[Karatix]

Dear All,

currently I am using CFX 10.0 and ICEM 10.0.
My aim is to calculate the aerodynamic properties of an airfoil using a C-Mesh.
So far I managed to use the blocking mechanism to create a premesh, which looks like on seen on the attached picture.
Then I converted the mesh to a structured multigrid mesh, which looks as the premesh.

I know that CFX is not able to do 2D, hence I have to extrude it.
When I tried that using the blocking function 2D to 3D, the mesh was gone (not visible, neither the premesh). However, I exported the data using the "Export Mesh" to Ansys function, but importing to CFX-Pre did not work.

When I tried various solvers only the CFX4 worked and even allowed a 2D mesh (using a thickness). However, creating boundary conditions (wall, inlet, outlet) on the edges is somehow not possible. Does anybody know why and how this can be improved?

Your help will be very much appreciated

Karatix

[PSYMN]

Your order of operations seems wrong. Once you convert the blocking to structured multiblock, further operations on the blocking don’t affect the structured mesh (they are separate branches).

To get your thickness, you should probably convert it from the blocking to UNSTRUCTURED Mesh, then use the mesh editing option to Extrude this mesh by one cell.

To create bocos, you need perimeter elements. In 2D, these would be line elements, but once you convert to 3D, the line elements are extruded as shell elements.

1)Make sure the perimeter curves are in a different part than the surface. This will ensure that the perimeter elements are in different parts than the “volume” elements so that you can apply different bocos to them.
2)When in 2D hexa, perimeter line elements are only created where edges are explicitly associated to the perimeter curves. If an edge is aligned with the edge and perhaps even has verts that are associated, but the edge its self is only associated to the surface (default) then no line elements will be created and the extrusion will not produce shell elements. You will have nothing to hang your bocos on. To check this at the blocking level, turn off the curves and just look at the edges. They should be green around all the boundaries. If any are still surface associated, associate those edges to curves.

Best regards,

Simon

[Karatix]

Hello Simon,

thank you for your advice. However, I aline the outer edges to the outer curves as you said. In addition the curves I created at the front, top and bottom are under Part Inlet and at the curves at the back at Part Outlet. The curves of the airfoil under airfoil.
Then I used the premesh under blocking and converted it to an unstructured mesh.
Using the extrude mesh (under mesh) I extruded it by one cell.
Up to here things worked perfectly.

Then under output --> solver I experimented with all the ones CFX-Pre can read. However for some reason below I could not create boundary conditions as wall, inlet, outlet. If I would use Star CD as a solver, it would be possible to set such boundary conditions.

CFX-4 (only for structured grid)
CFX Taskflow (only for monoblock grid in 2D)
Ansys, CGNS, IDEAS, Nastran did not allow me to write the input file or could not be imported into CFX Pre. Considering that I use version 10.0. Could there be another way?

Just as an experiment I aligned all edges to curves (also inner ones), but I did not have any success with that either.

I also tried to create an unstructured mesh by meshing the lines (without using blocking), but so far this did not work either. I will try again though.

Karatix

[PSYMN]

You are not the first person to have this confusion... Maybe I will get them to change this for the next release, or at least put it in two places

CFX is now "ANSYS CFX"... Scroll up in the output formats and you will find it near the top rather than with the other older (pre ANSYS) CFX variants...

I don't think you need to change anything else.

Simon

[Karatix]

Hello Simon,

you were right. It works with Ansys CFX. I was able to write the input file and import it into CFX Pre. Thank you.

The only last little bit that does not seem to work as I like it, are the boundary conditions. Could you please tell me what is wrong in my process here.

Use Blocking

1. Import airfoil as points and curve
2. Create curves (as parts) around the airfoil, shown in attachment
3. 2D planar Blocking
4. Split block, so the airfoil has a block within
5. Associate Edges to curves around airfoil and associate the edges within the airfoil on the airfoil
6. Delete Block in the airfoil
7. Premesh --> convert to unstruct mesh
8. Extrude by one cell
9. Output --> solver Ansys CFX --> BC (can only chose from Edges, Nodes and Mixed unknown)
If I select "create new" I can see the window:
CFX5.1 Boundary conditions:
Element PID

so I click on "Element PID" where I can only write next to "ID#" a number. (The help was not very useful here either). The idea was to use inlet, outlet and wall as the boundary conditions.


