[cnsidero]

Eren10 can you post of picture of what you're trying to do to help me understand? I might be better able to give you proper guidance this way.

Thanks, Chris

[Eren10]

Originally Posted by cnsidero

Eren10 can you post of picture of what you're trying to do to help me understand? I might be better able to give you proper guidance this way.

Thanks, Chris

I have attached a view of what I was trying to do. You can see that there are 2 domains, with overlapping region. This domains should fit at that section.

[cnsidero]

Eren10 to get the extrusions to match you need to extrude from all the airfoil connectors simultaneously. To do so, select all the airfoil connectors then perform the extrusion (Create > Extrude > Normal ...).

You may need to take some precautions near the trailing edge but I can't see the detail there. Is it blunt or sharp?

[Eren10]

It is sharp. I have created a lot of meshes with the method u said. but this way I have not much control over yplus values, but it is oke.

If it is possible I would save the BoundaryConditions once, else I have to type it again, I am using the geometry for different simulations.

And a last question: Is there a general function that will improve the meshquality after the mesh is generated ?

[ziad]

You can still have very good control over the Y+ values by doing it the way Chris advised. It is better to use several connectors on the pressure and suction sides, and then extrude from them all simultaneously. Your mesh will be much smoother and will not overlap.

As for mesh quality tools, you can use the elliptic solvers that come with the structured blocking tools. The default settings should be pretty good for this.

If you run into problems at the trailing edge, build a connector there that is approximately normal to the two surfaces of the airfoil and then extrude along this connector normal to the airfoil surface. Once done, you can then extrude this connector downstream to create your wake region.

[cnsidero]

Originally Posted by Eren10

It is sharp. I have created a lot of meshes, the last what I have asked was to have control over the yPlus values because I am using wallFunctions.

If it is possible I would save the BoundaryConditions once, else I have to type it again, I am using the geometry for different simulations.

It's not clear to me what you trying to accomplish - I am sorry for that. From the picture you attached it looked like you creating an extrusion for each connector ... ahhh, I know what you are trying to do now. You want the near wall spacing to vary along the length of the airfoil.

As you've found out, you can only specify one delta_s when creating an extrusion but there is a way to achieve what you're looking for. First, split the airfoil surfaces at one or more locations, e.g. 50% chord. I see you've done it on the suction side so do the same on the pressure side.

Now create the extrusion with all the connectors. So select them all then Create > Extrude > Normal ... You should now see the Assemble panel. Before clicking Done, in the Assemble Special frame, click Delete All Edges, change the Assemble Type to One Edge Per Connector, click Assemble and then click Done. Perform the extrusion as previously.

You'll notice now that one domain will be created from each connector and there are connectors emanating from the split points in the middle of the airfoil. Using Grid > Distribute you can modify the end spacing and distribution on these connectors to achieve the spacing you want at each location. For example, when I tried it I found that when I modified the spacing I had to also change the distribution function of the connector to Geometric.

The tricky part in the doing the above is that its most likely going to disturb the internal grid lines created the hyperbolic extrusion. You can remedy this by running the domains in the elliptic solver. Pick the domains, Grid > Solve ... and run the solver for 20-30 iterations.

I went through this procedure myself on a NACA4412 with C = 1. I split the airfoil at ~40% on top and bottom. I created a One Edge Per Connector extrusion (as outlined above) with ds = 0.0001, GR = 1.2 and 30 layers. I then change the middle normal connectors wall spacing to 0.0004 and distribution to Geometric. I did the same for the normal connectors at the trailing edge but with ds = 0.0008. I then ran the domains through elliptic solver for 30 iterations with default settings.

See the result in the attached image. It's a bit tough to see but you can make out the expanding BL near the TE.

Let me know how it goes, Chris

[cnsidero]

Originally Posted by ziad

You can still have very good control over the Y+ values by doing it the way Chris advised. It is better to use several connectors on the pressure and suction sides, and then extrude from them all simultaneously. Your mesh will be much smoother and will not overlap.

