s) 5×10−6 which i believe that it is the same as the particle step size is recommended to be very small then the solution is so time consuming. It takes one day for each 0.25 sec with a very good computer.
Does anybody have an idea to increase solution speed?

2- I suppose to have a continuous particle injection through the upper surface, but whatever I changed with the parcel release method, I got separate injections of particles. What to do to have a continuous solid flow?

3- Is it normal with transient flow to have highly oscillating residuals even if the simulation results were physically accepted?

Thank you

Dawood

[Liguoguo]

hello Amir

could you please send DEM helping material on my email address : wangtong218@gmail.com?

Now I'm working on the particle fouling in metal foam using DDPM + DEM.
it'll be really nice of you if you let me know this .

thanks

[medo-elbob]

hello every one
I'm trying to model multi-phase flow (water - oil) in corrugated plat separator using multi-phase eulerian model and dence Discrete Phase model + stochastic collision +coalescence model. I got problem modeling oil droplet behavior.
My set up:
1) multi-phase eulerian model active dense Discrete Phase model (all others setting are default here)
2) Transition k-kl-epsilon model
3) Discrete phase model: unsteady particles tracking, interaction with continuous phase, implicit tracking, no accuracy control (all others setting are default here)
4) check in physical model stochastic collision +coalescence model all others setting are default here)
5) There is one cell zone: operating pressure=101325pa, gravity on, operating density=1100kg/m3
6) Boundaries: one velocity inlet, 1 pressure outlets, all others are walls
7) All solution controls are default, time step size 1 s
i have message reversed flow pressure outlet
So my question to you how to set up oil- water gravity separation problem properly, what models should i use?
pleas help me

[sewgolam]

Hallo,
I'm doing my thesis currently an working on solar reactor.

I have a simple geometry of rectangular and i simulate am single phase flow and mixture flow in a laminar flow.

Now i want to inject particle in my flow but do not have idea how to do it.

I want to lagrangian-Eulerian model to track particle in my fluid.
Can anyone help my and coud you give me step wise how to do it because im totally new in fluent.

thank you