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

steady state problem

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

Like Tree1Likes
  • 1 Post By urosgrivc

Reply
 
LinkBack Thread Tools Display Modes
Old   April 24, 2016, 09:43
Default steady state problem
  #1
Senior Member
 
yaseen
Join Date: Oct 2015
Location: Hawler
Posts: 155
Rep Power: 3
yaseen wsu is on a distinguished road
hello every one
in steady state of free surface flow model, I have problem in mass air in all iteration is (ok), and after about 1000 iteration most equations doesnot reach (RMS residual 1*10^-4) which is required. is it related to small time scale?
thanks for your help

http://www.cfd-online.com/Forums/att...1&d=1461505262
http://www.cfd-online.com/Forums/att...1&d=1461505325
Attached Images
File Type: jpg 20160424_162249.jpg (167.9 KB, 13 views)
File Type: jpg 20160424_162307.jpg (199.6 KB, 9 views)
yaseen wsu is offline   Reply With Quote

Old   April 25, 2016, 02:25
Default
  #2
Senior Member
 
urosgrivc
Join Date: Dec 2015
Location: Slovenija
Posts: 126
Rep Power: 3
urosgrivc is on a distinguished road
+Are you monitoring any points?
Like: Volume fraction of the fluid in the domain or avgturbKE in the domain.

+Did imbalances fall low enough?
Check under workspace->new monitor->imbalances in solver manager

It is posible that it has converged already with the boundary conditions you have or mesh size you have.
I think that if monitor poins did not converge in 1000 iterations there is something wrong with the settings of the simulation or mesh.

Residuals could be high as you probably have two tipes of fluid in the same domain, so monitor points are beter to determine if it has converged or not.
But there is definitly no need to wait for more than 1000 iterations as it should converge in less than that.
urosgrivc is offline   Reply With Quote

Old   April 25, 2016, 06:44
Default
  #3
Senior Member
 
yaseen
Join Date: Oct 2015
Location: Hawler
Posts: 155
Rep Power: 3
yaseen wsu is on a distinguished road
my imbalances good (according to mass flow rate), I didnot add any monitor points.
what do you mean by avgturbKE in the domain? where is added (outlet ...)?
yaseen wsu is offline   Reply With Quote

Old   April 25, 2016, 07:01
Default
  #4
Senior Member
 
urosgrivc
Join Date: Dec 2015
Location: Slovenija
Posts: 126
Rep Power: 3
urosgrivc is on a distinguished road
It is best to add (wariables of interest as monitor points) in CFX-pre

That way you can monitor convergence of wariables that actualy matter to you while the solver runs.

If these converge or dont change threw iterations the problem has converged with the settings it was set up with

Wariables of interest can be anything (average domain temperature, mass flow, average pressure, Force, Moment, avgturbKE....) ones that are important to you

If you have a dual fluid domain problem you probably want to know how much of one fluid is in the domain so wariable of interest is definetly Volume fraction (Except you have a closed sistem)

than this walue is not apropriate for convergece valiadation as it will be constant from the begining (AVGtemp is also not apropriate for you as you dont have heat transfer)


You can set them up like this:
as you have k-epsilon or sst model included i proposed avgturbKE, as if this stops changing (it has converged) the flow will in general not change enymore with additional iterations.
You set up an expression volavg(turbKE)@yourdomain than set under output monitor point with this expression.

Just a sugestion as I dont know what You are simulating.
urosgrivc is offline   Reply With Quote

Old   April 25, 2016, 09:32
Default
  #5
Senior Member
 
yaseen
Join Date: Oct 2015
Location: Hawler
Posts: 155
Rep Power: 3
yaseen wsu is on a distinguished road
Quote:
Originally Posted by urosgrivc View Post
It is best to add (wariables of interest as monitor points) in CFX-pre

That way you can monitor convergence of wariables that actualy matter to you while the solver runs.

If these converge or dont change threw iterations the problem has converged with the settings it was set up with

Wariables of interest can be anything (average domain temperature, mass flow, average pressure, Force, Moment, avgturbKE....) ones that are important to you

If you have a dual fluid domain problem you probably want to know how much of one fluid is in the domain so wariable of interest is definetly Volume fraction (Except you have a closed sistem)

than this walue is not apropriate for convergece valiadation as it will be constant from the begining (AVGtemp is also not apropriate for you as you dont have heat transfer)


You can set them up like this:
as you have k-epsilon or sst model included i proposed avgturbKE, as if this stops changing (it has converged) the flow will in general not change enymore with additional iterations.
You set up an expression volavg(turbKE)@yourdomain than set under output monitor point with this expression.

Just a sugestion as I dont know what You are simulating.
thanks for your suggestion
ok, Iam simulating free surface water in spillway, volume of fraction and mass flow important to me. when I add monitor output via expression volavg(turbKE)@outlet (or domain???), then how can see them after completion run??? I used RNGK-E turb. model
yaseen wsu is offline   Reply With Quote

Old   April 26, 2016, 01:22
Default
  #6
Senior Member
 
urosgrivc
Join Date: Dec 2015
Location: Slovenija
Posts: 126
Rep Power: 3
urosgrivc is on a distinguished road
Hi
Do you have a massflow as an inlet boundary condition? if yes than measuring masflow on outlet is not usefull as it will be the same as inlet and a constant, if not
than you can set Water.massFlow()@outlet to measure mass flow of water at outlet plane vhile solving.

