CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (https://www.cfd-online.com/Forums/openfoam-solving/)
-   -   How to calculate y-plus? (https://www.cfd-online.com/Forums/openfoam-solving/116358-how-calculate-y-plus.html)

rogerliu April 17, 2013 15:11

How to calculate y-plus?
 
My case is unsteady flow past a cylinder using LES. Re=3900
How can I calculate the y-plus?
does y-plus refer the distance from the first grid to the wall? Is it the smaller, the better?

Thanks!

immortality April 17, 2013 18:41

hi
Type yPlusRAS or yPlusLES
If you have ras or les turbulency.

fredo490 April 18, 2013 05:21

Hello, y+ refers to the size of the mesh next to the wall compared to the fluid behavior. This number helps you to know where is your first cell center compared to the boundary layer thickness.

If you didn't study any boundary layer theory, you have to know that a boundary layer is composed of different parts. The one very close to the wall is dominated by viscous effects (= the viscous layer) and a bit outer you have the log layer.

To get an accurate simulation, your first cell center must be inside the viscous layer. We usually consider that a y+ smaller than 4 is required. Ideally, you should have a y+ smaller than 1 on all your surface. But there is no need to go to 1e-3 !

Be careful, the size of your first cell must correspond to your turbulence model. For example a RAS k-omega SST requires a y+ smaller than 1 but a k-epsilon standard requires a y+ between 30 and 60. I don't know about LES simulation but I guess it should be smaller than 1.

To get the yPlus, you can only do it as a post treatment (because you need to compute the velocity first). To get it, simply type "yPlusRas" or "yPlusLes" depending of your turbulence model. You can also write "yPlusLes -h" to get some help.

For example: yPlusRas -latestTime -compressible will only compute the yplus for your last export and it will apply a compressible correction (only use it with a compressible solver).

To get a rough estimation of the cell size you need next to the wall, you can use this tool:
http://www.cfd-online.com/Tools/yplus.php

immortality April 18, 2013 07:49

I wonder how we can calculate y+ at a laminar flow without any turbulent model? is it possible?

fredo490 April 18, 2013 08:01

At first the y+ has nothing to do with CFD but it has to do with the boundary layer theory (this number was created in the 1930's). The definition is here : http://www.cfd-online.com/Wiki/Dimen...stance_(y_plus)

Yes this number has a meaning for a laminar flow but we don't really care for CFD cases. It is mainly used for turbulent flow because the models we use are based on some assumptions that need to be verified.

VSass July 1, 2013 10:34

I have some problems calculating y+ during a compressible flow. I use Spalart-Allmaras model and the output in the results files is mut, not nut, which is prerequisite for the calculation of y+. Any ideas?

immortality July 1, 2013 10:44

hi
search this site.there are some good threads with y+ for compressible flows.
do you use low-Re or high-Re?

VSass July 1, 2013 11:15

I use high Re.

immortality July 1, 2013 12:18

then use yPlusRAS -compressible its for high-Re models Vasilios.

VSass July 1, 2013 13:10

I use yPlusRAS but it needs the "nut" values for each time step. My solution outputs "mut" files. That's the problem.

immortality July 1, 2013 13:21

type: "yPlusRAS -compressible" not only yPlusRAS

VSass July 1, 2013 13:25

Honestly,thanks!

VSass July 3, 2013 06:27

Well, using yPlusRAS -compressible works, but it plots a value of "0" in the field. Mut has an accepted distribution , but how come the distribution of yPlus is zero?

immortality July 3, 2013 09:23

where in the field? whats your case? if its something like shockTube maybe the flow has not reached there.

caoyinyue February 26, 2014 22:23

Quote:

Originally Posted by VSass (Post 437506)
Well, using yPlusRAS -compressible works, but it plots a value of "0" in the field. Mut has an accepted distribution , but how come the distribution of yPlus is zero?

Hello, I used the yPlusLES for calculating the incompressible flow field. the distribution of yplus is alos zero. It is very strange. Have you found any solution? Could you give me some hint? Thanks very much

Alhasan January 8, 2015 13:28

Quote:

Originally Posted by fredo490 (Post 421448)
Hello, y+ refers to the size of the mesh next to the wall compared to the fluid behavior. This number helps you to know where is your first cell center compared to the boundary layer thickness.

