[shsreekanth]

Hi,
I am using SU2 V2.0.7
1.When the result of turbulent flow over flat plate is opened in ParaView, I see that there are variables "conservative_1","conservative_2"...."conservative _5". What are these variables?
2.Where is velocity? This used to be there with SU2 V2.0.0
3.Which one is density?

Sreekanth

[economon]

Hi Sreekanth,

The conservative variables for the governing flow equations (Euler, N-S, RANS) are the mass, momentum, and energy, i.e. U = ( density, density*velocity, density*energy)^T. Therefore, the density is the first conservative variable, and in order to get the velocity, you should divide the momentum components by the density. In 2-D, for example, the x-velocity would then be vel_x = Conservative_2/Conservative_1.

Cheers,
Tom

[shsreekanth]

Hi,
Based on the above explanation , I would have 4 conservatives for a 2D problem and 5 for 3D problem.
I did a 2D problem in SU2 with Physical_problem = Navier stokes and KIND_TURB_MODEL= SA
I get 5 conservative variables .
If its a 3D problem, I get 6 conservatives. Which is the extra conservative variable calculated?

[liujmljm]

Originally Posted by shsreekanth

Hi,
Based on the above explanation , I would have 4 conservatives for a 2D problem and 5 for 3D problem.
I did a 2D problem in SU2 with Physical_problem = Navier stokes and KIND_TURB_MODEL= SA
I get 5 conservative variables .
If its a 3D problem, I get 6 conservatives. Which is the extra conservative variable calculated?

Dear, I suggest u should read some books on Fluid dynamics or CFD.
The extra conservative variable is eddy-viscosity variable in SA turbulent model.

Merry Xmas and happy new year.

Good Luck

[shsreekanth]

Thanks
Merry X'mas and Happy new year

[Nielson2]

Hi all,

I would like to continue this thread, if I may, with a question with regard to the conservation variables.

Sreekanth mentioned that the velocity parameter has disappeared in version 3.0, while it was there in the second version. I noticed the same, which I found quite a shame. The transition also changed the output parameters of flow.vtk files. With v2.0 flow.vtk files, I was able to visualize the direction of flow or velocity with the usage of glyphs in Paraview. I haven't found a way to achieve the same with v3.0 flow.vtk files. Does anybody know how I can achieve this?

Moreover, the v3.0 flow.vtk files also seem to miss the streamline functionability in Paraview.

Do I have to convert the flow.vtk files to be able to use this functions? If yes, how can I do this?

Thanks in advance!

Niels

[shsreekanth]

Hi,

To get the velocity vector , you have to use the filter 'calculator' in paraview. For 3D, the new variable should be "conservative2"/"conservative1"*iHat+"conservative3"/"conservative1"*jHat + "conservative4"/"conservative1"*kHat. This will give velocity vector (u,v,w) . After that, you can apply streamlines

I hope this is what you asked about.

Sreekanth

[JinZhiyi]

Originally Posted by liujmljm

dear, i suggest u should read some books on fluid dynamics or cfd.
The extra conservative variable is eddy-viscosity variable in sa turbulent model.

Merry xmas and happy new year.

Good luck

大哥您可是真犀利｀｀｀

[Nielson2]

Originally Posted by shsreekanth

Hi,

To get the velocity vector , you have to use the filter 'calculator' in paraview. For 3D, the new variable should be "conservative2"/"conservative1"*iHat+"conservative3"/"conservative1"*jHat + "conservative4"/"conservative1"*kHat. This will give velocity vector (u,v,w) . After that, you can apply streamlines

I hope this is what you asked about.

Sreekanth

Thanks! That was indeed what I was looking for!

[shsreekanth]

Hi,

Also, all these variables are scaled. So to get the actual value of velocity, you must multiply it with the value of reference velocity.

[novedevon]

I've just run the RANS Onera wing and trying to understand the resultant data. So I understand that the first 4 conservatives are [\rho, \rho u, \rho v, \rho w] and the last two represent energy. What type of energy? Whats the difference? Does turbulence come into it? I wasn't able to find specifics in the documentation.

From FAQ:
"For example, in the RANS solver additional turbulent terms are needed"

[hlk]

Originally Posted by novedevon

I've just run the RANS Onera wing and trying to understand the resultant data. So I understand that the first 4 conservatives are [\rho, \rho u, \rho v, \rho w] and the last two represent energy. What type of energy? Whats the difference? Does turbulence come into it? I wasn't able to find specifics in the documentation.

From FAQ:
"For example, in the RANS solver additional turbulent terms are needed"

The first n+2 equations come from the basic conservation equations - one for mass, n (2 or 3) for momentum and one for energy. In the one-equation SA turbulence model there is one additional variable. In the two-equation SST turbulence model there are two additional variables. CFD-online maintains a good wiki explaining the variables involved in these turbulence models:
http://www.cfd-online.com/Wiki/Spalart-Allmaras_model
http://www.cfd-online.com/Wiki/SST_k-omega_model

[beatlejuice]

Hi have also a questions regarding the conservative variables and the residuals (res[0], res[1],...):

I have a 2D, unsteady (compressible), RANS (SA) case where I have a problematic behaviour of res[3]. My res[4] is always zero, so i guess this must be the momentum residual for z-direction.

