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

Gas Cyclone convergence problem

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

Like Tree1Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   July 17, 2012, 01:34
Default Gas Cyclone convergence problem
  #1
Member
 
Join Date: Jul 2012
Posts: 39
Rep Power: 4
lxlylzl is on a distinguished road
Hi everybody

This is my 1st post in this forum and hope for your co-operation.

I'm working on reverse flow gas cyclone with DPM. I'm working with RSM: Non-equilibrium wall function. I've 1,65,525 hex cells (testing phase). I'm using SIMPLEC scheme for pressure-velocity coupling, Least Square Cell Based for Gradient, PRESTO for pressure, 2nd order Upwind for Turbulent ke and for Dissipation rate, and 1st order for Transient formulation. I've inlet velocity 10 m/s and DPM too has the same inlet velocity. My inlet is velocity inlet, outlet (top) is outflow, and rest other walls. All residuals are set to 1e-05.

Now I'm facing two problems.
  1. The solution in non-converging (I ran it for 3.1 sec. too!), whereas some of them claim to get convergence at 1.6 sec.
  2. The time average tangential velocity (max. value around 11 m/s) is not matching with the experimental one (max. value around 18m/s). However, the time average axial-velocity is somewhat near to the experimental values.
Without DPM I'm getting nearly the same results of Tangential velocity (i.e., max. tangential velocity around 11 m/s), but with convergence. Am I doing wrong somewhere? Please suggest me to get results with convergence.

Regards
Attached Images
File Type: jpg fluent-1-00670.jpg (83.8 KB, 67 views)

Last edited by lxlylzl; July 17, 2012 at 02:49.
lxlylzl is offline   Reply With Quote

Old   July 17, 2012, 03:55
Default
  #2
New Member
 
Elias Paez
Join Date: Nov 2011
Location: Madrid
Posts: 25
Rep Power: 5
sicfred is on a distinguished road
did you try to increase the number of iterations per time step? and also decrease the time step size?
sicfred is offline   Reply With Quote

Old   July 17, 2012, 04:04
Default
  #3
Member
 
Join Date: Jul 2012
Posts: 39
Rep Power: 4
lxlylzl is on a distinguished road
Thank you sicfred for your reply. I've increased and decreased the time step, but the results are the same as before. Well, throughout I've taken max. Iterations/time step as the default value,i.e., 20. I'll check it by substituting its value to be 50. Will it have any impact on the results ??? Thanks again.
lxlylzl is offline   Reply With Quote

Old   July 17, 2012, 04:17
Default
  #4
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,006
Rep Power: 15
RodriguezFatz will become famous soon enough
1) Do you consecutively inject particles at your inlet?
2) Do you have "Interaction with Continuous Phase" switched on?
RodriguezFatz is offline   Reply With Quote

Old   July 17, 2012, 04:43
Default
  #5
Member
 
Join Date: Jul 2012
Posts: 39
Rep Power: 4
lxlylzl is on a distinguished road
Thanx RodriguezFatz 4 ur reply.
Yes I've checked "Interaction with Continuous Phase", and I've been injecting around 750 particles normal to the surface (from inlet) per second !
lxlylzl is offline   Reply With Quote

Old   July 17, 2012, 04:49
Default
  #6
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,006
Rep Power: 15
RodriguezFatz will become famous soon enough
Quote:
Originally Posted by lxlylzl View Post
Thanx RodriguezFatz 4 ur reply.
Yes I've checked "Interaction with Continuous Phase", and I've been injecting around 750 particles normal to the surface (here inlet) per second !
Ok, then try "Update DPM Sources Every Flow Iteration", thats the checkbox below. You can also set "Number of Continuous Phase Iterations per DPM Iteration" to 1. And, also in the "Discrete Phase Model Dialog box" under "Numerics" set the numeric scheme to "implicit". Particle algorithms can become ugly, when you violate CFL criterion, so with implicit you are on the safe side!
RodriguezFatz is offline   Reply With Quote