Hello FOAMers and Frédéric,

Edit: Continuation from http://www.cfd-online.com/Forums/ope...provement.html

Please correct me if I am wrong

From reading all the posts my understanding of y+ is that we have an approximate estimation using the online calculators and once the simulation is done using the estimated y for the required y+ we use the Existing OpenFOAM utilities to calculate the actual y+ values am I right ?

I have used the online tools to estimate my Y distance for a required y+ value of 30. Then after running my simulations the openFOAM utilities say that my y+ value is 12. so Now I believe to get much accurate flow behaviour close to the wall I have to change the size of the y again !!!.

I have completed my simulation and OpenFOAM says my y+ value is 12 and I want it to be 30. My question is how do i determine the size of my first cell that is my Y distance now !.

And also my Y distance should be varying around my geometry right ? since flow behaves differently and Y+ value after the simulation is different all around the airfoil how do I determine the Y distances for different regions.

Thanks a lot for your time and reply,

Regards,
Hasan K.J

petr.f. January 8, 2015 16:54

Quote:

Originally Posted by Alhasan (Post 526625)
From reading all the posts my understanding of y+ is that we have an approximate estimation using the online calculators and once the simulation is done using the estimated y for the required y+ we use the Existing OpenFOAM utilities to calculate the actual y+ values am I right ?

- Yes, that's the usual way. At first you have to decide what level of precision in turbulence modelling in boundary layer do you need (nice overview: http://www.bakker.org/dartmouth06/engs150/11-bl.pdf).

Quote:

I have used the online tools to estimate my Y distance for a required y+ value of 30. Then after running my simulations the openFOAM utilities say that my y+ value is 12. so Now I believe to get much accurate flow behaviour close to the wall I have to change the size of the y again !!!.
- Not necessarily. It is true, that the simulation with y+ - 12 is more accurate than the one with y+ = 30, but in both cases you already don't capture behaviour in the viscous sublayer, you have to use the wall functions approach and hence model the buffer layer (at best). So the overall level of precision is the same. What differs is the refinement level of computational mesh (and the total number of cells). If you want shorter computational times then yes - re-mesh the case.

Quote:

I have completed my simulation and OpenFOAM says my y+ value is 12 and I want it to be 30. My question is how do i determine the size of my first cell that is my Y distance now !.
- what y+ is 12? The minimal or the average?

Quote:

And also my y+ should be varying around my geometry right ? since flow behaves differently how do I determine the y distances for different regions.
- usually you set your minimal y+ to the desired value for the largest cells in your "critical" region (e.g. the one with separation or highest velocity...) so you are estimating y+ for the "worst" case.

P.

Alhasan January 8, 2015 17:17

2 Attachment(s)
Hey Petr,

Thanks for your reply,

Let me explain what I am trying to do so you will get a better idea of what is happening I have described it in a different post here: http://www.cfd-online.com/Forums/ope...provement.html

on short note im just simulating a NACA 0012 airfoil

Quote:

Originally Posted by petr.f. (Post 526655)
- what y+ is 12? The minimal or the average?

Code:

Patch 0 named CURV1 y+ : min: 0 max: 12.6672 average: 4.48469
I had calculated using the online Y+ estimator that for a Y+ of 30 the Y distance was 0.00033 meters for my case and I had meshed with 0.00033 as my first cell height around my airfoil using ICEM. I wanted Y+ as 30 since I wanted to use the wall functions and I have used wall functions for my simulation using KW-SST.

I have also attached an image of the Y+ and Y* distribution on the upper and lower surface of the Airfoil. I have used one of the altered yPlus utilities on the forums to find my y+ values as the existing yPlusRANS supposedly calculates y*.

I got into this Y+ checking because of the results I was getting was not great as shown in the other post I have provided link above.

- So my question is To be accurate should I have a Y+ of 30 (using WF) around the airfoil equally If yes, How will I calculate the Y distance needed for every region.

Thanks,
Hasan K.J

petr.f. January 8, 2015 18:15

1 Attachment(s)
Hi Hasan,

you don't have to generate the mesh so that your y+ is 30 all over the profile. Actually I don't think that's even possible. From your simulations you already know the maximal velocity on the profile. I would use it for new delta s estimate for desired y+ and generate the mesh with y+ = 30 in this region (so it will be smaller in other areas).

