CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > Siemens > STAR-CCM+

Adding turbulence intensity source in separate region

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   September 3, 2019, 19:05
Post Adding turbulence intensity source in separate region
  #1
New Member
 
Timo H.
Join Date: Sep 2019
Location: Stuttgart - Germany
Posts: 3
Rep Power: 5
Haeussti6 is on a distinguished road
Hello everybody,

I am currently working on a parameter study to determine the influence of turbulence intensity in the field on overall drag and got stuck with the general setup.

I am working with two regions and want to have a turbulence source term in the region two to set the turbulence level back to the same amount I have at the flow inlet of my big flow volume region one.

Region two is only very thin and its only purpose is to make sure turbulence intensity levels behind it are the same like directly after the flow volume inlet. Any other than that I don't want the flow to be influenced by the second region. Therefore I created Internal interfaces with in-place topology to upstream face, downstream face and the sides and set the region type to Fluid too. I set the same value of modified turbulent diffusivity as source term that I have at the inlet (equals a turbulence intensity of 1%). I am running my case with a Spallart-Almaras DES turbulence model.

My problem now is that even though I specify the extra source term in region two, I don't see any change in the flow field. Neither in region two itself nor in the flow field of region one where I actually want the turbulence transported to.

Is there anything I forget to check? How can I get a certain level of turbulence at a specific spot in the field without disturbing the flow?
Any feedback on a approach/idea itself is welcome too.
Attached Images
File Type: jpg Turbulence intensity Screenshot.JPG (57.4 KB, 26 views)
Haeussti6 is offline   Reply With Quote

Old   September 4, 2019, 11:21
Default
  #2
Senior Member
 
Sebastian Engel
Join Date: Jun 2011
Location: Germany
Posts: 566
Rep Power: 19
bluebase will become famous soon enough
Quote:
Originally Posted by Haeussti6 View Post
[...]
I set the same value of modified turbulent diffusivity as source term that I have at the inlet (equals a turbulence intensity of 1%).[...]

My problem now is that even though I specify the extra source term in region two, I don't see any change in the flow field. [...]

Is there anything I forget to check? How can I get a certain level of turbulence at a specific spot in the field without disturbing the flow?
Any feedback on a approach/idea itself is welcome too.
[...]

Hi Timo,
could you state what formula you used as the source term?

How does the field function Modified Diffusivity look like in your simulation? Please share a screen shot. Add a scene for turb. eddy viscosity, too.

Does your source term contain density and time in some way - so, is it a properly defined rate?


You might review the FVM discretization (esp. the general transport equation), which quantity is acutally transported in the SA model (it's the mod. diffusivity), and how RANS models are intersecting the Navier-Stokes equation (with the turbulent eddy viscosity).

Best regards,
Sebastian
bluebase is offline   Reply With Quote

Old   September 5, 2019, 18:07
Post
  #3
New Member
 
Timo H.
Join Date: Sep 2019
Location: Stuttgart - Germany
Posts: 3
Rep Power: 5
Haeussti6 is on a distinguished road
Hi Sebastian,

and thanks a lot for your reply! I should have been more precise - I didn't use a source term but an in built source option to specify the turbulent diffusivity (see thumbnail).
I finally found why it didn't show me any changes behind region two. The modified diffusivity source (MDS) has a different unit than the modified diffusivity (MD) itself. The wanted value of MD that equals a turbulence intensity of 1% has to be multiplied with the mass flow and divided by the cell volume to get the value of MDS that has to be put in the source option of the region. First problem solved! Thanks for the thoughts Sebastian

Nevertheless I am wondering about my conditions at the inlet of the fluid volume after I ran same cases. I define turbulence at the inlet by setting turbulence intensity and length scale in the way that I get a turbulent viscosity ratio (TVR) of 1000 at the inlet (based on the turbulence related equations for SA in the User Guide) My initialization gives me this exact value I want over the whole inlet.
If I check the TVR at the inlet after the computation I get values that are not even close to 1000. I tried it with two different mesh sizes of which the both were smaller than the turbulent length scale I give as an initial and inlet boundary condition. Does Starccm somehow "overwrite" the length scale defined as boundary condition (in my case 0.09m) and replaces it with a value related to the cell length at the inlet? (0.015m and 0.045m - Screenshots)

Thanks in advance for your advices!

