mass inflow rate
 

I simulated free surface for inlet boundary condition I enter normal flow velocity after simulation the result of mass inlet is similar as I entered in terms velocity with coarse mesh, but same simulation with fine mesh it give me lesser mass in flow rate. what is that reason? how to over come this problem?
thanks

Your mesh is too coarse, so the mesh resolution is affecting results. You need to refine your mesh until it does not affect your results. This is called a mesh sensitivity study.

thanks for your reply
but I think you misunderstand from my problem, I did sensitivity analysis but I say in coarse mesh I have no problem, but in finer mesh in flow does not equal as I entered in terms of velocity (ex. I enter 33.5 kg/s, it give me 32.5 kg/sec)
note: (there is no problem of mass balance outlet approximately inlet but less than as I entered)

maybe try to measure the surface area of the inlet? Why not specify a mass flow? Whats the pressure?
Make a surface contour ot the velocity at the inlet in CFD post, see if the velocity (and pressure) is the constant across the entire inlet.
What is going in, a gas? Then if its moving fast, the density gets lower, hence with high velocity the mass flow gets lower.
So check pressure drop as well.
If your model was not converged and you changed something, that also may happen.
Also, finer mesh, what actually did you define? Towards the wall velocity is lower, with finer mesh the velocity distribution over a cross section becomes more accurate (see mesh inflation on walls)

You are right, I don't think I understand your question. Are you saying that the coarse mesh result is accurate but the fine mesh result is not accurate? Or are you saying that on the fine mesh simulation the boundary conditions are not applied correctly?

free surface inlet? Maybe its opening or entrainment?
Then check in the solver, if it creates a wall.

Could be continuing the same simulation, just changing the mesh. Because the solver (if not set initialisation) continues with the previous results. If it has not converged before, it keeps on going with some residuals.

The finer the mesh, the closer the surface area of the inlet is to the CAD model.

the question is just too unspecific.

thanks
but my question is specific in free surface flow, usually we take all the surface as inlet and from expression define inlet water height (UpH), in initialization set pressure, Vol of fluid .....
as I refined mesh (to the required) this reduce of mass inflow increase

I still do not understand what you are saying. Please post an image of what you are seeing and your CCL for both runs.

Yaseen, I think it would be helpful if you wrote all information about your project right in the first post. In the last few weeks, you have been opening new topics again and again and usually it took around 10 posts to find out what you are actually trying to ask.
Maybe in your case, it would even be useful if you added new questions about your project in old threads so that you don't have to describe your project over and over again.
Just my thoughts...

so its only driven by gravity? Not much pressure to get the 32kg through?
Maybe try different meshes, see what happens. I doubt, it makes so much of a difference.
Maybe just check the inlet conditions.
Take the model where you got the proper results, check that it converged. Save as new project, just refine the mesh and run the solver again.

Dear Glenn
the follow images are my model as I said my inlet flow rate (33.45 kg/s) I put inlet B.C. with normal velocity CFX in coarse mesh there is noproblem but in fine (which is necessary) this inlet flow rate become (32.5 kg/sec) after simulation
https://drive.google.com/open?id=0B3...mhIaDAySllkMk0
https://drive.google.com/open?id=0B3...F9OVUJHZFdreGs
https://drive.google.com/open?id=0B3...WhrcFNXMlRZck0
https://drive.google.com/open?id=0B3...FdackJuSG5OTUk

You are specifying the inlet velocity and volume fraction. So any variations you are getting from your expected mass flow rate are likely to be due to the free surface jumping between nodes as you refine your mesh. In other words - your initial condition does not specify the free surface level to sub-grid accuracy. You just change it from 0 to 1, so the solver has to guess where the actual free surface level is. There will be some error in this guess and that will create small changes in mass flow rate as you change the mesh.

The fix for this is to blur the initial free surface over a few elements. The solver does this anyway as the run progresses, so if you define the initial condition like this it will specify the free surface level to sub-grid accuracy and make it converge better too. Have a look in the documentation for how to create an blurred initial free surface level.

thanks for your reply
dear Maxim, yes I posted even more than 10 posts because I dont find any way to get the target. Iam MSc student my study on simulation of side channel spillway so only about three months to finish my study. the second one ANSYS Consultancy is very costly (1000$ per hour), and you know free surface model has problems of convergence, time step, B.C ..... to overcome these problem only I used CFX documentation and forum.
so sorry for extra posting.
thanks

I understand your situation - I have been there as well as a student :)
Usually it is better not "hijack" old threads with new questions but I was thinking that maybe in your case it might be helpful to post follow-up questions in the same thread since you are working on one project.
But I leave that decision to the admins and mods :)
Good luck and sorry that I can't help you more

Maxim thank a lot

Dear glenn
I read CFX model initialization part but I do not blurred initial free surface level, can you tell me more detail, what is blur intial free surface??

Have a look at the free surface generated by your initial condition. It will jump from VF=0 to VF=1 in one element. Run a free surface simulation for a while (any simulation, the tutorial example will be OK) and have a look at the free surface. The transition from VF=0 to VF=1 occurs over about 4 element lengths. So as the simulation runs it naturally blurs the surface over a few element lengths.

You will find that the CFX solver runs best when the free surface is blurred over a few elements like this. When you start with a sharp initial condition one of the reasons you get poor convergence in the first iterations is that it has to blur the surface. So you can improve convergence by starting with an initially blurred surface.

And secondly, if you look at your initial surface you will note it has small steps and jumps in it. This is where the surface jumps from one element to the next. This is where your small error in mass flow rate is coming from and why it is mesh dependant. After a few iterations the free surface is smooth as it is blurred over a few elements and the free surface is accurately resolved to sub-grid accuracy.

Have a look in the CFX documentation, CFX Modelling guide under free surface flow/surface tension.

thanks for your long definition of the problem
as in documentation said When setting initial conditions for surface tension calculations, it may also be beneficial to assign a smeared volume fraction rather than a discontinuous one, is my case discontinuous, it talked bout droplet radius and centroid.
so, if I increase (UpH) by a small amount this problem can be overcome? please what is your suggestion, or change VF air and water from expression to value 0 and 1
thanks

No, the function smears the surface over a few element lengths. You need to do the same. Keep the free surface height the same, but use a smearing function so it transitions over a few element lengths.

I wrote the following relation in Expression
rdrop = 0.3 [m]
dist = rdrop - sqrt((x-0.5 [m])^2 + (y-0.5[m]^0.5)
delta = 0.01 [m]
drop = 0.5*tanh(dist/delta)+0.5
but nothing happen, also I used laplacian (volume-weighted) for initial volume fraction smoothing in solver control, but have the same problem as before.