However, after reading your other post I have two questions:
- what are your boundary conditions for k and omega on the profile (slip wall) in the no-WF simulations?
- what is the topology of your mesh (H mesh, C mesh, O mesh) ? 200000 cells for 2D case is quite a lot. For your purpose I would go for a C-mesh with ~ 50000 cells (and that's with y+ = 1), like the one in the attached picture. Such a mesh you can get easily from Tecplot (if you have the license, not sure if they still offer time-limited demo) or Gridpro (the academic license used to be free) or with a little effort from cMesh or "simple simple airfoil mesher" - http://www.cfd-online.com/Forums/ope...-aerofoil.html

P.

Alhasan January 8, 2015 18:35

1 Attachment(s)
Hi Petr,

Thanks for you reply,

Quote:

Originally Posted by petr.f. (Post 526667)
I would use it for new delta s estimate for desired y+ and generate the mesh with y+ = 30 in this region (so it will be smaller in other areas).

- What do you mean by delta s estimate ? you mean to say I have to use the new velocity to get the y distance estimate using the online calculators

Quote:

Originally Posted by petr.f. (Post 526667)
- what are your boundary conditions for k and omega on the profile (slip wall) in the no-WF simulations?

I have used fixed value on the airfoil surface wall with no slip
Code:

    {
        type            fixedValue;
        value          uniform 1e-11;
    }

Quote:

Originally Posted by petr.f. (Post 526667)
what is the topology of your mesh ?

You are absolutely right 200,000 quite a lot but since I had good computation power just stuck to it how ever I had done a mesh dependency test with approximately 8 cases with no elements varying from 50,000 to 800,000.

Edit: I think my 200,000 is only as good as your 50,000 as my domain is big !!

I have used a C mesh and I have used ICEM and I have grown quite comfortable with that software as you can control the mesh very well with that software and I do have license for techplot360.

However I am interested in your meshing topology does it come under C-Mesh..? and isn't the outlet very close to the airfoil My domain is massive just to avoid any BC problems as suggested in the literature I have 10c above and 10 c below my geometry and 20c behind my airfoil as shown in the image, the mesh look ridiculously dense it is not its just paraFoam showing it like that.

I did go with the y+ of 1 for all my Mesh dependancy cases like u had suggested but the results were not promising but the result with WF looks some what reasonable and I am hoping for better results after the Y+ correction

Regards,
Hasan K.J

petr.f. January 9, 2015 07:54

Quote:

Originally Posted by Alhasan (Post 526669)
Hi Petr,
- What do you mean by delta s estimate ? you mean to say I have to use the new velocity to get the y distance estimate using the online calculators

- yes, exactly. I'm ususally using the Pointwise Y+ Calucator (http://www.pointwise.com/yplus/) where the distance of the first cell from wall is denoted as delta s.

Quote:

I have used fixed value on the airfoil surface wall with no slip ...
- no-slip, of course, my bad. As for the boundary conditions for the y+ = 1 case: k_wall = 0, and since omega = O(y^-2) (where y is distance to the wall) in the vicinity of the wall you should use some analytical estimate. One of possible approaches is to set

omega_wall = Const * nu / (beta * y^2)

where beta = 0.075, nu is kinematic viscosity, y is distance between the wall and centre of gravity of the first cell and Const = 6 (but you can try Const = 9 as well).

About the mesh - your domain is really big, IMHO too much. You're dealing with simple incompressible flow, so there will be no shock-waves and the flow should be quite "nice". 10 c in front of, above and below the aerofoil is OK, as for behind - 7c is quite enough (in some cases even 5c is ok). My mesh is indeed a C-mesh (although multiblock, which produces those two mesh density lines behind the aerofoil). Even if you have a good computation power the fact is that all your simulations can be ~4 times faster, I wouldn't hesitate ;)

P.