Old   July 17, 2012, 05:00
Default
  #7
Member
 
Join Date: Jul 2012
Posts: 39
Rep Power: 4
lxlylzl is on a distinguished road
Thanx RodriguezFatz. I am already using "Update DPM Sources Every Flow Iteration" with its default value (i.e. 20). For tracking parameters I'm using 9e+05 as max. no. of steps. Under numerics, I've been using implicit for high order schemes (which is by default in fluent). Under particle treatment box, I've checked "Unsteady particle tracking" and also "Track with fluid flow time step". This means particle time step size is 0.001 (Fluent's default). Thanx.
lxlylzl is offline   Reply With Quote

Old   July 17, 2012, 05:22
Default
  #8
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,006
Rep Power: 15
RodriguezFatz will become famous soon enough
Quote:
Originally Posted by lxlylzl View Post
I am already using "Update DPM Sources Every Flow Iteration" with its default value (i.e. 20).
Try "1".


Quote:
Originally Posted by lxlylzl View Post
Under numerics, I've been using implicit for high order schemes (which is by default in fluent).
Are you sure? In my case "trapezoidal" was set as default.


The rest sounds fine.
Did you calculate your particle mass flow correctly?
RodriguezFatz is offline   Reply With Quote

Old   July 17, 2012, 05:40
Default
  #9
Member
 
Join Date: Jul 2012
Posts: 39
Rep Power: 4
lxlylzl is on a distinguished road
Hi RodriguezFatz. My mass flow rate for particles is 0.001 Kg/s. I'll try "Number of Continuous Phase Iterations per DPM Iteration" equal to 1.
Yes, for numerics, my default is : "High order scheme : trapezoidal", and "Lower order scheme : implicit". O.K.!! I'm saying this when "Automated" option is checked under "Tracking Scheme Selection"!!! Do I have to uncheck it? If so, I'm getting various options under Tracking scheme like: implicit, analytic, trapezoidal, or Runge-kutta (default is trapezoidal). So shall I proceed by unchecking "Automated" box and with implicit as tracking scheme? Is this the option (by unchecking) you were talking about? Do I need to uncheck "Accuracy Control" under "Numerics" tab too? In my case it is checked ! Thanx.
lxlylzl is offline   Reply With Quote

Old   July 17, 2012, 05:50
Default
  #10
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,006
Rep Power: 15
RodriguezFatz will become famous soon enough
1) What's the density of your particle material? How large is the inlet area?
2) Try to uncheck "Automated". Then choose just "implicit". You have to get rid of your numerical problems first, then you can enhance accuracy. On that score, "implicit" is the best choice, since it is unconditionally stable.
RodriguezFatz is offline   Reply With Quote

Old   July 17, 2012, 05:57
Default
  #11
Member
 
Join Date: Jul 2012
Posts: 39
Rep Power: 4
lxlylzl is on a distinguished road
Hi RodriguezFatz. Particle density is 860 Kg/m^3, and Inlet area is (0.145 x 0.058) m^2. After passing through inlet, air along with DPM experiences swirl motion to separate out the discrete phase out of the continuous phase (i.e. air) due to centrifugal action. Thanx
lakhi likes this.
lxlylzl is offline   Reply With Quote

Old   July 17, 2012, 06:05
Default
  #12
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,006
Rep Power: 15
RodriguezFatz will become famous soon enough
If my quick calculation was correctly, your input should be fine. I have a volume fraction of 1.38e-5 for your case, which is by far low enough!
Try a run with the new settings, it should work now...
I will keep my fingers crossed.
RodriguezFatz is offline   Reply With Quote

Old   July 17, 2012, 06:39
Default
  #13
Member
 
Join Date: Jul 2012
Posts: 39
Rep Power: 4
lxlylzl is on a distinguished road
Thank you RodriguezFatz, I'll try with the new settings tonight and let you know the results.
lxlylzl is offline   Reply With Quote

Old   July 17, 2012, 10:39
Default
  #14
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,006
Rep Power: 15
RodriguezFatz will become famous soon enough
One other thing: Reduce the order of your continuous phase numerics towards more dissipative schemes ("as much 1st order upwind as possible"). That did the trick for me right now!
RodriguezFatz is offline   Reply With Quote