From the SU2-FAQ and this previous conversation, i know that:

conservative1 = density; (mass conservation)
conservative2, conservative3, conservative4 = x,y,z-momentum; (mom. conservation)
conservative5 = energy (e. conservation)
and the eddy viscosity

So the intuitive thought would be:
res[0} = density residual ???
res[1}, res[2}, res[3}= x,y,z-momentum residual ???
res[4} = residual of energy conservation ?????
resturb[0} = must be eddy visc.

But this doesn't make sense to my first conclusion that my residual res[4] , which is always zero must be for z-momentum. And also that i would have a non-zero residual for z-momentum, if res[3] would be the residual for z-momentum.

So, my question is:
which residual (res[0], res[1],...) corresponds to which quantity? I was not able to find any hint in the web....please help =)

[hlk]

Originally Posted by beatlejuice

Hi have also a questions regarding the conservative variables and the residuals (res[0], res[1],...):

I have a 2D, unsteady (compressible), RANS (SA) case where I have a problematic behaviour of res[3]. My res[4] is always zero, so i guess this must be the momentum residual for z-direction.

From the SU2-FAQ and this previous conversation, i know that:

conservative1 = density; (mass conservation)
conservative2, conservative3, conservative4 = x,y,z-momentum; (mom. conservation)
conservative5 = energy (e. conservation)
and the eddy viscosity

So the intuitive thought would be:
res[0} = density residual ???
res[1}, res[2}, res[3}= x,y,z-momentum residual ???
res[4} = residual of energy conservation ?????
resturb[0} = must be eddy visc.

But this doesn't make sense to my first conclusion that my residual res[4] , which is always zero must be for z-momentum. And also that i would have a non-zero residual for z-momentum, if res[3] would be the residual for z-momentum.

So, my question is:
which residual (res[0], res[1],...) corresponds to which quantity? I was not able to find any hint in the web....please help =)

Thank you for your question
I believe what is going on here is that, probably for code simplicity/efficiency, the four residuals from the 2-dimensional problem are output into the first four columns, with the extraneous column left as zero.
This means that res[0] is the density, in the two-D case res[1-2] are the momentum residuals, and res[3] is the energy residual. For the 3-D case it would be res[1-3] for momentum and res[4] for energy.
Sorry that this is not clearer - the output code is abstracted to avoid repeated code for different physical problems, and as a consequence includes less problem-specific detail in some parts of the output, including this portion as you note being vague as to which residual is associated with which variable. Thank you for posting, this feedback can help inform future code updates.

[beatlejuice]

Thank you very much!

[EAS105]

First post here. Since retiring at the end of 2014 I've been playing around with an aircraft design I made as a project to graduate in 1984. I've had the idea in the back of my head for some 30 years. I started as an engineer in manufacturing industry, but got placed in financial and personnel management, so I never really got to pursue or keep up with technical advances in the field of aircraft design.

The intention has been to convert this design to a virtual aircraft for a flight simulator. My design is a bit unorthodox, being a three-surface with supercritical airfoils. I had no real data, and usual methods of analysis to find various stability derivatives were not quite satisfactory for me. I wanted to see if new computer tools could give me a better idea of how the design would behave.

I had to relearn a lot of things, and now in process of learning a lot of new things. Among those, is use of SU2 and Paraview. Being on retirement budget now, I like the open-source software. When I graduated, none of these tools were available. I began with 2D paper drawings, and a stack of saved reports, calculations, charts, graphs, etc.

All that said, I wanted to view streamlines around the aircraft. I've run this thing in a multitude of iterative configurations over the last several months. The virtual wind tunnel streamlines had confounded me for quite some time, and I wanted to see them over the wing surface at various angles-of-attack and Mach numbers.

Finally found this thread, and the wonderful solution in post#7 above has made yet another facet of this project realized. Thank you.
Here are a couple of screen shots I made from an earlier and simpler configuration just today. I used a lower resolution mesh to see if this would work for me. As you can see, I got a nice result.

Stream1 (Small)2.jpg

Stream2 (Small).jpg

[dwstevens]

Originally Posted by economon

Hi Sreekanth,

The conservative variables for the governing flow equations (Euler, N-S, RANS) are the mass, momentum, and energy, i.e. U = ( density, density*velocity, density*energy)^T. Therefore, the density is the first conservative variable, and in order to get the velocity, you should divide the momentum components by the density. In 2-D, for example, the x-velocity would then be vel_x = Conservative_2/Conservative_1.

Cheers,
Tom

Tom and others,


I am currently reading "CFD" by John D.. Anderson and performing some basic compressible flow simulations using Su2. It seems Su2 has changed the format of the output quantities shown in Paraview etc... One can now see density, x-momentum etc... Anyway as Tom stated you can calculate Vx = x-momentum/density using the calculator function. However this is a bit counter intuitive to me as I normally think of momentum being expressed in [MLT^-1] units. I you divide this by density [ML^-3] you obtain [L^4T^-1] which is certainly is not velocity. From the above it appears Tom is referring to momentum in as (velocity*density) I am assuming this is from the conservation form of the momentum equation d(rho*u)/dt + Divergence * (rho*u*V). Can anyone help me connect the dots here?


Appreciated,


David

[wallym]

Hi David,

The form of the conservation equation you wrote is correct. An your intuition is correct, (rho*u) isn't physically momentum as we normally see it.
Explaining the confusion: we see in the time dependent term exists (rho*u). This is the conservative variable in question. Jumping further, the second term is actually Divergence*Flux of (rho*u). I find this link useful:https://web.stanford.edu/group/frg/c...AA214B-Ch2.pdf

Hope this helps,
Wally