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

Hey Fluent wizards..Need help here !!

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

Reply
 
LinkBack Thread Tools Display Modes
Old   June 14, 2006, 01:34
Default Hey Fluent wizards..Need help here !!
  #1
Amr
Guest
 
Posts: n/a
All,

I am simulating a heat-flow problem that is a real pain. The problem is a 3-D rectangular room (3.4L X 3.3W X 3.05H) in meters with a 2 m high door at the east wall. Fire is supposed to be simulated through a non combustion approach as heat and mass sources of CO2 and H2O. It is desired to calculate the transient distribution of temperature and gases for up to 300 seconds. Volumetric heat and mass sources are presented in the room domain by a separate fluid zone (cube) on the room's floor. My BC's are pressure outlet at the door and a steady heat and mass sources (6 MW /m3) and 0.136 kg/m3 respectively.

I have done so many trails trying to simulate this experiment with no good as follows:

-Without combustion, a steady heat source of 6 MW, issued from a separate fluid zone. -Smoke is alternatively simulated as CO2 and H2O from a "mass flow inlet" with different mass fractions from the bottom face of the "fire zone". -A mixture of O2, N2, H2O and CO2 is set so as all properties are temperature dependant (kinetic theory). -Density is set to be "compressible Ideal gas" or "Incompressible ideal gas", Bousinessque approximation is not used. -Standard k-e model used with standard near wall treatment. -Used "body force weighed", Quick, 1st order discretization schemes for pressure, density and other equations respectively. -Gird is comprised of perfect hexahederals with maximum skewness of 0.2. Spacing is 10 cm all over. Note that gird adaption was used near the fire zone (with hanging nodes) so that grid spacing near fire source was 3 cm. Initial elements count is 35000. -Segregated solver was used. Transient simulation with 0.5 sec, and once with 1e-10 sec for a 600 seconds duration.

1- In the above simulations -while setting a 0.5 sec time step and very low URF's- I was not getting convergence in terms of total mass flow rate inside the domain (mass conservation). Scaled residues were dropping to 1e-3 in the first few iterations with high fluctuations.

2- I noticed that the convergence works okay when I decreased the time step size to 1e-5. For such, even with adaptive time settings, I waited for two whole days and it only made 0.002 sec !!!. This would take weeks to finish my simulation.

3- Have tried to see simulations with reduced heat and mass sources of (10 KW/m3 and 0.013 kg/m3) with the coupled solver "with CFL of 100" and once with the segregated solver. This worked well in terms of convergence and residues though more robust with the coupled solver.

4- Now, till this moment, I failed to simulate the problem with the complete heat and mass sources defined. I am thinking that Fluent is not accepting the sudden introduction of large heat and mass sources even with low URF's. Could UDF's that is increasing till the steady complete value of heat or mass sources be a rescue?

Would so much appreciate any of your advices as what are better practices (or do's and don'ts) that may guide. I am in real need for any help in this transient heat-flow problem. Looking forward to hearing back from you.

Cheers, Amr

  Reply With Quote

Old   June 14, 2006, 04:06
Default Re: Hey Fluent wizards..Need help here !!
  #2
Swarup
Guest
 
Posts: n/a
1. adaptive time stepping is a tricky game. I have never managed to tame it (even with Fluent recommendations). It generally sits on the smallest time step that you set and is very sensitive to errors. Manual advises you to continue with old time step for some number of iterations. 2. CFL of 100 appears very large considering the default of 1 (explicit) and 5(implicit). 3. Sudden appearance of source is indeed unsettling. It will sometimes also lead to repeated temperature limit messages. In this case, gradual ramping up of source terms can be a good alternate. But there is a difficulty; how will you determine the steady state if you have no knowledge of time dependence of source?

Swarup.
  Reply With Quote

Old   June 14, 2006, 04:09
Default Re: Hey Fluent wizards..Need help here !!
  #3
Swarup
Guest
 
Posts: n/a
Additionally,

are you sure you have taken required inputs for a natural convection problem into consideration?

Swarup.
  Reply With Quote

Old   June 14, 2006, 04:30
Default Re: Hey Fluent wizards..Need help here !!
  #4
Swarup
Guest
 
Posts: n/a
Check this:

your mass source unit is suspect: you should have mass rate per unit volume.

also, note that your mass if not accompanied by some momentum source will tend to reduce temperature and momentum of your domain. This can cause difficulties.

Swarup.
  Reply With Quote

Old   June 14, 2006, 08:31
Default Re: Hey Fluent wizards..Need help here !!
  #5
Amr
Guest
 
Posts: n/a
Hi Swarup,

Very glad to see you responding. I agree with you that the adaptive time setting is a hard game. From my many trials I performed I noticed that the coupled solver gives relatively good results but with a much less heat generation. In these runs, I also noticed that convergence and residues drop happens faster with higher CFL. Yes, in manual, it is mentioned that CFL could be even 100 or higher (but it is not wise to start with 100).

