Hi all,

Below is a step by step on how I performed a tracer anlysis of my CFX model. I've spent long hours trying to figure this out! If any of the steps are incorrect or misguided, I would appreciate it if the experts out there could point them out for me.

1) Set up my problem and solve to steady state.

2) Open CFXPre, load same problem and save under different name!

2) Add additional variable, caller "Tracer". Variable Type: Specific, Units: [].

3) Edit all Domains, on fluid models Tab, click "Tracer" onthe additional variables list and Tick the box "Tracer". I did not tick Kinematic Diff, because I do not know the value and don't think it will affect it much (I am adding LiCl as a tracer to thick slurry).

4) Select my inlet and, under Boundary details tab, set additional variables>Tracer>Value to zero. (No LiCl enters through the inlet)

5) Create an expression for the injection of the Tracer: TracerInjection = X * step((t-Y[s])/-1[s]) [kg s^-1] Where X is my input rate in kg/s and Y is the time taken to input the tracer.

6) Create an expression to monitor the output of the tracer TracerOut = areaAve(Tracer)@Outlet

7)Create a source point called TracerIn. Select where I am injecting the tracer as co-ordinates. Under Sources Tab, click Sources, expand Boundary Sources, Click Tracer, Set Option to Total Source and set total source to the expression above "TracerInjection".

8) Define the simulation type as Transient, setting appropriate total time and timesteps.

9)Define the global Initial Conditions under additional variables>Tracer>value to zero.

10) Click "Create Output Files and monitor" button, Monitor Tab>Monitor points and Expressions>add new Item. Set option to expression and set expression to "TracerOut" as defined at (6) above.

11)Save and run solver.

Do I need to set Solver Control>Equation Class Settings > Additional Variable> Advection Scheme or Transient Scheme as ticked?

I have tried it both ways and it doesn't seem to make much of a difference.

Hi,

By doing so you are selecting the Advection and Transient schemes for a particular equation. If you don't do this, the Advection and Transient schemes will be those selected in the main Solver Control window.

Rui

Hi,

I suppose you want to find the transient behaviour of the variable Tracer in a steady flow field. So, when you set up the transient simulation set the Expert Parameter solve fluid to f (false), and when you run the simulation select the steady state .res file as the Initial Values File.

Regards,

Rui

Thanks, that's what I forgot to mention, set expert paramters>model overides> solve fluid to false. I also set turbulence and wall scale to false, is this correct?

I get an output graph that follows the trend I am after, but I don't know what it means.

My bulk fluid flow rate in a 0.1m radius pipe is 10kg/s. My units for the additional variable "tracer" are unspecified, by I inject it from a source point using an equation at 2E-5 kg/s. The equation: areaAve(Tracer)@Outlet, gives me a value of 3.14E-6 (steady state for constant injection of tracer).

Does anyone know what 3.14E-6 means? If it was kg Tracer/kg Total it would be 2E-6 and if it was kg/s tracer in the outflow it would be 2E-5, so where does CFX get this number from?! .

Hallo Graeme,

What do you want to know by this output "TracerOut = areaAve(Tracer)@Outlet " if you need to know the concentration of your tracer, then this is not the right option, for it gives the average area of the tracer in your outlet, and by the way you can also define the dimention of your tracer as in the following example of mine... below you will see how I defined my tracer source and the tracer (as the additional variable)and then as you also did a "SOURCE POINT" for the tracer input and at the end a "MONITOR POINT" to calculate the tracer concentration... I hope this example will help you out... best regards, houman

EXPRESSIONS:

Tracer Source = 0.555*step((t-2350[s])/-1[s]) [g s^-1]

...

END

ADDITIONAL VARIABLE: Tracer

Option = Definition

Tensor Type = SCALAR

Units = [ kg m^-3 ]

Variable Type = Volumetric

END ...

SOURCE POINT: Source Point 1

Cartesian Coordinates = 0 [m], 0.049 [m], 2.47 [m]

Option = Cartesian Coordinates

BULK SOURCES:

Option = Use Volume Fraction

EQUATION SOURCE: Tracer

Option = Total Source

Total Source = Tracer Source

END

END

END ...

MONITOR POINT: Tracer Concentration

Option = Cartesian Coordinates

Cartesian Coordinates = 0 [m], 0 [m], 0.18 [m]

Output Variables List = Water at 25 C.Tracer

END

Thanks Houman,

This method will get me the concentration at a certain point on the outlet, but how do I get the average concentration over the whole outlet?

Hallo Graeme, Now I understand what you are looking for, so in this case your expression "TracerOut = areaAve(Tracer)@Outlet " is correct... but still you can define your tracer dimention as I mentioned in my previous message, so that in your output you get a meaningful result...

regards, houman

Hi, Houman

Have you figured out how to use the averages flow fields as initial condition for tracer simulations?

Could you please introduce your approach? Is the results good?

Regards!

Gab

Thanks again Houman.

I was using a rough mesh to run short models testing what values these end up as. Only when I set Kinnematic Diffusivity to a rediculously high number, did the values actually reach what I was aiming for.

Anyway, it all works now.

Hallo Gab,

Since somthing else came between in my work, therefore I left it away for a while, and didn't try it, but if you have CFX 10.0, then here is the procedure: (I got it from the support):

1. check your def file on which variables you will exactly need for initialisation (velocity components for each fluid, turbulence, volume fractions, ...)

2. define the transient statistics to output all the data fields you need and run the transient calculation

3. export from CFX Post as BC Profile, option: Custom and mark all the averages (e.g. "Velocity.Trnavg X") for export to csv. ... this file is going to be huge ...

4. open the def file in CFX Pre and select Tools/Initialise Profile Data and open the export.csv - the data will then be available as a User Function in CEL, having the name of the Domain the data comes from (e.g. "Fluid") e.g. u can be adressed as child object "Fluid.Velocity.Trnavg X(x,y,z)"

5. open the initialisation panel, choose automatic with value for ALL variables and enter the CEL names of the User Function child objects, e.g. "Fluid.Velocity.Trnavg X(x,y,z)"

6. be sure to freeze the equations by setting solve fluids, turbulence, energy, ... to "f"

Thanks Houman for sharing this procedure. I will try it.

Best regards!

Gab