[urosgrivc]

and why is the 1st solution I mentioned not ok?

Just load your 15th timestep or choose from the (clock) tipe of buton on top in post

[gbrajtm]

Originally Posted by urosgrivc

and why is the 1st solution I mentioned not ok?

Just load your 15th timestep or choose from the (clock) tipe of buton on top in post

My requirement needs a force from expression.

I am using this expression in optimisation problem as the output parameter to design of experiments (DOE). This DOE takes the values of the first time step, which not a desirable for my problem. Instead, i want maximum value of force among all time steps (nearly 250 are there in my analysis).
To obtain this I have to write an expression which could calculate the force at a particular time (time belong to max value of force) then i can assign this expression as the output parameter to DOE.

[urosgrivc]

Now this is quite a diferent thing than originaly posted.
i think this will be a tough nut to crack.

I am thinking something about; if and acumulated timestep but i doubt that this will work in this case,

[gbrajtm]

Yea, I am trying all possible ways but it still taking the default time. If could manage to calculate the force though CEL with a current time step, it would solve my problem. Since I know which time have maximum value of Force.

Thank you.

[Ali Di]

Dear forum members,

I want to monitor maximum of entered fluid mass and its position in a specific volume of a tank which is empty, but I don't know how do this by adjusting monitor expressions in output control in CFX?

Thank you very much in advance.

[Gert-Jan]

You have to split up and mesh your tank in different named volume parts. Then in Pre you can add expressions like volInt(Liquid 1.Mass Fraction)@volume 1 where it integrates the total amount of of the volume represented by the massfraction of the substance you are interested in.

The maximum position can be derived from an isosurface of a certain massfraction value (e.g. 0.5). Then you can create an expression like maxVal(Z)@Isosurface 1, where Z is the z-coordinate. But I think this cannot be done during the solving process, but only afterwards in Post using transient files.

[Ali Di]

Dear Jan,

Thanks for your solution, I tried your solution but it gives me a m^3 parameter, whereas I want a Kg parameter. Therefore, I have tried "massFlowInt(Liquid 1.Volume Fraction)@Fluid Fluid Interface" which gives me mass rate of flowing Fluid 1. But, it just works in "Post", whereas as I want this parameter in "Pre". Can you help me to solve this problem?

About second solution you are right it cant be done in Pre. But, my mean was center of mass of the entered mass in specific volume.

Thanks for all your help

[ghorrocks]

Gert's function returns a volume, so if you want the mass of fluid you just multiply it by density. This function should work fine in the solver.

You are correct that the isosurface function only works in CFD-Post.

[Ali Di]

Thank you Glenn, you are right. That was my fault.

Do you have any idea how I can locate CoM of moving fluid in the solver?

[ghorrocks]

This should give you the x location: volumeInt(density*x)@domain/volumeInt(density)@domain

[Ali Di]

Dear Glenn,

Thank you for your comment. It was really helpful. But, there are two problem. First, this function works in CFX-Post, since just single recognized variables are supported by volumeInt in CFX-Pre.

Moreover, I want to simulate a turbulent fluid, so I have a two-phase fluid (water and air) and this function considers both phases as a unit fluid (water) in considered domain and give me a constant value all over simulation time for vertical axis (z axis).

[AtoHM]

I hope I understand your question correctly. In a multiphase simulation you can (or better have to?!) distinguish between the phases by prefixing the phase to the variable you look at. Instead of volumeInt(Velocity) you would write volumeInt(Fluid.Velocity).

[Ali Di]

Dear M,

Thank you for your helpful comment. In my problem it works if I could distinguish between Z axes. I mean Z axis for water and Z axis for air. Therefore, I have tried volumeInt(Density*water.Velocity w*t)/volumeInt(Density). But, I think it's wrong.

[Opaque]

The workaround of using expressions in the argument of functions in CFX-Pre is to create Algebraic Equation Additional Variable, say

MyAVExpressionX

as Unspecified and the dimensions expected for the expression, then activate the variable in the domain of interest (kg/m^3 * m)

Additional Variable Value = Density * x

Then, in the other expression use

CofMx = volumeInt( MyAVExpressionX)@Domain / volumeInt(Density)@Domain

Repeat for CofMy, and CofMz

[Ali Di]

Thank you for your comment. But, if you mean

MyAVExpressionX=Density*x

and

CofMx = volumeInt( MyAVExpressionX)@Domain / volumeInt(Density)@Domain

it didnt work, and I faced to the same error.

[Gert-Jan]

And what is "the same error". The same as what?
Don't let us guess. Please share a screenshot or a text file.

[Ali Di]

When I add this expression (CofMx) to a monitor point, this is the error that I face to:

Only arguments that consist of a single recognized variable name are supported by the solver.

[Ali Di]

Dear Glenn,

Since I simulate turbulent and two-phase fluid (water and air), do you think that following expression give me more precise response?

volumeInt(water.Density*water.Volume Fraction*z)@region/volumeInt(water.Density)@region

Thank you so much.

[ghorrocks]

Opaque's post told you how to work around that error.

Whether your equation or my original equation is more accurate depends on what you are trying to do and what you are trying to measure. If you want the COM of the entire fluid domain then mine is the correct one. If you want the COM of the water fraction only then yours is the correct one. I don't know what you are trying to do, so cannot say what is correct.

[AS_Aero]

Hi All

I have a channel inside which I have some wall with holes in it. I have interface at these holes as I have divided my domain as inlet domain and outlet domain. Now the thing is I need to monitor the massflow/volumeflow through these holes. I am not able to do this because when I give in OutputControl monitor, CFX says unvalid surface is selected
In my expression I selected Interface_holes