I came to understand that there is actually a problem with the sudden appearance of heat source espicially. Do you know why???.

Regarding the heat ramping, I am simulating a validation case where I have the heat generation curve. Yes, in the experiment, the heat generation starts from zero till it reaches 3 MW in 100 seconds, then it settles at 3 MW till the end of the 600 sec.
  Reply With Quote

Old   June 14, 2006, 08:41
Default Re: Hey Fluent wizards..Need help here !!
  #6
Amr
Guest
 
Posts: n/a
Yes, I am aware of the manual at this part. To check with you, the following are set:

1- Pressure discretization is |Body force weighted. URF: 0.3

2-Density discretization is 1st order and then after 1st time step it is Quick. URF; 0.5. Density is set for compressible ideal gas.

3-Gravity is set -9.8 in z direction. Full buoyancy effect is accounted in the k-e model.

4-Pressure-velocity coupling is PISO.

5-Time step was set to 1e-5 at the beginning when I was setting the 3 MW source. It worked fine, but took two days for 0.2 second. Results are different when I reduced the heat source.

6-Momentum URF: 0.5, Energy URF: 0.2
  Reply With Quote

Old   June 14, 2006, 09:06
Default Re: Hey Fluent wizards..Need help here !!
  #7
Amr
Guest
 
Posts: n/a
Hi Swarup,

|I have taken care of my mass source unit. It's set as kg/s/m3.

Yes, I only set mass sources with no momentum of turbulence sources. I thought, Fluent will calculate their velolcity from the known zone's volume. Why is it really necessary to set a momentum source?.

In regards to my previous message, would you think a heat generation udf that specifies the ramp up curve would help?.

One interesting thing to share with you is that I tried to set my full 3 MW -which becomes 6e06 Watts/m3- with a time step of 0.5 sec. and very low URFs for Temperature and momentum as 1e-05 and 0.0001 respectively. Though residues were dropped to convergence limits in only two iterations, the temperature and species countours are not representing reality (i.e. after 60 sec for example, it shows you the expected contours of after 3 seconds).

As for grid resolution, -and only when I performed tests with a smaller heat generation 100000 MW/m3- I made a coarse grid of 0.1 m spacing, and in the other one, I just made grid adaption so that the area above smoke plume is approximately 0.05 m spacing. For the segregated solver, the grid resolution matters alot. Even with smaller time steps, the segregated solver showed a skewed smoke profile towards the exh. door when I used the coarse gird. With the coupled solver, however, countours were going okay even with coarse grid. Do you know why?

Cheers, Amr
  Reply With Quote

Old   June 14, 2006, 10:12
Default Re: Hey Fluent wizards..Need help here !!
  #8
Swarup
Guest
 
Posts: n/a
Hi Amr,

I do not know about the need of momentum source along with a mass source. If you read manual, there is a clear mention of this requirement. It is said that other sources can be on their own. However, in some cases, you may have a dead mass. One reason could be nature of this term physically. It just appears numerically and not as a part of "domain". Moreover, look at the units: you are really mentioning a moving mass (due to mass rate). This is not very obvious.

As far as ramping is concerned, since you have experimental situation, it is better to "mimic" it and it is proper also.

It is a bad idea to have very low URFs and then call solution as converged! It's spurious. URFs are only to under-relax changes in the early phases and ideally you should gradually restore them back if possible.

Fine grids tend to deteriorate multigrid performance when no reasonably good initial solution is available. What is recommended solver in such problems? The real comparison should be between explicit and implicit methods of solution.

Swarup.
  Reply With Quote

Old   June 14, 2006, 10:22
Default Re: Hey Fluent wizards..Need help here !!
  #9
Swarup
Guest
 
Posts: n/a
Well,

Higher CFL and convergence is confusing to me! Does your solution start from very good initial values and disturbances build slowly or after some time? Did you see rising residuals once you started your source (and they kept rising)?

This source remains for every time step you advance. Any error in last step is carried over to next one and so on.

Swarup.
  Reply With Quote

Old   June 14, 2006, 12:09
Default Re: Hey Fluent wizards..Need help here !!
  #10
steve
Guest
 
Posts: n/a
hi amr! could you please check the solution by setting the URF for Energy in between 0.95 to 1...

steve
  Reply With Quote

Old   June 14, 2006, 12:21
Default Re: Hey Fluent wizards..Need help here !!
  #11
Amr
Guest
 
Posts: n/a
Hi Swarup,

Thanks for your response. As for the coupled solver run, I started the solution with CFL being 2 and then increased the CFL to 100 gradually. I don't recall having such instabilities, but certainly, residues were not all dropping below 1e-03. Meanwhile, the mass continuity was conserved as appeared in the mass-flow-rate plot for all my domain surfaces (i think this is a good way to judge convergence as the manual says). Do you see anything wrong with that?