Alhasan January 9, 2015 09:34

Hi Petr,

Thanks for your Reply,

Quote:

Originally Posted by petr.f. (Post 526737)
-
omega_wall = Const * nu / (beta * y^2)

where beta = 0.075, nu is kinematic viscosity, y is distance between the wall and centre of gravity of the first cell and Const = 6 (but you can try Const = 9 as well).

so you mean to say I have to use Omega_wall = 9*1.5e-5/(0.075*0.00033^2) = 16528.9

Where Y = 0.00033 the existing value just to make the point clear

(by any chance do u have any reference for this as I am coming across it for the first time)

so for omega boundary condition
Code:

Airfoil
{
        type            fixedValue;
        value          uniform 16529;
    }

So what omega value do I use for the inlet boundary condition I am currently using the below which was calculated using the http://www.cfd-online.com/Wiki/Turbu...ary_conditions
equations for omega

Code:

TOP
    {
        type            turbulentMixingLengthFrequencyInlet;
        mixingLength    0.022;
        value          uniform 9.4512;
    }

Thanks for your opinion about the domain I think I will reduce domain size to 10c behind airfoil as well as there is lot of URANS simulations pending

Regards,
Hasan K.J

petr.f. January 9, 2015 10:28

Hi Hasan,

the relation for omega comes from omega transport equation by Wilcox (Wilcox D. C.: Reassesment of the scale-determining equation for advanced turbulence models, AIAA J., 26, 1299-1310, (1988)), which (near the wall) can be reduced to

mu * d^2 omega/d y^2 - betta * rho * omega^2 = 0 (1)

Solution of (1) is the mentioned relation for omega. As for the inlet - I'm using the same equations you've referred to but combined with the fixedValue BC (but of course, both ways are possible).

P.

Alhasan January 9, 2015 12:16

Hi Petr,

Thanks for the reference I will go through it in detail,

So for the wall is the boundary condition on my previous post looks reasonable enough for the omega ?

because I have never used the equation before I feel that the value is massive but I will have to do the simulations to see what happens but since you have a very good understanding and previous experience I would go with your word, if that is the type of value we are looking at for omega at airfoil wall.

Regards,
Hasan

Alhasan January 12, 2015 12:30

Quote:

Originally Posted by petr.f. (Post 526737)
- yes, exactly. I'm ususally using the Pointwise Y+ Calucator (http://www.pointwise.com/yplus/) where the distance of the first cell from wall is denoted as delta s.

Hello Petr,

Even using the Local velocity to find the Y distance using the online calculators gives me a wrong Y+ value when i check the Y+ after the simulations and I am aware openFOAM finds the Y* and I am using an altered yPlus utility to cacluate the Y+ after the simulation what could I do find the right Y distance for a Y+ of 30 any advice.

Kinds Regards,
Hasan K.J

petr.f. January 12, 2015 12:51

Hi Hassan,

what values of y+ did you get during the last simulation?

What I've advised should lead to y+ <= 30 (not y+ = 30 all over the profile).

Btw, what values of k and omega do you set on the inlet?

Regards, P.

Alhasan January 12, 2015 15:04

Hi Petr,

I am not trying for Y+ all over the the profile only for some regions and My max Y+ is not going above 12 I was hoping at least my Max Y+ will go above 30 my main aim was to get an average Y+ of 30 when I run the utility,

The K and W are the values I calculated using CFD wiki at the inlet, K =0.0216 and W = 9.45 at the inlet. and I am using wall functions as it is giving better results

Just came across this page:http://www.cfd-online.com/Forums/ope...lus-field.html
thinking might be of somehelp but dont know

Kind Regards,
Hasan K.J

petr.f. January 14, 2015 17:33

Hi Hasan,

that seems quite good. I'd be interester in the results you achieve with this utility.

I've checked once more the schemes you are using and I'd give a try to the following settings:

gradSchemes
default cellLimited Gauss linear 1.0;

divSchemes
div(phi,U) bounded Gauss linearUpwindV grad(U);
div(phi,k) bounded Gauss linearUpwind grad(k);
div(phi,omega) bounded Gauss linearUpwind grad(omega);

laplacianSchemes
default Gauss linear corrected;

snGradSchemes
default corrected

according to http://www.dicat.unige.it/guerrero/o...sandtricks.pdf
and http://sourceforge.net/projects/open...k.tar/download

Should there be convergence problems of turbulent quantities start with simple 1st order upwind and after e.g. 200 iteration switch to 2nd order upwind as is written above.

Then to speed-up the convergence a bit you can try pre-conditioned version of GaussSeidel, that's DICGaussSeidel for p and DILUGaussSeidel for the rest (U,k,omega).

Alhasan January 14, 2015 18:05

Hi Petr,

Thanks a lot for your reply,

Yes It is an awesome Utility those people have written, I makes a lot of job so much simpler. However It did not aid me much with my problem.

