[kannstmasehn]

Hello,

I want to simulate a cyclone in Star CCM+. I have a ICEM .prj file with .atr, .blk, .fbc, .par and .tin. I extracted a mesh with 800k cells. How can I change the number of cells? The rest should stay the same. Is that possible or do I need a new icem project? I tried to reduce the size of the cells but that didn't really work. Can you help me?


Thank you very much!

[diamondx]

you need to generate a new mesh. that should not take longtime because you have the blk. open the geometry, open the blocking and reduce the number of node of your edges. then output it again

[kannstmasehn]

do i have to select each edge or can I increase the number of nodes for the whole geometry? can you take a screenshot how to do it? or which tab do I need to use? i want to increase the number of cells but decrease would be also good

[diamondx]

yes, each edge. you will find that in the blocking tab. i suppose you are not familiar with icem cfd and you don't have time to pass trough the tutorial. then just take some minutes in youtube to learn how to do that.

[asal]

If you have equal spacing in all or most of the edges you can easily change the spacing in the part mesh setup and then update it blocking => pre-mesh params.
Then you don't need to assign new spacing for each edge.

[kannstmasehn]

Thank you very much. I created more and less cells, that worked well. Now I need to add some prism layers. I think the mesh doesn't have any. Can I easily add some oder maybe how can I refine the cell number just near to the wall?

Another problem is in Star CCM+. The SDR does not converge. What does that mean? And how do I fix that problem?
I am always reading about k-epsilon and RSM. Why does no one goes with k-omega? Can you explain that to me? Is that model not working with cyclones? I think it's a little bit better than k-epsilon. Or is it not?

[asal]

In the mesh, global mesh setup, prism, set the number of layers and other parameters for you prism. In mesh part setup, mark the parts which you want to have prism. In the compute mesh, prism, choose the existing mesh and then click compute!
ICEM with add prism layer in the mesh.

[kannstmasehn]

okay, thank you. I'll have to go through every step, right?
Could it be that no prism layers are created because the cells are already very small?
I just have an inlet, an outlet and a wall. To select the parts for the prism layers I just cannot select 'wall', I need to create new parts, because I don't want to have prism layers everywhere, is that right?

[asal]

Originally Posted by kannstmasehn

okay, thank you. I'll have to go through every step, right? Could it be that no prism layers are created because the cells are already very small?

No

Originally Posted by kannstmasehn

I just have an inlet, an outlet and a wall. To select the parts for the prism layers I just cannot select 'wall', I need to create new parts, because I don't want to have prism layers everywhere, is that right?

Yes!

[kannstmasehn]

The prism layers worked. But it seems that icem did not create the number of prism layers I wanted to have. Or am I wrong? Here is a picture of my actually mesh:

http://s7.directupload.net/file/d/3212/kf8m6qw8_jpg.htm

The next problem with the mesh is that star ccm says the mesh is invalid:

-> MESH VALIDITY:
Mesh is INVALID:
# Negative Volume Cells: 55
# Unclosed Cells: 426

In icem I run in 'edit mesh' --> 'check mesh' and there was no problem. I went throug Blocking --> Block Checks --> "Run Check/ Fix" and "Fix inverted blocks". But nothing really happened. It just asked if I want to remesh and I said yes. How can I fix that?

Num. of inverted Hexa elements = 268
Fixing inverted hexas by diagonal smoothing...
Num. of inverted Hexa elements = 252
Num. of inverted Hexa elements = 127
Num. of inverted Hexa elements = 107
Num. of inverted Hexa elements = 108
Warning: could not fix all iverted hexas

This appears while creating the prism layers.

[asal]

Do you generate hexa by using blocking?!!!!
Then why inflation? you should use the spacing to fine the mesh close to the walls. I think you want to generate tetra.
See the figures!

[kannstmasehn]

Originally Posted by asal

Do you generate hexa by using blocking?!!!!

what do you mean by that? how I create the mesh? As I said, I did not create the icem-project myself. I just want to extract some meshes with different cell numbers and for y+, I want to make the mesh finer or coarser near the wall.

My procedure to get a .msh file out of the icem project was first to right-click on 'pre-mesh' and then 'convert to unstructered mesh', then on output I selected the wall, velocity inlet and pressure outlet. For increasing/ decreasing the cell numbers I changed the number of nodes for every edge. If this way is wrong, please tell me, I'm not an expert in icem.
Finally I want to have a hexa mesh structured as it is on your picture. I want to change the number of cells and the refinement near the wall for different y+ values. Do you understand? I just need the mesh in some varieties.

It would be great if you can help me with that!

