CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > CFX

Finmes error

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   April 13, 2015, 03:29
Default Finmes error
  #1
New Member
 
Alessio Mancini
Join Date: Apr 2015
Posts: 19
Rep Power: 9
Aliosha86 is on a distinguished road
Hi guys,

I am running a simulation with CFX for my thesis. The problem is simple: I have to pressurize a tank with an air flow. My initial condition are 300 Pa and 293 K in the entire volume. The pressurization of the tank must be done imposing a time-dependent flow rate. The flow rate is imposed at the inlet through a law obtained by a regression of the experimental data.
I previously run a simulation with 2000 Pa and 293. The flow is subsonic and I have any problems. The results are in perfect agreement with the experimental ones. The results are obtained using SSG turbolence model, a time step of 0.01 seconds.

Now changing the initial condition to 300 Pa, CFX do only few iterations and then gives me the message "FINMES error". Probably I have to reduce my time-step to 0.001 sec, but in this case the simulation starts, but it does not follow the experimental results giving me a lot of peaks and other strange things.
I run this simulation using the same turbolence model, and I changed the "solver advanced control" using "high speed numerics, pressure control and etc..". Probably in some point of the field the flow can become supersonic.

Does anyone have some suggestions???

Thanks in advance

Alessio
Aliosha86 is offline   Reply With Quote

Old   April 13, 2015, 04:09
Default
  #2
Member
 
Nick
Join Date: Apr 2015
Posts: 40
Rep Power: 9
nickjuana is on a distinguished road
Try other turbulence models like K-omega and K-epsilon.
nickjuana is offline   Reply With Quote

Old   April 13, 2015, 07:19
Default
  #3
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,233
Rep Power: 135
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
I agree - use a simpler turbulence model unless you know you need the SSG model.

And your question is an FAQ: http://www.cfd-online.com/Wiki/Ansys...do_about_it.3F
ghorrocks is offline   Reply With Quote

Old   April 13, 2015, 08:00
Default
  #4
New Member
 
Alessio Mancini
Join Date: Apr 2015
Posts: 19
Rep Power: 9
Aliosha86 is on a distinguished road
Thanks, but I started with the k-epsilon model, and the results were not so good. I tried this model because it gave me the best results with the initial condition of 2000 Pa.
Aliosha86 is offline   Reply With Quote

Old   April 13, 2015, 08:23
Default
  #5
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,233
Rep Power: 135
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
The SSG model is chronically unstable and hard to converge. It is no surprise you are having problems with it. Do not use SSG unless you know you need it (and know why you need it ).

The turbulence model I recommend is SST. Give it a try - it is the best general purpose turbulence model in CFX. It also has options for curvature correction and lots of other things which may assist. SST is also quite stable and easy to use.
ghorrocks is offline   Reply With Quote

Old   April 13, 2015, 09:00
Default
  #6
New Member
 
Alessio Mancini
Join Date: Apr 2015
Posts: 19
Rep Power: 9
Aliosha86 is on a distinguished road
Thanks I will give it a look and I will let u know

Do you think that it can be also suitable for flows which became supersonic starting from subsonic condition?
Aliosha86 is offline   Reply With Quote

Old   April 13, 2015, 19:09
Default
  #7
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,233
Rep Power: 135
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Yes, that is fine.
ghorrocks is offline   Reply With Quote

Old   April 14, 2015, 03:42
Default
  #8
New Member
 
Alessio Mancini
Join Date: Apr 2015
Posts: 19
Rep Power: 9
Aliosha86 is on a distinguished road
I started the simulation with the SST model and it runs. Nevertheless, the graphic of the pressure is not so clean as I expected. I get a constant pressurization rate after the transient of the valve but during the transient the pressure has a strange behaviour. I attach the graphics of the pressure and the temperature.

In parallel I am also running a simulation with the k-omega model, and I hope to get the right results. Or a least I can make a comparison on which model can be the best option.

Thank you very much for the advice, and if you have any ideas do not hesitate to suggest.



Alessio
Attached Images
File Type: jpg Pressure.jpg (31.6 KB, 9 views)
File Type: jpg Temperature.jpg (30.6 KB, 9 views)
Aliosha86 is offline   Reply With Quote

Old   April 15, 2015, 07:23
Default
  #9
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,233
Rep Power: 135
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Why do you think the rate should be smooth? Shouldn't there be shock waves and other flow features bouncing around?

It is highly unlikely that simply switching turbulence model will make the results "correct". I recommend you stay with the SST model and read this FAQ: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F
ghorrocks is offline   Reply With Quote

Old   April 16, 2015, 03:39
Default
  #10
New Member
 
Alessio Mancini
Join Date: Apr 2015
Posts: 19
Rep Power: 9
Aliosha86 is on a distinguished road
Glenn, I know that physics rules above numerics . Shock waves exists and I cannot get rid of them
Therefore, I am expecting a bunch of shock waves, because my flow became early supersonic.

What seems strange to me is that the behaviour is linear for a period of time, then became messy and became linear again. I do not know if there are some numerical errors that affect my simulation.
That is why I want to check some different models, just to verify which is more stable and robust.



Alessio
Aliosha86 is offline   Reply With Quote

Old   April 16, 2015, 04:47
Default
  #11
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,233
Rep Power: 135
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
These features are unlikely to be turbulence model related. Much more likely it is initial transients and shock waves.
ghorrocks is offline   Reply With Quote

Old   April 16, 2015, 05:08
Default
  #12
Senior Member
 
Thomas MADELEINE
Join Date: Oct 2014
Posts: 126
Rep Power: 10
Thomas MADELEINE is on a distinguished road
if there are shock waves I would rather use k-omega instead of SST.
SST use k-omega only for near wall region and k-epsilon in the middle of the fluid region (if I understood clearly).

Problem is k-epsilon model have some troubles with big pressure evolution like shock wave.
I had this problem a while ago in a nozzle and using k-omega model helped me.
Thomas MADELEINE is offline   Reply With Quote

Old   April 16, 2015, 06:24
Default
  #13
New Member
 
Alessio Mancini
Join Date: Apr 2015
Posts: 19
Rep Power: 9
Aliosha86 is on a distinguished road
Thanks Thomas. I agree with you. The k-omega model seems to reproduce the pressurization rate that I measure with my sensors during the experiments.
But I have to wait till my simulation stops to be sure of these results.


Alessio
Aliosha86 is offline   Reply With Quote

Reply

Tags
cfx, finmes, supersonic flow

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
[OpenFOAM.org] compile error in dynamicMesh and thermophysicalModels libraries NickG OpenFOAM Installation 3 December 30, 2019 01:21
[blockMesh] blockMesh with double grading. spwater OpenFOAM Meshing & Mesh Conversion 92 January 12, 2019 10:00
Ansys Fluent 13.0 UDF compilation problem in Window XP (32 bit) Yogini Fluent UDF and Scheme Programming 7 October 3, 2012 08:24
checking the system setup and Qt version vivek070176 OpenFOAM Installation 22 June 1, 2010 13:34
POSDAT problem piotka STAR-CD 4 June 12, 2009 09:43


All times are GMT -4. The time now is 11:54.