Infact I have been using that tips and tricks for sometime now It is a very good link. I have tried the schemes long ago on the same case and they don't give the changes we are expecting !!

However I have figured out the actual problem
The problem was clearly with the mesh and the first cell height.

How i figured out was but just taking a linear relationship between the Y+ i was getting from OpenFOAM to get the Y+ that i needed.

finally I had changed the first cell size to 0.0011m in the meshing software. (which is basically a random value i got with some linear relationship)

But when I converted the mesh to OpenFOAM and checked the Y+ using the online utilities this was the result I got
Code:

d  : min: 0.000143678 max: 0.000573121 average: 0.000463817
 uTau: min: 0.368982 max: 1.61318 average: 1.03683
 y+  : min: 11.9173 max: 35.9611 average: 30.8851

And also the boundary layer problem I had with the results were sorted in the results with this mesh.

But the funny Problem I am having now is when I assign a first cell height of 0.0011m in my meshing software I donot know why I am getting 0.00057 when the utility calculates the first cell distance in openFOAM. I am getting the correct results only when the Utility says my Y+ is 30.

I just have to figure out why this is happening If not just have to play with first cell height every single time :( :(. By any chance do you know how to check the distance between two points in ParaView

And if at all you have time please have a look at this post
http://www.cfd-online.com/Forums/ope...tml#post527629
Thanks a lot for all your replies and time.
Hasan K.J

petr.f. January 15, 2015 10:37

Hi Hasan,

my experience with ICEM is limited - I was using it 4 years ago for 3D tetra meshing...

However, for measuring distance of two points in Paraview you can use the ruler tool (with 2D option in the layout window on). As far as I know Paraview doesn't snap to points with ruler, but if you zoom close enough you'll get reasonable value...

P.

Alhasan January 15, 2015 13:18

Hi Petr,

There is no problem with mesh conversion from ICEM to openFOAM since the ruler option reads the same distance of first cell in paraView that I have used in ICEM. so this option is out I think it id just the yPlus utility takes someother factors into consideration and calculates Y as the value it gives and It appears to be 1/2 of the actual first cell distance so it does make some sense

Thanks again :)
Hasan K.J

Blanco February 1, 2015 05:52

Quote:

Originally Posted by Alhasan (Post 527668)
I think it id just the yPlus utility takes someother factors into consideration and calculates Y as the value it gives and It appears to be 1/2 of the actual first cell distance so it does make some sense

Thanks again :)
Hasan K.J

I'll give my two cents on this problem.

I know this may looks like an obvious observation but...have you considered that "y" in the y+ formula is NOT the first near-wall cell height? It is the first near-wall cell CENTROID height indeed, which is half of the cell height for a prism cell. This because in finite volume methods (as in OF) we refer to cell centroids and not to cell vertex as in finite-element methods. I suppose that's why you have that mismatch...I've never had this kind of mismatch in my sim, y+ was correctly calculated by OF. I've tested also on ICEM mesh converted to OF format.

Best,

Andrea

Alhasan February 1, 2015 08:26

Quote:

Originally Posted by Blanco (Post 529870)

"y" in the y+ formula is NOT the first near-wall cell height? It is the first near-wall cell CENTROID height indeed, which is half of the cell height for a prism cell. This because in finite volume methods (as in OF) we refer to cell centroids and not to cell vertex as in finite-element methods. I suppose that's why you have that mismatch...

Hey Andrea,

Thanks for your reply and I think that is pretty much why I am having this problem, now it makes total sense !!!.

So my question now is to have a required Y+ should my first near-wall cell centroid be set to the distance given by the online calculators and not my first cell wall ? for the solution to be accurate.
or it is just the utility that uses this method to calculate it this manner and I should go by my usual method of setting my first cell height to the distance given by the online calculators.

Thanks for your time
Regards,
Hasan K.J

Blanco February 1, 2015 09:51

Yes you should set your first near wall cell centroid position to be equal to the y coming from on line calculators. If you prefer to refer to first near wall cell height, you should set it to the double of y coming from y+ calculators, to obtain the required y+.