[asal]

To be honest, I cannot understand you!!
What do you mean by this:
"then on output I selected the wall, velocity inlet and pressure outlet."!!!

y+ is a function of velocity and kinematic viscosity and not just function of the mesh.
See below:
http://www.cfd-online.com/Wiki/Dimen...tance_(y_plus)

You should first use the blocking and then as I said assign the correct spacing to fine/course the mesh near the walls, if you want to generate hexa meshing. Prism is used just for tetra meshing!

try some tutorial same as below:

http://www.youtube.com/watch?v=9h97FvWJPcY

[kannstmasehn]

Originally Posted by asal

To be honest, I cannot understand you!!
What do you mean by this:
"then on output I selected the wall, velocity inlet and pressure outlet."!!!

To extract a .msh I right-clicked as it is seen in the video you posted at 9:20 on 'pre-mesh' and then on the tab 'output' at the top. There I assigned my parts to 'wall' and so on and then extractet the .msh file. I just wanted you to explain how my was to get the .msh-file out of the project, maybe there is a different or better way.

You should first use the blocking

Within the blocking I can change with the number of nodes of every edge and as a consequence the number of cells. Do you want to say that? If not I do not know what you want to say.

and then as I said assign the correct spacing to fine/course the mesh near the walls, if you want to generate hexa meshing.

Yes, I understand that. I need a certain heigth for the cell near the wall, can I just control the cellheigth with the spacing and the number of nodes, if the length of the edge is given?

Prism is used just for tetra meshing!

That was my mistake. Thank you!

[asal]

Originally Posted by kannstmasehn

Within the blocking I can change with the number of nodes of every edge and as a consequence the number of cells. Do you want to say that? If not I do not know what you want to say.

Yes!

Originally Posted by kannstmasehn

Yes, I understand that. I need a certain heigth for the cell near the wall, can I just control the cellheigth with the spacing and the number of nodes, if the length of the edge is given?

Yes!

[kannstmasehn]

great!

Is there an easy way to change the measurements of the mesh? I think of diameteres and something like that. Do I have to scale every edge or which way should I go for that?

[Nima Shah]

Originally Posted by asal

If you have equal spacing in all or most of the edges you can easily change the spacing in the part mesh setup and then update it blocking => pre-mesh params.
Then you don't need to assign new spacing for each edge.

Hi, thanks for the comment. Do you possibly know where we can change the edging that we could do in pre-mesh after converting the mesh to unstructured mesh? I mean now I have a mesh that needs to add some more divisions and wall prism layers, however, I have converted the mesh to .msh and now I do not know how I can have control over the blocking and ore-mesh.
I wonder if you can help or provide some resource
Best

[alainislas]

Were you the author of the mesh in ICEM CFD? If so, under the project directory you should have access to


(1) .tin files contain geometry entities: lines, curves, points, bodies
(2) .blk files contain the blocking, pre-mesh params,
(3) .fbc, .atr contain the attributes and boundary conditions
(4) .uns is the unstructured mesh (before writing .msh)
(4) .msh is the final mesh ready to use in Fluent, OpenFOAM, etc...



Check whether you have these files or not, and simply unload the .uns or .msh files, so you remain with the first 3 and you can continue editing from there

[Nima Shah]

Originally Posted by alainislas

Were you the author of the mesh in ICEM CFD? If so, under the project directory you should have access to


(1) .tin files contain geometry entities: lines, curves, points, bodies
(2) .blk files contain the blocking, pre-mesh params,
(3) .fbc, .atr contain the attributes and boundary conditions
(4) .uns is the unstructured mesh (before writing .msh)
(4) .msh is the final mesh ready to use in Fluent, OpenFOAM, etc...



Check whether you have these files or not, and simply unload the .uns or .msh files, so you remain with the first 3 and you can continue editing from there

Hello dear alainislas and thanks for your reply.
I have created two grids in Workbench with same Geom file. I have the .blk,
.tin .uns .prj and .msh
My problem is that : I want to keep refining and modifying my mesh by getting the .msh and solving the problem for some iterations/timesteps. However, I don't know how I can have the option to modify my mesh before several times after converting to unstructured mesh.
How may I unload the .uns?
I am a bit new to ICEM, so I appreciate it if I could know how to save copies of a blocking so each time you can only change the bunching and number of edge sizings? Should I just go to dp0>ICM>and copy the .blk and .tin files? In that case, the next time I make changes to the Mesh, it will be saved on the new copy I guess.

Regards

[alainislas]

Hi,

To unload the .uns file simply go to file/mesh-> close mesh. What you want to do is relatively simple,



Option 1
Create many folders
You can clone the project files as many times as necessary. Edit the blocking for each case, generate corresponding .uns file and then write output .msh.


Option 2
Under the same project folder
Unload the .uns file. Continue editing the blocking from there. Save blocking (.blk files are appended with numbers, e.g. blk1, blk2, blk3, etc.. ICEM uses the latest file, which is the one without numbers). Once with the new params, generate pre-mesh and convert to unstructured mesh. In the dialog box, give another name to the newly .uns file. Then simply load and unload .uns so you write the desired output .msh