Without Blocking

1. Import airfoil as points and curve
2. Create curves (as parts) around the airfoil, shown in attachment
3. Mesh the curves
(3.1 fiddle with the size of the cells)
4. Extrude mesh by one cell
5. Output --> solver Ansys CFX --> BC (can only chose from Edges, Nodes and Mixed unknown)
If I select "create new" I can see the window:
CFX5.1 Boundary conditions:
Element PID

which is the same problem as before.

In CFX Pre I cannot choose from different locations either to define the boundary conditions, instead I have only the single mesh.

(Btw, as my C-Mesh always had a thin small unmeshed region, in front of the leading, I experimented with a simple square. The reason is that the two edges I curved around to create the curved region did not connect as the command promised.
In addition an unstructured grid might make multi-element analysis easier.)

Thank you for your help in advance,

Karatix

[PSYMN]

I had a quick back and forth on the side with some ICEM CFD experts and they say don’t setup the bocos in ICEM CFD… They all just make sure that the mesh is in separate part names (INLET, OUTLET, WALL, FLUID, etc.) and then dump the file to ANSYS CFD and setup the bocos in CFXPre.

If you see “mixed/unknown” it means you have more than one element type in that part. For instance, your surface and points may be in the same part and so it doesn’t know if it should be applying volume or line properties (since these are both extruded). I would recommend separating your parts so this doesn’t happen.

As for your blocking its self, you could get a better near wall mesh with the Ogrid tool. Instead of deleting the block for the airfoil, create a new blocking material called “dead” or something like that. Then go to OGrid and create an Ogrid with that Dead block(s), make sure to select the option for “Around blocks”. Then adjust this ogrid, adjust the distribution normal to the wall, etc. If you want to get really fancy, you could also select the block behind the ogrid and select the exit edge to create a C-Grid that would give you the best results and a controllable wake refinement.


In the end, turn off DEAD in the parts branch of the tree before converting to Unstructured Mesh.

[Karatix]

Hi Simon,

thank you for the advice. I will have a go at it and hope it will work this time. Btw, parts can also be lines and suround an area. Is this correct or do I have to create surfaces as well, so the mesh can be seperate and therefore different boundary conditions can be set up in CFX Pre?

All the best

Karatix

[PSYMN]

Right, ICEM CFD uses a 3 types of entities... Surfaces, curves, and points. The average 2D model will be surfaces surrounded by curves with points on the corners... But it could also just be curves and points and use the blocking material for the area.

You can put those curves into individual parts. For instance, the curve (line) that represents the opening could be put in the "inlet" part. When the model is meshed, the line elements that form along this curve will be in the INLET part and can be selected for the inlet boundary condition.

If you extrude the mesh, the line elements will become shell elements, but still in the INLET part...

Simon

[Karatix]

Hi Simon,

after some more playing around, I found out that you have to add the blocks to the parts in order to be able to pick inlet, outlet within the CFX-Pre.
Another way is to define the regions of the mesh to a part, but then sometimes the system (or myself) might miss one line of cells and as a results can't simulate anything in CFX.

With adding the entities to the parts I still have to fiddle a bit and see how things respond as it was unsuccessful so far.

It might even work keeping the block (as you labled "DEAD") within the airfoil and just define it as a wall to calculate CL, CD, CM, ... later on.

However, overall it seems that just having the lines within the parts is not enough for setting up the bocos.

Thank you again for your help. I keep you posted, how things are doing.

Karatix

[PSYMN]

Not just lines, but Lines and surfaces should be enough for CFX. You should not need to put the blocks into the surface parts, in fact, that should cause a problem.

If you want to create a very simple setup (maybe just a pipe) and set it up the way you are working... I can take a look and tell you what you need to change.

Alternately, you could follow some of the tutorials that go all the way to the solver.

