[michellemay1993]

Hi,

Can I know how the mass flow rate vs time chart is plotted in CFX Post?

[urosgrivc]

When in post:

[1] insert a new chart than set

[2 ]XY- transient or sequence

- go to data series tab

[3] set an expression: right click in the window _functions _cfd post
chose mass flow()@your location

That is it

Your location can be an already existing surface or you can make a new plane where you want to measure it in your domain.

-It can take a wery long time to calculate the graph if your mesh is fine and you have a lot of timesteps (it will calculate variables at every timestep).
That is why I prefer to export time dependant data from the monitor points that
you are able to set in pre before solving (almost instant export)

There is a lot of other powerfull capabilities in the chart settings.
You are able to pres export on the bottom this will create (.csv) file
that you can open in excel.
You will need to use the data function in excel to get your data into multiple coloumns
->IF<- the numbers are wery huge you will have to divide them in excel by a factor 1000 000 00.
I have no idea Why If someone has please let me know.

[michellemay1993]

Should I set any variable in Y axis?

[urosgrivc]

no just leave it

x will be time and y will be mass flow or your epression value

[michellemay1993]

After apply the chart, there is a warning window pop up. It says:
Unable to calculate mass flow for the surface. Some or all of the require variables are not present: Density; Velocity; and for multi-phase cases, Volume Fraction.

What should I do?

[urosgrivc]

I dont know what you are modeling, more data will be needed.
-Did you simulate water and air or something like that, if so
than you need to specify mass flow of what component in the expresssion also,
-It is also posible that you did not save variables at each timestep or you have set to save to litle wariables at each timestep.

[michellemay1993]

It's a nozzle diffuser pump. Opening bc with 0kPa relative pressure inlet and outlet.

[urosgrivc]

so you have multiphase simulation.
http://148.204.81.206/Ansys/150/ANSY...ce%20Guide.pdf

for multiphase expressions PAGE 232

[michellemay1993]

No it's single phase (water)... In the CFX Pre, density should be selected in the trn result output variable list?

[urosgrivc]

If you leave the trn result output at default that should be sufficient
but these must be exported at each timestep.

[michellemay1993]

I selected the density and velocity normal to surface and rerun the solution. It works now!!! Thank you very much urosgrivc