Best
Timo
Attached Images
File Type: jpg 01_TVR_inlet_0015.jpg (74.0 KB, 22 views)
File Type: jpg 01_TVR_inlet_0045.jpg (78.3 KB, 20 views)
File Type: jpg 01_TVR_inlet_0045_initial.jpg (26.9 KB, 18 views)
File Type: jpg 01_Object tree.JPG (57.7 KB, 17 views)
Haeussti6 is offline   Reply With Quote

Old   September 6, 2019, 08:29
Default
  #4
Senior Member
 
Sebastian Engel
Join Date: Jun 2011
Location: Germany
Posts: 566
Rep Power: 19
bluebase will become famous soon enough
Quote:
Originally Posted by Haeussti6 View Post
[...]
Nevertheless I am wondering about my conditions at the inlet of the fluid volume after I ran same cases. I define turbulence at the inlet by setting turbulence intensity and length scale in the way that I get a turbulent viscosity ratio (TVR) of 1000 at the inlet (based on the turbulence related equations for SA in the User Guide) My initialization gives me this exact value I want over the whole inlet.
If I check the TVR at the inlet after the computation I get values that are not even close to 1000. I tried it with two different mesh sizes of which the both were smaller than the turbulent length scale I give as an initial and inlet boundary condition. Does Starccm somehow "overwrite" the length scale defined as boundary condition (in my case 0.09m) and replaces it with a value related to the cell length at the inlet? (0.015m and 0.045m - Screenshots)

Thanks in advance for your advices!

Best
Timo


Quote:
Does Starccm somehow "overwrite" the length scale defined as boundary condition (in my case 0.09m) and replaces it with a value related to the cell length at the inlet? (0.015m and 0.045m - Screenshots)
No, a mesh change should not change the boundary condition. You already said you did, but check whether you have set boundary conditions or initial conditions again.
Moreover, the transported quantity is the modified diffusivity(MD) for the SA model. All turbulence bcs therefore should yield a specific MD as boundary value -- which should be constant, if you set a constant value.
So begin to examine the problem with the MD.

The turbulent eddy viscosity (ratio) is a derived quantity.
The manual says: \mu_t = \rho f_{\nu 1} \tilde{\nu}
where f_{\nu 1} is dependend from the kinematic viscosity.
\tilde{\nu} depends on its transport equation which contaitns also kin. viscosity, density, but also the wall distance and the velocity field.
That the turb. viscosity ratio is changing close to the wall is to be expected. You might see in the equations that the MD is damped close to a wall. However, the MD value shouldn't change at the inlet (if it was set constant).
I'd suggest after checking the bc value for MD if any of the quantities the MD depends on is changing instead, such as, is the inlet velocity set correctly, do you have a compressible fluid, then check density/pressure/temperature/.... there might be something set unintentionally wrong.

Anyhow, if you want a specific viscosity ratio, why do you not choose the option to set the viscosity ratio directly? It should be an available turbulence specification.
bluebase is offline   Reply With Quote

Old   September 10, 2019, 23:58
Default
  #5
New Member
 
Timo H.
Join Date: Sep 2019
Location: Stuttgart - Germany
Posts: 3
Rep Power: 5
Haeussti6 is on a distinguished road
Hi Sebastian,
Thank you for your reply and your thoughts. They definitely gave me a better understanding of the turbulence model. I double-checked initial and boundary conditions, which were all the way I wanted them to be.


Quote:
Originally Posted by bluebase View Post
Anyhow, if you want a specific viscosity ratio, why do you not choose the option to set the viscosity ratio directly? It should be an available turbulence specification.

I am using a DES model that uses the Spalart-Allmaras approach to model the turbulence in areas where it doesn’t get resolved. Therefore I am activating the “Synthetic Turbulence Specification” in the inlets Physics conditions that “provides turbulent eddies across inflow boundaries” (UserGuide) and is necessary to get correct results in LES and DES simulations. By using it, I am limited to only one method of defining the turbulence at the inlet – which is turbulence intensity and length scale.

The “box shaped region’s” purpose in the middle of my flow field is it so to add additional turbulence to the field without disturbing other quantities (like velocity, pressure etc.). As I mentioned it earlier, I am using internal in-place interfaces therefore. If I want to add turbulence to this region by using a source option, I again do only get a single choice to define the turbulence. Which is by setting a value for a modified diffusivity (MD) source.