Simon

[Karatix]

Hi Simon,

sorry that it has been a while, but I kept testing it. Instead of extruding the mesh after the 2D Blocking I set it up as a 3D problem from the beginning.
I then used the volume mesher to create the mesh. By naming the outer surfaces within the parts (Inlet, Outlet, ...) By using the cut loft function I was able to create the hole in the mesh and later on model the problem in CFX. I could see the streamlines going past the airfoil.

So far I have not figured out how to get the lift and drag coefficient of the airfoil, but I am sure I work it out soon.

When I tried using the 3D blocking (o-grid) it had some trouble. In addition I would like to see how a slat and its position effects the flow over the airfoil. Would you say that the automaticly generated mesh would be better to use for this purpose?

In addtion are there any disadvantages in using the volume mesher, apart from longer computing time?

Thank you for your help,

Karatix

[jszl]

Dear friends,

I have a problem. I am just a beginner to use ICEM.

My probelm is

I made two bodies: fluid and solid very simply with blocks.

Then I meshed with hex dominant.

Afterward, I tranfered it into cfx in gtm format.

But there is only one body for fluid. Not for solid inside the fluid.

Ps help me as soon as possible.

Thank you very much


jszl

[PSYMN]

Karatix,

I think the hexa blocking would be excellent for studying an airfoil with flaps and slats. Certainly you could get a higher quality solution. If you wanted it to study a wide range of positions, you could script it. The only down side is the learning curve.

It would be simpler to script an unstructured tetra/prism analysis for a series of batch runs.

If you go with the tetra prism in 3D instead of surface meshing and extruding the triangles and quads into prisms and hexas, the tetras may degrade the quality of your solution slightly. On the other hand, CFX as a solver, is very tetra tolerant.

When I have to do "2.5D" with CFX, I typically do start with 3D mesh to get access to the better Prism inflation, but then I delete everything except the front face and and extrude (sweep) the 2D mesh back to 3D to create the volume model. It is an extra couple steps, but may be worth it.

There are many ways to get what you need. Some are slightly easier or more accurate than others. You can decide which suites you best.

[PSYMN]

JSZL,

Sorry, I don't have enough info to help here. Do you mean you blocked it with ICEM CFD Hexa? And then converted the Premesh to Unstructured mesh? Did you have blocks in the two parts? If you look at the cross section (cut plane) could you see that the solid and fluid were different parts? Could you turn them off independently in the tree? Were there shell elements between them?

If you still need help with this problem, perhaps grab a few pics and a few more details. Then start a new thread so we can help you with this.

In the mean time, you should also go thru some of the tutorials, etc. to make sure you can get thru those examples before heading off on your own.

Simon

[jszl]

Dear Simon,

I will present it in new thread.

Actually I want to simulate the solid in the duct and analyze heat conduction in solid and convection between solid and liquid. Velocity profile as well.
But I have only academic license and so number of nodes is limited.
So I tried to use ICEM to reduce the nodes as much as I can.
But there is only one 3d region after it is exported to cfx pre all the time in either gtm format or cfx5 format.

I got two 3d regions if I followed the procedure of conjugate heating coil from CFX Mesh tutorial documents. I think you may know it.
It is like that it is ok if I use cfx meshing procedure but not ICEM.

But my problem is limited-license. And so I cannot run cfxpre with the meshing quality got from cfx meshing. But I can run with same size in hexa mesh from ICEM blocking. But the simulation I could run is only single phase.

For two phase I could haven't exported to cfx yet.

Please help me if you could understand my problem mentioned above.

Please wait for a while until I make the new thread for that if what I mentioned above is confusing.

Thanks a lot,

JSZL

[KevinW]

Just for those who searched ended up here, it's stupid but might help.
I also have encountered this problem: 2D S809 airfoil structured mesh generated---extrude mesh---CFX, but in CFX-Pre, i have only "fluid"and "topface" as location for boundary.
I finally find it is because when I extrude the 2D mesh, I did not tick the "lines" under "mesh" tree. It's stupid, no line element, then no shell. Now, I have inlet,outlet, wall, all ready.
Two hours figuring this out, hope it help to freshman like me.