[hamed.majeed]

Hi,

What are the parameters used to test the mesh quality:
I know a few such as aspect ration, expansion ratio, orthogonality angle.
There is also this parameter CGI, kindly explain it.
Add any other parameters that are important when reporting a mesh.

Thank you
Regards
Hamed

[diamondx]

topic about mesh quality is discussed multiple time in this forum try searching the forum i'm sure you will find a lot.
Don't know much about cgi parameters, hope someone else can explain it.

[Far]

Originally Posted by hamed.majeed

Hi,

What are the parameters used to test the mesh quality:
I know a few such as aspect ration, expansion ratio, orthogonality angle.
There is also this parameter CGI, kindly explain it.
Add any other parameters that are important when reporting a mesh.

Thank you
Regards
Hamed

mostly we are interested in min angle (>18 deg) , minimum quality (shoud be > 0.3) and expansion ratio. Mostly these parameters are viewed from solver point of view.

There is very nice explanation of these parameters by Simon on this forum, search is the key

[navedahmid]

I think its GCI not CGI

[PSYMN]

The Help documentation should also include something for each metric, but I am not sure what metric you are asking about (GCI or CGI, I don't know of either). What tool are you looking in?

[hamed.majeed]

Hi,
It is the grid convergence index GCI. It is a factor to estimate discretization error based on Richardson extrapolation principle

[Far]

Originally Posted by hamed.majeed

Hi
It is the grid convergence index GCI. It is a factor to estimate discretization error based on Richardson extrapolation principle

Well it is the index of quality of CFD which you are performing. In other words, it is you who will decide that how much mesh size is needed to the asymptomatic behaviour. Whether it is 1 million, 10 million or even 100 million. ICEM will give you whatever you ask for.

[hamed.majeed]

Hi,
thnx for reply.

I have another question. We place the 1st node from the wall based on y+ value and the formula 1st node distance is
delta y = sqrt(74)*Re^(-13/14)*L*y+*L
The value of y+ in above formula depends on the turbulence model used.

My question is:
Once 1st node distance is specified using above formula, what are the parameters that govern the selection of expansion ratio applied to the mesh.
I mean what should the increasing gap of node be starting from the 1st node

[PSYMN]

Usually a ratio of 1.2 is used. But you could go higher or lower if you want the total height of your boundary layer to be less or greater.

The point is just to have enough mesh discretization to capture the boundary layer profile. That profile is changing faster near the wall and reduces as you move away. The ratio is just to reduce the number of nodes so you are not using the same resolution to capture less change.

[Far]

Originally Posted by hamed.majeed

Hi,
thnx for reply.

I have another question. We place the 1st node from the wall based on y+ value and the formula 1st node distance is
delta y = sqrt(74)*Re^(-13/14)*L*y+*L
The value of y+ in above formula depends on the turbulence model used.

My question is:
Once 1st node distance is specified using above formula, what are the parameters that govern the selection of expansion ratio applied to the mesh.
I mean what should the increasing gap of node be starting from the 1st node

Rule(s) of thumb:

1. Use expansion ratio 1.2 at max and for transition critical flows lower values to 1.15 or 1.1

2. For fully turbulent flows you can use the Y+ upto 10, in that case you will have the 10-15 nodes in the whole boundary layer. You can find the boundary layer total thickness from the turbulent flat plate boundary layer formulae

3. Boundary layer gets thinner as Reynolds number increases and vice-versa

[cfd seeker]

2. For fully turbulent flows you can use the Y+ upto 10, in that case you will have the 10-15 nodes in the whole boundary layer

Aaah I wish the whole world would have like that but the transitional flows always give me a headache and as a result extra care for wall y+ and no. of cells in boundary layer

You can find the boundary layer total thickness from the turbulent flat plate boundary layer formulae

I want to add something here, after finding boundary layer thickness from turbulent flat plate boundary layer formula, reduce it by an order of magnitude to get good approximate for airfoils/wing problems

[Far]

Originally Posted by Far

For fully turbulent flows you can use the Y+ upto 10, in that case you will have the 10-15 nodes in the whole boundary layer.

Originally Posted by cfd seeker

Aaah I wish the whole world would have like that but the transitional flows always give me a headache and as a result extra care for wall y+ and no. of cells in boundary layer .

-----------

For transitional flows (laminar to turbulent), you need Y+ less than 1 with other constraints.

[cfd seeker]

For transitional flows (laminar to turbulent), you need Y+ less than 1 with other constraints.

Yes and the most important constraint is values of "Turbulence Parameters"

[Far]

Originally Posted by cfd seeker

Yes and the most important constraint is values of "Turbulence Parameters"

I meant the mesh constraints like enough no of nodes in normal and streamwise direction.

[cfd seeker]

Originally Posted by Far

I meant the mesh constraints like enough no of nodes in normal and streamwise direction.

Turbulence parameters also affects the performance of Turbulent Transitional Models