Learning Forum

[tubiy]

Hi,

I want to plot  Mass Flow Rate vs Time in a specific plane.

The specific plane defined during the Meshing process

A special emphasis is that I already calculated my simulation and saved data any 10sec.

I know that there is an option to make file report before running the simulation and so but it's not relevant now.

 

I try 2 ways:

1. Through Fluent Results-->XY plot but there is no option to define the X-axis as Time.

2. Through Results-->location-->creat plan-->Chart. The problem is when I tried to choose this plane in the locations tag the plane not exist.

I attached pictures for option 2 (the gray plane is the plane that I made).  

 

I will be very glad if someone can help me with this. It's a very basic thing so I am sure there is an easy way to do this.

Thanks,

Tubi

[DrAmine]

You need to define that as report and enable report-plot. You can then see that during the run and read it back as file plot.

[tubiy]

Hi Amine,

I know that I can do it like this, but as I mentioned I already have the simulation results.

The simulation ran for about a month, so it's not relevant for me to run it again from the beginning.

I hoped there was another way to create this plot, you have another way?

Thanks.

[DrAmine]

If you have a couple intermediate data you can do that in easy way in CFD-Post. Do you have transient intermediate data files?

[tubiy]

 yes, I have. 

I saved data any 5 seconds through Autosave Dialog Box.

I succeed to create a point and plot Temperature/ Velocity vs Time in  CFD-Post at a specific point by using

chart -->XY - Transient or Sequence.

But If I'm not mistaken it's impossible to use "XY - Transient or Sequence"  for a surface, it's just for a point,

and I didn't find any way to make a plot of average temperature or Mass Flow Rate that requires a surface.

What the process for this?

 

Best regards,

 

Tubi.

 

'

[DrAmine]

For a surface you need to create an expression where you define area average for example of temperature and then use that expression for the transient chart.

For mass flow rate just use massflow()@your surface for your expression.

 

 

[tubiy]

 

I tried to define the  expression as you suggest but it always gave me an error, I tried to change the name of the surface or to

create a new surface at CFD-Post (plane 2) but it does not work out (I've attached a picture of the error)

I defined the expression according to Anays manual.

Can you explain to me where I'm wrong? Or write down the exact Syntax?

The name of my surface as it is defined in FLUENT is:

"interior-hot_pipe_outlet(id=16)" 

and for example, I want the average of the temperature on the surface.

 

Best regards,

Tubi.

 

[DrAmine]

You need to use the available surfaces and planes in CFD Post. Best to RMB within the expressions and select the locators from that menu.

[tubiy]

Thanks now it works.
I will just add to those who don't know, that the expression is case sensitive. so when I defined the mass 
flow expression it was like this:

massFlow()@location

 

Best regards,

Tubi.

 

[LinjoRejoy]

Is it possible to plot this expression, massFlow()@Location with timesteps as x axis. I have already done the transient flow analysis.

Thanks in advance

Linjo

[DrAmine]

yes pos

[DrAmine]

Yes just add a transient chart.