|
steady state problem
2 Attachment(s)
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 |
+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. |
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 ...)? |
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. :) |
Quote:
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 |
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. |
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) |
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. |
2 Attachment(s)
Quote:
thanks http://www.cfd-online.com/Forums/att...1&d=1461677739 http://www.cfd-online.com/Forums/att...1&d=1461677754 |
"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..
|
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. |
| All times are GMT -4. The time now is 07:59. |