As for mesh quality tools, you can use the elliptic solvers that come with the structured blocking tools. The default settings should be pretty good for this.

If you run into problems at the trailing edge, build a connector there that is approximately normal to the two surfaces of the airfoil and then extrude along this connector normal to the airfoil surface. Once done, you can then extrude this connector downstream to create your wake region.

Sorry Ziad, you replied before I could finish my long explanation ;-). Thanks for your help.

[ziad]

Originally Posted by cnsidero

Sorry Ziad, you replied before I could finish my long explanation ;-). Thanks for your help.

Don't worry about it

BTW I don't think it is necessary to have such tight control over the normal spacing to the wall to achieve a good Y+. If Eren is using RANS with the usual wall function recipes he will need to have 30 <= Y+ <= 150 and this will give a comfortable margin of wall spacing to use.

Another way of doing this would be creating one connector at the TE and then extruding it along the pressure and suction sides, followed with a healthy elliptic solver dose...

[Eren10]

Originally Posted by cnsidero

I created a One Edge Per Connector extrusion (as outlined above) with ds = 0.0001, GR = 1.2 and 30 layers.

To vary the yPlus values I should be able to change the y distance to the first cell. With the procedure you explained this can't.

I am trying to reduce simulation error as far as I can. Anyway, I will continue with the one normal extruded mesh.

Thank you Chris and Ziad.

[Eren10]

I have a question about the function " solve " in Pointwise. I think this can be done after mesh is generated. Wat is its function ? Shall the mesh quality improve ?

Regards.

[omidomani]

Originally Posted by ziad

I've been using Gridgen and Pointwise for over three years and recommend both. For about a year now you can export Pointwise meshes directly in OpenFOAM format. Never had a problem with any mesh created with these two packages. Just make sure you run the GridGen/Pointwise own mesh improvement algorithms first and you will get high quality meshes.

Both are fairly easy to learn through the provided tutorials. Gridgen has a lot of very advanced (and poorly documented) features that allow you to micro-manage almost any aspect of the mesh but I've never had to use them. The basic aspects covered in the tutorial make it possible to create quality meshes for both commercial work and research.

Ziad

Dear Ziad,
You have mentioned that it is possible to export Pointwise meshes directly in OpenFOAM format. Before I begin creating the mesh in Pointwise, I can choose OpenFOAM as the solver. After creating the mesh, it is possible to export it as a grid file (.gg). Would you please let me know what further steps should be taken to generate the mesh in OpenFOAM, by using this .gg file?

[ziad]

Originally Posted by omidomani

Dear Ziad,
You have mentioned that it is possible to export Pointwise meshes directly in OpenFOAM format. Before I begin creating the mesh in Pointwise, I can choose OpenFOAM as the solver. After creating the mesh, it is possible to export it as a grid file (.gg). Would you please let me know what further steps should be taken to generate the mesh in OpenFOAM, by using this .gg file?

Hi,

Not sure I understand what you mean. I haven't used Pointwise for a while now and don't have a license available for checking, but off the top of my head *.gg is the original GridGen format. Why do you need it anyway? Save your mesh under pointwise format (*.pw) and proceed as usual. The manual has all the info needed.

Ziad

[omidomani]

Thanks for your response. To make my question clear, as you know, it is possible to convert a mesh created in a commercial software, into the format that OpenFOAM uses. For exam, "gambitToFoam" command is used for converting a gambit mesh to OpenFOAM format. My question is that, what is the process to convert the ".pw" file to the format that OpenFOAM uses.
Thanks in advance!

[ziad]

Originally Posted by omidomani

Thanks for your response. To make my question clear, as you know, it is possible to convert a mesh created in a commercial software, into the format that OpenFOAM uses. For exam, "gambitToFoam" command is used for converting a gambit mesh to OpenFOAM format. My question is that, what is the process to convert the ".pw" file to the format that OpenFOAM uses.
Thanks in advance!

Pointwise has native export into OpenFOAM format. No need to use an OpenFOAM utility, an there isn't one anyway. Just go to Export->CAE under the File menu in Pointwise. For details check the manual.