As for the natural convection settings, am I missing anything? (please refer to my reply to your question in the previous message). Some people are suspecious about hanging node adaption -which I had performed after importing the mesh from gambit- how does this sound to you?

Regarding your latest message, could you clarify what you mean by a dead mass and a moving mass?. I should be simulating a smoke coming out with a velocity. Based on my simple thinking, Fluent will calculate the smoke velocity from the mass source, volume and calculated density. Do you think I need to set a momentum source still?.

One thing else, do you think the coupled solver will be more suitable in such problems?. I don't really know what benefit can the explicit method brings here. Do you see those benefits?. I would be more than happy to send you a schematic "pdf" document showing my domain. IF this is possible, let me know your email.

Thanks again !. Too much questions, isn't it

Cheers, Amr

  Reply With Quote

Old   June 14, 2006, 12:28
Default Re: Hey Fluent wizards..Need help here !!
  #12
Amr
Guest
 
Posts: n/a
Hi steve,

Happy to see you joining us !.

In regards to what you suggest, I assure you that it won't work. As you may have captured from my previous messages, I have a problem with heat generation. I wish to start the solution with a sudden and constant heat source of 6000000 Watt/m3. I failed to do that and I am tying to understand why. The whole thing works when I reduce the heat generation, but to remove instabilities in energy residues, I need to lower its URF a bit. In this reduced heat source, I think energy URF could be safely restored to 1 after few time steps as you suggest.

Would be happy to know your ideas.

Cheers, Amr
  Reply With Quote

Old   June 14, 2006, 12:46
Default Re: Hey Fluent wizards..Need help here !!
  #13
Swarup
Guest
 
Posts: n/a
Hi Amr,

I will try to answer last two questions now, first two afterwards!

Dead mass is something not moving. This cannot happen in a mass source, not with the units (kg/m2.s) and continuity! This is what I wanted to tell you. In my opinion, you need to set momentum source.

Coupled explicit is considered more time accurate than coupled implicit.

You may send it to: syj02@rediffmail.com (hope it is not very big!)

Regards. Swarup.

  Reply With Quote

Old   June 15, 2006, 03:46
Default Re: How about a UDF for the heat source? !!
  #14
Amr
Guest
 
Posts: n/a
Swarup,

How about utilizing a udf to gradually introduce the fire heat source into the domain?. Have you came across such udf's before or know how they are written?

Also, to respond to your dead mass issue, don't you see that the units in fluent for the mass source is kg/m3.s means that the mass is already with a velocity? Is this interpretation correct?

Cheers, Amr
  Reply With Quote

Old   June 15, 2006, 06:30
Default Re: How about a UDF for the heat source? !!
  #15
Swarup
Guest
 
Posts: n/a
It is simple to introduce such a source. Utilize CURRENT_TIME for flow time. Everything else reamins same in DEFINE_SOURCE like UDFs you find in manual. You need to define your source as a ramp function utilizing CURRENT_TIME. dS[eqn]=0.0 since source is independent of primitive variable (temperature and velocity). Since your source is time dependent, it will either be removed or will be present after some time duration. That condition can also be incorporated in terms of an if statement.

I can very well see that unit! It is straightforward to say that mass is already having some velocity just looking at units. Best help can be from Fluent support so that ambiguity does not exist any longer.

Swarup.
  Reply With Quote

Old   June 15, 2006, 08:04
Default Please note!!
  #16
Swarup
Guest
 
Posts: n/a
I said coupled explicit is more accurate than coupled implicit. This is related to time discretization. Explicit time discretization is improper for incompressible flows. Thanx.

Swarup.
  Reply With Quote

Old   June 15, 2006, 08:27
Default Re: Please note!!
  #17
Amr
Guest
 
Posts: n/a
Hi Swarup,

Thanks alot !. Have you taken a look on my shematic drawing I sent along with my e-mail to you?. Do you have any comments?

Also, I would appreciate your response to my previous couple of concerns regarding convergence judgement based on mass conservation and missing settings for the natural convection problem raised earlier.

Best, Amr

  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
Fluent3DMeshToFoam simvun OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 48 May 14, 2012 05:20
Exporting structured mesh from ICEMCFD to Fluent? jeevan kumar FLUENT 1 January 23, 2012 12:21
Abaqus - Fluent Coupling WITHOUT MPCCI s.mishra FLUENT 0 May 1, 2011 09:45
few quesions on ANSYS ICEMCFD and FLUENT Prakash.Paudel ANSYS 0 August 12, 2010 12:07
Fidap to Fluent Ravi FLUENT 3 July 10, 2008 13:31


All times are GMT -4. The time now is 03:11.