[flyply]

Hello

I simulated the volute and fan (steady state).
For monitoring the data with CFD-Post simultaneously, I used the "User Locations", This feature are available in v17.0, maybe.

It worked well. (see the https://www.youtube.com/watch?v=IH75o5bNm3s)

The problem is that.. the results (mass) of the massFlow function are different at same location, but different surface. i.e.,

< massFlow()@Original surface > are not equal to < massFlow()@User Locations (it is exported surface of the original surface) >

Original surface is just general surface generated in CFD post using Plane feature with Iso Clip. This surface is used to create the csv file that is used as an input file in CFX-Pre to generate "User Location"

Therefore two surface is identical. and scalar value at the surfaces are same such as pressure. But when using massFlow function, results are different as above mentioned it.

Dose anyone know the details of massFlow funtion?

[ghorrocks]

The CFX results file does not include the values at the integration points by default. So if you calculate mass flow in the solver it uses integration point data (and is more accurate), but if you use the results file data in CFD-Post it uses nodal values (and is less accurate).

So there will be a difference between massflows calculated in the solver and post-processing. The difference should be small for an accurate mesh, and should reduce as the mesh is refined. Also, there is an expert parameter to put the integration point data in the results file and this may stop the difference you are seeing.

[Rajaero]

yes i agree with Glenn. it is very difficult to achieve the mass conservation in Ansys. i tried to find out mass for transient analysis but still i got some fluctuation in the mass. i am not sure if it is steady state we may achieve.

[ghorrocks]

Sorry, I did not say it is hard to achieve mass conservation in ANSYS. The difficulty in convergence varies for different simulations - some are hard, some are easy. In general, you will find CFX easier to obtain convergence than many competitor software as the coupled solver is more robust than most of the alternative approaches.

If you are having troubles obtaining convergence see this FAQ: https://www.cfd-online.com/Wiki/Ansy...gence_criteria

[flyply]

I checked it with few more things...

It does not seem to be a mass flow function problem.
at the Ansys document,

massFlow function is defined as
mass = density * velocity dot Normal vector

It is physically right... so I tried to another way, like this

sum( Area * 1.185 [kg m^-3] * (Velocity u * Normal X + Velocity v * Normal Y + Velocity w * Normal Z))@Location

It yields a same values as massFlow()@Location

However, still results are different between User Location and General Plane.
It is almost double...

please, see the attachments