Regards,

Andrea

ashim February 4, 2015 12:28

Hi Andrea,

Good afternoon. I am following this thread, as I have the same problem as Hasan KJ. I have set the y double in meshing process to get the required y+ in meshing software (cfMesh, Ansys ICEM). I have checked in paraview that the first wall thickness is same as specified in Meshing. But when I am calculating y+ in openFoam, it gives me different values. Another thing is that I am getting different y+ from yPlusRAS and yPlusLES. Any kind of suggestions will help me a lot.

Regards,

Ali

Alhasan February 4, 2015 12:37

Quote:

Originally Posted by ashim (Post 530399)

But when I am calculating y+ in openFoam, it gives me different values. Another thing is that I am getting different y+ from yPlusRAS and yPlusLES. Any kind of suggestions will help me a lot.

Hi Ali,

YPlusRAS calculates the Y star and not the Y Plus so

You might want to look in to these following threads for further details.

http://www.cfd-online.com/Forums/ope...-testcase.html

http://www.cfd-online.com/Forums/ope...lus-field.html

hope this helps you,

all the best,
Hasan K.J

Blanco February 5, 2015 11:52

Well, in my understanding the yPlusRAS utility let you have the y+ or the y* depending on what is the boundary condition you are using on your wall.

I mean, if I use the nutLowReWallFunction then from its code I get:

Code:

tmp<scalarField> nutLowReWallFunctionFvPatchScalarField::yPlus() const
{
    const label patchi = patch().index();
    const turbulenceModel& turbModel =
        db().lookupObject<turbulenceModel>("turbulenceModel");
    const scalarField& y = turbModel.y()[patchi];
    const tmp<volScalarField> tnu = turbModel.nu();
    const volScalarField& nu = tnu();
    const scalarField& nuw = nu.boundaryField()[patchi];
    const fvPatchVectorField& Uw = turbModel.U().boundaryField()[patchi];

    return y*sqrt(nuw*mag(Uw.snGrad()))/nuw;
}

where y is the centroid distance from the wall patch, nuw is the kinematic viscosity and Uw is the fluid velocity both evaluated in the cell centroid next to the wall. We know that

y+=(y*U_tau)/nu
(where * mean multiply, I'm not referring to y* here)

and the formula in nutLowReWallFunction gives me exactly the y+ value, because we know that U_tau = sqrt(nu*dU/dy) evaluated at wall, assuming that y is the axis perpendicular to the wall.

Therefore I get the exact y+ value from the yPlusRAS utility if I use the nutLowReWallFunction boundary condition.

This is also consistent with the comments I found here:

http://www.openfoam.org/mantisbt/view.php?id=835

Please correct me if you have other info about this topic.

Best regards,

Andrea

JasonWang3 March 18, 2015 10:21

Quote:

Originally Posted by immortality (Post 437082)
hi
search this site.there are some good threads with y+ for compressible flows.
do you use low-Re or high-Re?

Hi
I use LowRe model. When I type in ''yPlusRAS -compressible'', y+ is zero in all cells.
I noticed that you mentioned that this command was for HighRe model.
What can I do when I use LowRe model?

Blanco March 18, 2015 11:48

yPlusRAS works both for HighRe and LowRe turbulence models, the only difference is that it uses nut for incompressible flow while it uses mut for compressible flow.

There should be some other problem that gives you y+=0 in your cells...how do you check y+ value?

JasonWang3 March 18, 2015 13:05

Quote:

Originally Posted by Blanco (Post 536979)
yPlusRAS works both for HighRe and LowRe turbulence models, the only difference is that it uses nut for incompressible flow while it uses mut for compressible flow.

There should be some other problem that gives you y+=0 in your cells...how do you check y+ value?

I noticed that there is no rho file in the folders. When I look into the file '' yPlusRAS.C ''

IOobject rhoHeader
(
"rho",
runTime.timeName(),
mesh,
IOobject::MUST_READ,
IOobject::NO_WRITE
);

if (!rhoHeader.headerOk())
{
Info<< " no rho field" << endl;
return;
}

Info<< "Reading field rho\n" << endl;
volScalarField rho(rhoHeader, mesh);

This probably means that the rho file must be required when using yPlusRAS.
And I am using sonicFoam, there is phi instead of rho.
So this is the reason why all the plus values is zero.
But still have no idea how to obtain the yPlus value, maybe rho from the state equation and then use yPlusRAS.

Do you have other suggestions? And thanks for your replying.


All times are GMT -4. The time now is 11:32.