How to plot `turbulent intensity' in Starccm+
 

I would like to plot graph in Starr cmm+ such as velocity magnitude, axial velocity and turbulent intensity.

I have created the plan section in 'derived part'.
Then when I plotted it, there several points (lines) in the graph.

What should I do if I would like to get only 1 line in the graph.

sort the data - go to the properties | data under Plots and sort the data by their Position (X) to plot a nice line.

for turbulent intensity, you need a time series data velocity vs time. with the data, use excel or matlab to compute the mean and standard deviation to find turbulence intensity (std/mean).

Your plots are not visible. Turbulence intensity in an analysis that uses a turbulence model (k-e, k-w, sst, etc...) will be a field function. No need to export and calculate.

Not sure exactly what you are trying to do. You have a derived part (plane) but are plotting points in the plane? Please elaborate.

correct me if wrong.

selecting the RANS equations with the desired turbulence models does give you some field function relating to turbulence (i see Tke, Viscosity Ratio etc). But it does not report on the turbulence intensity. I think one has to export the data and post-process.

I stand (partially) corrected. I assumed intensity was an output, not sure why they don't include it. However, export is definitely not needed.


First, if doing a steady RANS analysis you aren't going to see any turbulent fluctuation a given point in your flow. The assumption of RANS is that turbulence all averages out to zero.


To get turbulence intensity simply setup a field function:
1. Right-Click Tools > Field Functions
2. Select New > Scalar
3. Set Function Name to Turbulence_Intensity.
4. Leave as dimensionless.
5. Set Definition to sqrt(2/3*${TurbulentKineticEnergy})/mag($${Velocity})
7. Rename Field Function to Turbulence Intensity.
8. Now use it like you would any other field function.

http://www.cfd-online.com/Wiki/Turbulence_intensity

I understand what you are saying here.

But Turbulent Intensity by definition, requires a time series. from the time series, one can find the fluctuation and the mean value and thereby compute TI.

Like what you said, if it is a steady case, from the above method, one can get the TI - but it was based on the TKE right at the end of the simulation. It is a steady case because some selected parameter (e.g. velocity) has converged.

But I have some weird thing going on now. I tried to plot the TKE field scene.

I have a steady RANS case which has converged solution - I can see that I have a vorticity field from my vorticity scene and I was expecting to have an obvious TKE field scene.

However, my TKE field scene is showing zero throughout the domain. Any idea what could be wrong?

I shouldn't have said steady. turbulent fluctuations will always average to zero in a RANS analysis. You may still see transient behavior but not random. Not sure why you say that uses TKE is from the end of the simulation. Definitely not the case.

When you say TKE is zero, are you sure its not just really really small? If this is the same problem you were working back when I helped before, you probably won't have terribly huge values of TKE. Can you send me a shot or something?

Sorry for the late reply.

To obtain the graph in 1 lline, I already figured out what I should do.

But for the turbulent intensity, I still do not get your points.

Obviously, my simulation is in the turbulent flow and I also selected the method of K-e and bla bla any related to turbulent.

In fluent, we can get the intensity graph directly ( as I remember)
but in starccm+, there are turbulent kinetic energy, turbulent viscosity , and bla bla
http://s9.postimg.org/hs2ugn92n/turbulent.png

And the point is I want to get the turbulent intensity.
Do you have any idea what should I do?

Still no images. To get a field function (aka variable) that you can plot do exactly as I listed. Its not a defalut field function apparently so you must define it yourself. It's not a big deal. If these step-by-steps aren't clear enough I am not sure I can help you.

"To get turbulence intensity simply setup a field function:
1. Right-Click Tools > Field Functions
2. Select New > Scalar
3. Set Function Name to Turbulence_Intensity.
4. Leave as dimensionless.
5. Set Definition to sqrt(2/3*${TurbulentKineticEnergy})/mag($${Velocity})
7. Rename Field Function to Turbulence Intensity.
8. Now use it like you would any other field function."

I will try to follow your step.

And now I have a problem with the "a request for memory failed this is typically due to insufficient virtual memory" when I am simulating.

I am monitoring the memory during the simulation, and the swap free memory is showing '0'.

The physical properties of my computer are 7 GB of swap and I am using 64 bit of star cmm+ .

Do you have any idea to solve this problem??

Moreover, I am simulating a horizontal pipe (simple simulation) with 12 m length and 0.08 m diameter.

I set 0.08 for base size, 40 for number of prism layer .


Thank you for your kind

That is probably an indication that your mesh is exceeding the capacity of your machine. 7GB isn't a whole lot and will limit you to ~<3.5M poly cells.

40 prism layers is very aggressive too. Sounds like you should reassess your approach for pipe flow. Star-CCM has some cylinder mesh options which will use less memory for a straight pipe.

I should reduce the number of prism layer to get the lower number of meshes.

The option of cylinder mesher, I have already done with this one. The result is quite weird. Then I am trying to use another functions to get the comparison result.

Anyways, Thank you in advance for helping me

Can you post a shot of your mesh or something? It's hard to say, 40 layer may be appropriate but it seems high. The cylinder mesher can be troublesome on occasion. It usualy just means you have something set wrong. Also, make sure you mesh don't mesh in parallel when you have that mesh option activated. It can cause issues.

http://www.cfd-online.com/Forums/<a ...e%20mesh_1.png[/IMG]

I am not sure that you can see the picture or not.

delete pic

This mesh is most likely inappropriate for your problem. Have you solved anything yet or are you still trying to mesh? Two rules of thumb for meshing:

1. Target wall y+ values that are between 1-5 (for near wall treatment) 30-60 (for high wall treatment) or keep between 1 and 60 for all wall y+ treatment. (Actually, for all wall y+ avoid 5-30 range if you can. The values are interpolated between near wall and high wall methods in this range). Should be easy enough for a simple pipe flow.

2. Set number of prism layers and prism layer ratio such that your prism cells more-or-less transition into your core cells without a large change in volume. Right now it looks like you jump about 400% between your last prism and the core mesh. Keep that closer to 20%.

That being said, for your model I would maybe start with 5-7 prism layers. A thickness that is about 1/3 - 1/2 of what you have now and a prism growth rate of 1.3. Mesh, run and look at your y+ values then re-asses your prism layer settings.

No, I am still trying to work with the mesh because when I do the simulation, I always get the memory error.

Tomorrow, I will follow your advise and keep update again. Thank you

:)

Memory error is because your mesh is too aggressive. Try the settings I mentioned, that should get you moving at least.

I did follow what you have said.
Everything works well (Simulation can run).

One more question how do we know what is y+ desired value?

:):):):)

Thank you very much :):)