-for the other question volumeavg(tubrKE) already means that location must be a volume, your outlet is probably a plane so no it wont work that way. You can set that one asveal
volumeAve(Turbulence Kinetic Energy)@Yourdomainname

or this one, thiss will tel you how much watter is in the domain
massInt(Water.Volume fraction)@Yourdomainname

CFX will help you pick up the wright wariables from in the expression tab. Dont copy paste this ones as I still know wery litle about your problem

If you set these three you should be able to see when the problem will converge. and yes you can see all in the solver manager and in cfx-post
either these are wright or I understood the phisics of your problem incorectly.
urosgrivc is offline   Reply With Quote

Old   April 26, 2016, 01:35
Default
  #7
Senior Member
 
yaseen
Join Date: Oct 2015
Location: Hawler
Posts: 155
Rep Power: 3
yaseen wsu is on a distinguished road
yes you are right, my inflow is velocity not massinflow
as you said monotor points can be seen in solver manager after run completion, is that? like imbalances ..... and in expression I can create them, they need names like (UpH, UpVFWater)
yaseen wsu is offline   Reply With Quote

Old   April 26, 2016, 01:43
Default
  #8
Senior Member
 
urosgrivc
Join Date: Dec 2015
Location: Slovenija
Posts: 126
Rep Power: 3
urosgrivc is on a distinguished road
Yes that is wright.
When these waribles stop changing you now that convergence is reached.
And yes these monitor points are updated every iteration and you see them as graph in solver manager.

Vhen you have an expression (with a name yes) next thing is to create monitor points in (output control)->(monitor)->(monitor points and expressions)->create it and insert in expresion you have created

And if you have velocity inflow of water threw an area that is not changing -> this is a massinflow as massflow=area*velocity*densiti vhich are all constants.
So mass flow at an outlet will still probably be a constant, unless something else happens in betven that I dont know of.
and if it is a constant than meassuring massflow on outlet is NOT a valid way of determining convergence.
volumeavg(turbKE) should still work as it is only flow dependant.
yaseen wsu likes this.
urosgrivc is offline   Reply With Quote

Old   April 26, 2016, 09:39
Default
  #9
Senior Member
 
yaseen
Join Date: Oct 2015
Location: Hawler
Posts: 155
Rep Power: 3
yaseen wsu is on a distinguished road
Quote:
Originally Posted by urosgrivc View Post
Yes that is wright.
When these waribles stop changing you now that convergence is reached.
And yes these monitor points are updated every iteration and you see them as graph in solver manager.

Vhen you have an expression (with a name yes) next thing is to create monitor points in (output control)->(monitor)->(monitor points and expressions)->create it and insert in expresion you have created

And if you have velocity inflow of water threw an area that is not changing -> this is a massinflow as massflow=area*velocity*densiti vhich are all constants.
So mass flow at an outlet will still probably be a constant, unless something else happens in betven that I dont know of.
and if it is a constant than meassuring massflow on outlet is NOT a valid way of determining convergence.
volumeavg(turbKE) should still work as it is only flow dependant.
I have the following error when I create expression in expression tab in the name (monitor 1) and then create monitor point vis expression 1- I put name of expression (monitor 1) in the blank field 2- I put (Water.massFlow()@outle) in the blank field in both cases error happens.
thanks

http://www.cfd-online.com/Forums/att...1&d=1461677739
http://www.cfd-online.com/Forums/att...1&d=1461677754
Attached Images
File Type: jpg monitor1.jpg (35.9 KB, 10 views)
File Type: png expression.png (5.3 KB, 6 views)
yaseen wsu is offline   Reply With Quote

Old   April 26, 2016, 10:00
Default
  #10
Senior Member
 
Join Date: Aug 2014
Posts: 176
Rep Power: 4
fresty is on a distinguished road
"outlet" is surely not the what you named your outlet region as.. you may need to recheck that .. precisely i mean, should even match the letter case..
fresty is offline   Reply With Quote

Old   April 26, 2016, 11:06
Default
  #11
Senior Member
 
urosgrivc
Join Date: Dec 2015
Location: Slovenija
Posts: 126
Rep Power: 3
urosgrivc is on a distinguished road
Yes like fresty sad, there is something wrong with the name of your outlet plane.
@location
edit your expression
delete the word outlet -> right click behind the @ sign -> phisics locators -> 2D -> "select your outlet plane name"

CFX tels you alot about the problems that occure becouse of users mistakes.
Be sure to read them cerfully
Also if the solver fails or something, cfx provides wery good sugestions and answers to what went wrong.
urosgrivc 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
Solver for transonic flow? Martin Hegedus OpenFOAM Running, Solving & CFD 22 December 16, 2015 05:59
Problem with pimpleDyMFoam: Initialise steady state solution Lancester OpenFOAM Running, Solving & CFD 2 September 29, 2015 09:49
POPULATION BALANCE MODELING (PBM) in Steady State osha Fluent Multiphase 0 July 18, 2015 19:09
Convergence problem using simpleFoam steady state vvqf OpenFOAM Running, Solving & CFD 12 May 18, 2011 07:51
steady state PISO problem denizen CD-adapco 0 December 20, 2006 03:55


All times are GMT -4. The time now is 02:05.