[aero_cfd]

Hi,

Attached are some pictures of a wing i am trying to mesh, however I get highly skewed elements around the sharp trailing edge and the leading edge, in addition the prism layer seems too large.

I used the setting in shown in the picture , I tried to play with the maximum angle criteria and Equi-angle , but always the same problem.
I defined the wing as a wall boundary condtions with a DeltaS of 1e-5.

It is worth mentioning that I would like to have a tetrahedral region around the trailing edge tip to eliminate the highly skewed elements

What should I do to improve the quality of this mesh ?

Thank you a lot.

[rmatus]

You are not getting any T-Rex layers at the leading and trailing edges because the T-Rex first step size is as large as or larger than the local surface meshing. T-Rex automatically stops when the marching step size and the lateral size are equal, so it is never getting started in these locations.

I would try using a smaller initial Delta S for the T-Rex walls. Unless this is a really low Reynolds number flow, it looks like it needs to be smaller to resolve the boundary layer anyway.

[aero_cfd]

Originally Posted by rmatus

You are not getting any T-Rex layers at the leading and trailing edges because the T-Rex first step size is as large as or larger than the local surface meshing. T-Rex automatically stops when the marching step size and the lateral size are equal, so it is never getting started in these locations.

I would try using a smaller initial Delta S for the T-Rex walls. Unless this is a really low Reynolds number flow, it looks like it needs to be smaller to resolve the boundary layer anyway.

Hi,

Thanks a lot for your answer, I followed your advice, changed the Delta S to 1e-6 , however as you see the problem at the TE persists , I used Maximum Angle criteria of 165 and Full layers =0 since it's a sharp TE.

Is there something else that can be done to improve the TE area ?

Cheers,

[rmatus]

With a sharp trailing edge like that, you are not going to be able to get a cell with an included angle less than 165 degrees on either side of it. There are several options to get more layers at the trailing edge:

1. Allow included angles bigger than 165 degrees.
2. Set full layers to zero. This will allow Pointwise to extrude multiple normals off the sharp trailing edge to improve cell quality.
3. Use a C-type domain topology to remove the sharp trailing edge angle from the mesh. See tutorial #2 from the Pointwise tutorial manual to see how this works.

Let me know if any of those give you what you want.

[aero_cfd]

Originally Posted by rmatus

With a sharp trailing edge like that, you are not going to be able to get a cell with an included angle less than 165 degrees on either side of it. There are several options to get more layers at the trailing edge:

1. Allow included angles bigger than 165 degrees.
2. Set full layers to zero. This will allow Pointwise to extrude multiple normals off the sharp trailing edge to improve cell quality.
3. Use a C-type domain topology to remove the sharp trailing edge angle from the mesh. See tutorial #2 from the Pointwise tutorial manual to see how this works.

Let me know if any of those give you what you want.

Hi,

Thank you for your reply,

I already used the two first options with no success.
I need tetrahedral cells around the trailing edge for my application, is it possible to get a block around a small portion of the TE with tetrahedral and the rest of the wing with T-REX ?

I tried to split the block created in order to create a hole there then fill that block with tet cells, but apparently Pointwise can't split unstructured blocks ?

Thank you again.

[rmatus]

If you want to force tetrahedral cells around the trailing edge you could put a cylindrical block around that area and fill it with tets as in the attached image.

[aero_cfd]

Originally Posted by rmatus

If you want to force tetrahedral cells around the trailing edge you could put a cylindrical block around that area and fill it with tets as in the attached image.

This is in 2D? how is it done in 3D? create a cylindrical block there and use its exterior surfaces with the T-REX?

[rmatus]

Yes, I did this in 2D just for simplicity, but the same idea works in 3D. Just set the cylindrical domains to a match type T-Rex BC when you extrude T-Rex cells on the main block.

[aero_cfd]

Originally Posted by rmatus

Yes, I did this in 2D just for simplicity, but the same idea works in 3D. Just set the cylindrical domains to a match type T-Rex BC when you extrude T-Rex cells on the main block.

I tried what you suggested but the cylinder had highly skewed tetra in it.
I changed the approach and I translated a 2D mesh, and made a a block as shown in the figure , but I still have the same problem when I initialise it.

This mesh is a coarser mesh then the the ones I had before , the domains around re structured created from the translations , and the front and back domains are unstructured.