Old   July 17, 2012, 15:04
Default
  #15
Member
 
Join Date: Jul 2012
Posts: 39
Rep Power: 4
lxlylzl is on a distinguished road
Hi RodriguezFatz, nice to hear you again. I think you mean that I shall reduce the spatial discretization parameters to 1st order upwind, right! As soon as I finish the previous problem (which is still in progress), I'll try that too. I hope it converges on 2nd order upwind scheme as per our discussion. Many thanx for ur support.
lxlylzl is offline   Reply With Quote

Old   July 18, 2012, 00:56
Default
  #16
Member
 
Join Date: Jul 2012
Posts: 39
Rep Power: 4
lxlylzl is on a distinguished road
Hi RodriguezFatz, I couldn't achieve convergence with 2nd order upwind with DPM (image attached).
With single phase, i somehow got convergence (image attached).

To reduce simulation time, I'm working with 60,000 hex cells.

In a thesis I've read that with DPM, convergence was achieved within 1.6 to 1.7 seconds, and for me, even on single phase it took nearly 2.9 seconds to converge. Do I have to rework on single phase first to achieve convergence within 2 seconds ? I'm also not getting desired tangential velocity (1.7 to 2.5 times inlet velocity) of 18 m/s (mine is 11m/s). I still can't figure out where exactly is the problem. !!!!!!!!!!!!
Attached Images
File Type: jpg DPM.jpg (96.4 KB, 35 views)
File Type: jpg single phase.jpg (83.4 KB, 35 views)
lxlylzl is offline   Reply With Quote

Old   July 18, 2012, 03:48
Default
  #17
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,006
Rep Power: 15
RodriguezFatz will become famous soon enough
During each timestep, do the residuals stop getting better after some iteration and remain at, let's say 1.0e-2 ?
How large is you maximum number of iterations per timestep?
RodriguezFatz is offline   Reply With Quote

Old   July 18, 2012, 04:48
Default
  #18
Member
 
Join Date: Jul 2012
Posts: 39
Rep Power: 4
lxlylzl is on a distinguished road
Hi RodriguezFatz
After few time steps, the continuity line in the residuals is mainly fluctuating. In the beginning, all the lines slopes down in a group and after, say, nearly 2000 iterations, continuity line starts separating out and its fluctuation is more (its like, rushing up to 1e-01 residual in a very unusual manner) than any other parameter with the increasing number of time steps. Continuity line slopes up drastically at few time steps, while other parameters are comparatively fluctuating at very slow rate. At few time steps there is sudden jump in all parameters ( with sudden fall down too !), as can be seen in the figure.

Well, my Max Iterations/Time Step is 40. Since I'm working on a very coarse mesh (around 65K hex cells), I've taken time step as 0.03
lxlylzl is offline   Reply With Quote

Old   July 18, 2012, 09:04
Default
  #19
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,006
Rep Power: 15
RodriguezFatz will become famous soon enough
Quote:
Originally Posted by lxlylzl View Post
I couldn't achieve convergence with 2nd order upwind with DPM (image attached).
With single phase, i somehow got convergence (image attached).
That sounds exactly like my problem. Try 1st order upwind.
RodriguezFatz is offline   Reply With Quote

Old   July 18, 2012, 09:31
Default
  #20
New Member
 
Join Date: Oct 2010
Posts: 20
Rep Power: 6
lakhi is on a distinguished road
I'm having the same problem too.
lakhi is offline   Reply With Quote

Reply

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
Convergence problem in a vertical vessel juliom CFX 3 March 14, 2012 18:21
source term in a gas mixture problem Kevin CD-adapco 0 March 27, 2008 07:55
Convergence problem for P1 & Energy HP FLUENT 5 May 21, 2005 16:01
convergence problem Trushar Phoenics 5 August 28, 2002 00:40
cyclone problem Jichun FLUENT 4 May 16, 2002 05:43


All times are GMT -4. The time now is 11:10.