I need some pointers to create a grid using ICEM CFD, I have tried but the outcome hasn't been very good

kind regards Dan

Well, to get good advice you need to provide a lot more specifics than that. What does your geometry look like? What grid do you want and what type of analysis is it to be used for? What did you try and why was the outcome not good?

In general, make shure your geometry is as simple as possible before importing, and also error free (all surfaces connected, volumes completely enclosed etc). There is no point in going further unless the Geometry Check tool is totally error free. Avoid sharp points on parts where you are going to use prism layers.

/C

Hello Chebeba Thank you for your answer, My geometry consists of a blade with three different airfoil in the spanwise direction (13 blade station). The varation of twist from root to tip includes angles of 10.5, 2.5, 0 and -2,5 at the tip. the trailing edge of the blade is sharp. I'm trying to use a structured hexa mesh for the blade region, (I would like to capture separation on the suction side of the blade if it is present) and a unstructured hexa mesh for the other flow domain. The problem arises when I am dividing the blade into blocks using Hexa mesh. Because I am going to simulate a steady condition I'm jus modelling a 120 degrees sector (It is a 3bladed wind turbine). I have problems moving vertex inside the volume in the blocking process. Can ICEM CFD use cylindrical coordinates? It is being very difficuk to use cartesian coordinates to arrange the vertices. I can send you an image of how is the problem developing

Kind Regards Dan

You can create local coordinate systems with ICEM CFD. In the upper left you'll see an icon with 'LCS' on it. These can be cartesian, cylindrical, or spherical.

If you associate your vertices with a curve, it becomes very easy to move them around using Move Vertex, since they will slide along the curve.

Another advice: If you use a structured mesh going all the way out to the tip, the shells will get very small and have rather poor aspect ratios. What I'd do for a blade is start with 4 structured 2D blocks from the root and going all the way up to where the tip is becoming narrow, then end with 4 unstructured triangular blocks. Result is similar to this:



/C

Thanks a lot for your advice, by the way when you block your geometry fif you follow the blocking of the tutorial wing body ?? Regards Dan

The wing body tutorial is a fully structured mesh, which is fine if that's what you want. My advice above is for a 2D blocking hybrid mesh, which is much more useful for me. Unfortunately there is no good docs or tutorial on 2D hybrid blocking... It seems to be new stuff with version 10. /C

Dear Chebeba I was wondering if you as well could answer some other questions I have about the boundary conditions that you use opening, inlet etc, etc. for the simulation. The postprocessing with CFX, How can I get Lift and drag coefficients at a specific span location, as well pressure coeficient distribution? As you might notice I'm quite a beginner using CFX and ICEM CFD with this kind of simulations

Kind Regards Dan

Dear Chebeba,

Can you give some idea about how to make the unstructured mesh like your mesh near the tip of the blade? I met some difficulty with my mesh on an impeller, and I think your solution is very helpful for me, but I don't know how to do that. I always follow the tutorial of ICEM, but it seems only for structured mesh.

Please, and thanks alot!!

[luxingzhe]

Originally Posted by Chebeba
;75538

If you associate your vertices with a curve, it becomes very easy to move them around using Move Vertex, since they will slide along the curve.

Another advice: If you use a structured mesh going all the way out to the tip, the shells will get very small and have rather poor aspect ratios. What I'd do for a blade is start with 4 structured 2D blocks from the root and going all the way up to where the tip is becoming narrow, then end with 4 unstructured triangular blocks. Result is similar to this:



/C

Anyone have an idea how to do this?
I also have several low quality element around my wind turbine tip, my strategy is to block out the tip with a square, and trying to form non-conformal mesh (later define interface), but it is not the best solution to me. Again anyone know how to deal with the tip mesh as has been done in this post?

[PSYMN]

Under Blocking => Edit Block => Convert Block Type, you can change the blocks from mapped to swept, change the free face or free block mesh type, etc.

You can do it with a full 3D blocking, but it is usually easier with a surface blocking, then run 2D to 3D fill with an Ogrid. The Ogrid manages the the boundary layer and will sweep out the paved mesh. Then the complex volume around that is "filled" with an unstructured fill, such as tetra.

ICEM_MultiZone_F6.jpg

[luxingzhe]

Originally Posted by PSYMN

Under Blocking => Edit Block => Convert Block Type, you can change the blocks from mapped to swept, change the free face or free block mesh type, etc.

You can do it with a full 3D blocking, but it is usually easier with a surface blocking, then run 2D to 3D fill with an Ogrid. The Ogrid manages the the boundary layer and will sweep out the paved mesh. Then the complex volume around that is "filled" with an unstructured fill, such as tetra.

Attachment 13519

Hi, Simon

As I already blocked my model in 3D, and I just used the "convert block type" to help me with the mesh around the tip, the pre-mesh is pretty good (as attached pic 1,2), however, when i convert the pre-mesh into unstructured mesh, the mesh quality becomes bad, am i doing something wrong?

Besides, how to add boundary layer for my case?

Thanks in advance for your help.