I do get way higher values for MD in my coarser mesh than for my fine one through the whole field, not only at the inlet. Which is generally not surprising because a bigger part of the turbulence doesn’t get resolved anymore due to the mesh quality and more turbulence gets actually modeled by the Spalart-Almaras model. I assume that to be a reason for the lower than initialized values at the inlet. If turbulence gets resolved, it doesn’t need a variable as a quantity for the amount of turbulence anymore.
Maybe that explains why as soon as the simulation starts running the values at the inlet drop down from the set initial value. That the set value is only some static value that changes as soon as the resolving “kicks in” and that it would only retain the initialized value levels if the there was no resolving of turbulence at all and only modeling (a plain RANS model)

This assumption would also explain why the field of turbulence intensity of the coarse and the fine mesh are not too different and at least of the same scale compared to the MD –levels... Anyway that just opens up a whole bunch of more questions to me though…

I am wondering if the defining of a source of modified diffusivity in my “box” area that equals a turbulence intensity of 1% (following Spalart-Allmaras) – does actually really equal an introduction of 1% turbulence to the combined field. If the modified diffusivity does actually get “picked up” or “interpreted” right by the resolving equations after it’s introduced to the flow field. I see way quicker decay of turbulence intensity behind the box region in the fine mesh compared to a small decay in the coarse one (screenshots) - that is why I am confused and wondering.

Again I would appreciate any equation, source or thought that might help enlightening me in this issue

Best
Timo
Haeussti6 is offline   Reply With Quote

Old   September 11, 2019, 10:27
Default
  #6
Senior Member
 
Sebastian Engel
Join Date: Jun 2011
Location: Germany
Posts: 566
Rep Power: 19
bluebase will become famous soon enough
Quote:
DES
That's the imformation i have overread foolishly! Sorry. I then implicitly assumed you were using a plain RANS model.
Though DES is a different story.

In the DES models you have a length scale (or multiple) which are indeed depending on the mesh resolution. To be precise, they depend on the largest distance between cell centers of neighbouring cells. It's too laborious to copy that section from the theory guide.
However, the respective mesh parameter can be found in the function "Detached Eddy Length Scale", . This function is probably changing between different mesh resolutions.
Moreover, this DE length scale modifies the SA model's wall distance. So the modified diffusivity might need to be scaled too.

Quote:
I am wondering if the defining of a source of modified diffusivity in my “box” area that equals a turbulence intensity of 1% (following Spalart-Allmaras) – does actually really equal an introduction of 1% turbulence to the combined field. If the modified diffusivity does actually get “picked up” or “interpreted” right by the resolving equations after it’s introduced to the flow field. I see way quicker decay of turbulence intensity behind the box region in the fine mesh compared to a small decay in the coarse one (screenshots) - that is why I am confused and wondering.
You are probably right, that MD is not really have an impact here, because the turbulence is probably fully blended into the LES formulation here. So the SA model would not have a (large) impact there.

Unfortunately my expertise on LES and DES simulations is small, so far i never have checked on paper how to correlate the synthetic turbulance boundary conditions to RANS boundary conditions, such as the volumetric modified diffusivity source.

I'd need some time playing with the equations, though i won't have that much in the next couple of days. I guess, the starting point for this will be the theory guide, and it's references to understand this turbulence model. How the Reynolds stress tensors are interlinked explicitly. It might become clear then, how to set the boundary conditions to get the desired effect.
bluebase is offline   Reply With Quote

Reply

Tags
interface, regions, source term, turbulence intensity

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
[swak4Foam] Installation Problem with OF 6 version Aurel OpenFOAM Community Contributions 14 November 18, 2020 17:18
Trouble compiling utilities using source-built OpenFOAM Artur OpenFOAM Programming & Development 14 October 29, 2013 11:59
[swak4Foam] build problem swak4Foam OF 2.2.0 mcathela OpenFOAM Community Contributions 14 April 23, 2013 14:59
friction forces icoFoam ofslcm OpenFOAM 3 April 7, 2012 11:57
"parabolicVelocity" in OpenFoam 2.1.0 ? sawyer86 OpenFOAM Running, Solving & CFD 21 February 7, 2012 12:44


All times are GMT -4. The time now is 13:13.