[s.m]

Hi Dear All;
i use snappyHexMesh for meshing the domain around two element airfoil.
during the running of snappyHexMesh, this message is appear that ""did not succesfully snap mesh. Giving up"" . is it related to the parameters in snapControls section of snappyHexMeshDict?
if yes, what changes should i do in my snappyHexMeshDict that i have attached in the following?
thank you

[chegdan]

I would make your base mesh smaller (i.e. change your blockMeshDict to have more subdivisions), decrease your levels on your edges from 6 7 to 5 6 or lower depending on your base mesh sizing and change

    tolerance 1.0;
    nSolveIter 300;

in snapControls. A lot of errors with SHM are resolved by changing your base mesh sizing.

[s.m]

Originally Posted by chegdan

I would make your base mesh smaller (i.e. change your blockMeshDict to have more subdivisions), decrease your levels on your edges from 6 7 to 5 6 or lower depending on your base mesh sizing and change

    tolerance 1.0;
    nSolveIter 300;

in snapControls. A lot of errors with SHM are resolved by changing your base mesh sizing.

Hi Dear chegdan,
i am using the OF 2.2.0. this is my blockMeshDict, would you please look at it and tell me is it necessary to increase the subdivisions?

[chegdan]

The closer you make your base mesh cell aspect ratio to unity (equal length in x y and z direction), the better results you will see in SHM. Try:

blocks
(
    hex (0 1 2 3 4 5 6 7) (880 480 1) simpleGrading (1 1 1)
);

and maybe change your z-thickness to 0.025 to match the aspect ratio of the x and y-directions. With your current settings of levels 6 7 you have cells that are on the size of 0.025/(2^6) = 3.9E-4 [m] to 0.025/(2^7) = 1.95E-4 [m].

[s.m]

Originally Posted by chegdan

The closer you make your base mesh cell aspect ratio to unity (equal length in x y and z direction), the better results you will see in SHM. Try:

blocks
(
    hex (0 1 2 3 4 5 6 7) (880 480 1) simpleGrading (1 1 1)
);

and maybe change your z-thickness to 0.025 to match the aspect ratio of the x and y-directions. With your current settings of levels 6 7 you have cells that are on the size of 0.025/(2^6) = 3.9E-4 [m] to 0.025/(2^7) = 1.95E-4 [m].

thank you,is my cells size good or i should increase the level of refinementSurfaces?

[chegdan]

...is my cells size good or i should increase the level of refinementSurfaces?

This ultimately depends on your y+ and turbulence model you are using so I can't comment on it. To snap to the surface, it should be fine.

[s.m]

Originally Posted by chegdan

This ultimately depends on your y+ and turbulence model you are using so I can't comment on it. To snap to the surface, it should be fine.

i have both high-Re and low-Re number turbulent model, "k-wSST & lunderSharmaKE" would you please guide me?
is this cell size belong to all the cells around my airfoil? i ask this question, becuase for computing the y+ i only need to know the first cell size of my mesh.
thank you again for your advice

[chegdan]

From my experience

lunderSharmaKE needs y+ <= 1

but it really can't be calculated until your simulation has been run to know how much further you need to refine your mesh. You can use the yPlusRAS utility to calculate the y+ value.

[s.m]

Originally Posted by chegdan

From my experience

lunderSharmaKE needs y+ <= 1

but it really can't be calculated until your simulation has been run to know how much further you need to refine your mesh. You can use the yPlusRAS utility to calculate the y+ value.

yes you are right. for reducing my y+ to be appropriate for low-Re number turbulent models, i should increase the subdivision in blockMeshDict, is it right?
is it better to use level (6 6) for the refinementSurface, to have squre cells size?

[chegdan]

the (6 6) would mean that if a featureEdge is encountered then the same refinement (a level 6) will be used. If you had done a (6 7) then a further refinement of 7 would be done around the "turn" of the edge.

[s.m]

Originally Posted by chegdan

the (6 6) would mean that if a featureEdge is encountered then the same refinement (a level 6) will be used. If you had done a (6 7) then a further refinement of 7 would be done around the "turn" of the edge.

Thank you i am running the case, with new blockMeshDict and also new snappyHexMeshDict. i'll put the resulted logFile after fininshing.

[s.m]

Hi,
i didn't recive that message anymore, thank you very much for your kind help.
i put some picture of my mesh, would you please tell me is this mesh looks good?
and i also attach the snappyHexMesh and checkMesh logfile.

as you see in checkMesh, "Mesh non-orthogonality Max: 59.5431 average: 7.46241" is it fine?
thank you very much again

[s.m]

and these are, another picture of this snappyHexMesh, as you see ot just doesn't capture the main trailling edge corner angle true,if you have a comment to fix it, please tell me
thanks.

[chegdan]

as you see in checkMesh, "Mesh non-orthogonality Max: 59.5431 average: 7.46241" is it fine?

This is fine, anything above a 70 would be a concern.

also...if you are doing a 2D case, you will be better off doing a 2D mesh. have a look at

tutorials/incompressible/pimpleDyMFoam/wingMotion/wingMotion_snappyHexMesh

for some inspiration on how to generate a 2D mesh.

For resolving the edge, you could try drawing a refinement box around the edge and then make the cells there really small. Lastly, to make your mesh look better in screenshots (i.e. get rid of diagonal cuts in hex cells) you can check "use VTKPolyhedron" in Paraview object inspector when you first import results into Paraview.

[s.m]

Originally Posted by chegdan

This is fine, anything above a 70 would be a concern.

also...if you are doing a 2D case, you will be better off doing a 2D mesh. have a look at

tutorials/incompressible/pimpleDyMFoam/wingMotion/wingMotion_snappyHexMesh

for some inspiration on how to generate a 2D mesh.

For resolving the edge, you could try drawing a refinement box around the edge and then make the cells there really small. Lastly, to make your mesh look better in screenshots (i.e. get rid of diagonal cuts in hex cells) you can check "use VTKPolyhedron" in Paraview object inspector when you first import results into Paraview.

yes, i looked at it some times ago, i didn't check "use VTKPolyhedron" anyTime, but i examine it now, it was really nice. thank you very much
i have another problem yet
as you see, the mesh around the airfoil is extremely tiny but, i get the pressure countour around it really bad.
i write my problem in the solving forum of openFoam.
Home > Forums > OpenFOAM Running, Solving & CFD > wrong contour of pressure at the airfoil leading edge
would you please take a look at it,thank you.

[chegdan]

I will leave that thread to the experts. However, you may want to add some boundary layers cells to your mesh and/or increase the refinement near the surface. If you give as much info as possible on that thread and also search the forum....i bet you will get it solved. Good luck!

[s.m]

Originally Posted by chegdan

I will leave that thread to the experts. However, you may want to add some boundary layers cells to your mesh and/or increase the refinement near the surface. I'm not an expert at airfoils so if you give as much info as possible on that thread and also search the forum....i bet you will get it solved. Good luck!

ok, thank you