What can I do to get this block populated with high quality tetrahedral ? I was working on this for a while but can't get what I am doing wrong.

Thank you!

[rmatus]

Any chance you could share your Pointwise project file (.pw) here? I can think of several possible causes of the problem you are seeing:

1. Looks like there are some large spacings on the boundaries of the region you are trying to put a tetrahedral mesh on.
2. There might be inconsistent spacings between adjacent domains (and/or connectors) on the boundary.
3. Some tetrahedral solver setting preventing it from getting an initial mesh.

For background, why do you want to put terahedral cells in the trailing edge region rather than continue on with hexahedral cells like on either side of that region?

Thanks,
Rick

[aero_cfd]

Originally Posted by rmatus

Any chance you could share your Pointwise project file (.pw) here? I can think of several possible causes of the problem you are seeing:

1. Looks like there are some large spacings on the boundaries of the region you are trying to put a tetrahedral mesh on.
2. There might be inconsistent spacings between adjacent domains (and/or connectors) on the boundary.
3. Some tetrahedral solver setting preventing it from getting an initial mesh.

For background, why do you want to put terahedral cells in the trailing edge region rather than continue on with hexahedral cells like on either side of that region?

Thanks,
Rick

I attached the project file here

I want to have a 3D C_mesh around the wing, with that region with tetrahedral because for my application I want to remesh that tetra region when the TE deforms , and only tetrahedral can be re-meshed efficiently in Fluent .

[rmatus]

Thanks, but when I try to download the file from JustBeamIt it gives the message, "sorry, this download link no longer exists "

[aero_cfd]

Originally Posted by rmatus

Thanks, but when I try to download the file from JustBeamIt it gives the message, "sorry, this download link no longer exists "

I sent you a link in private messages, I hope that one works .

[rmatus]

Yes, the private link worked. Thank you.

The poor mesh quality is caused by large differences in spacings (an order of magnitude jump) between abutting connectors and a large difference spacing between the spanwise (Z) direction and the other two directions (3 orders of magnitude different).

Since you are trying to put an isotropic (same in all directions) tetrahedral grid inside a boundary that is highly non-isotropic there are conflicting constraints that result in poor grid quality.

How do you fix this? You can use Pointwise's T-Rex anisotropic tetrahedral extrusion to solve the first problem, but you will still have problems in its isotropic core region due to the 3 order of magnitude difference in grid edge lengths between the Z direction and the X and Y directions. If Fluent requires fully tetrahedral grid for its adaption then you have to use more uniform grid spacing, which means adding more grid points in the Z direction and thus increasing the cell count significantly.

If you want to try a completely different approach, you could script the TE deformation in Pointwise, which would let you use the more desirable structured, C-topology you want. Here is a webinar that gives a quick introduction to how it works: http://www.pointwise.com/workshops/2...cripting.shtml

Hope this helps.

[aero_cfd]

Originally Posted by rmatus

Yes, the private link worked. Thank you.

The poor mesh quality is caused by large differences in spacings (an order of magnitude jump) between abutting connectors and a large difference spacing between the spanwise (Z) direction and the other two directions (3 orders of magnitude different).

Since you are trying to put an isotropic (same in all directions) tetrahedral grid inside a boundary that is highly non-isotropic there are conflicting constraints that result in poor grid quality.

How do you fix this? You can use Pointwise's T-Rex anisotropic tetrahedral extrusion to solve the first problem, but you will still have problems in its isotropic core region due to the 3 order of magnitude difference in grid edge lengths between the Z direction and the X and Y directions. If Fluent requires fully tetrahedral grid for its adaption then you have to use more uniform grid spacing, which means adding more grid points in the Z direction and thus increasing the cell count significantly.

If you want to try a completely different approach, you could script the TE deformation in Pointwise, which would let you use the more desirable structured, C-topology you want. Here is a webinar that gives a quick introduction to how it works: http://www.pointwise.com/workshops/2...cripting.shtml

Hope this helps.

Thank you a lot for your help, one last question, I didn't uite understand what you meant by scripting the TE deformation, you mean create different meshes for each TE deformation ?

Cheers,

[rmatus]

Yes, you can script both the geometric deformations and the regeneration of the mesh using the Glyph scripting language.