[aylalisa]

Hi to everybody,

I am a newbie with meshing and/but try to mesh a cylindrical furnace with a concentric cylindrical heating element. The air inside the furnace is connected to the surrounding area via two cylindrical drill holes (air inlet, air outlet).
First of all I only try to mesh the air (neiter insulation around the air, nor heating element) with a volume mesh.

Is it possible to add surface meshes for contact areas air/insulation and air/heating element???

I've tried to work with blocking and o-grids but awfully failed at the positions where the drill holes are connected to the air volume,
although I spent really much time.
How can I adjust the meshes of the air inlet and outlet and the air volume mesh???
Please help me!

Since the heating element does not belong to that mesh I need to delete the central block.

Aylalisa

[energy382]

Associate face to surface (in the area of destroyed elements). If it doesn't work, use interpolate.

You've to provide your .tin and .blk files if you don't get rid of the bad elements

Originally Posted by aylalisa

Hi to everybody,

I am a newbie with meshing and/but try to mesh a cylindrical furnace with a concentric cylindrical heating element. The air inside the furnace is connected to the surrounding area via two cylindrical drill holes (air inlet, air outlet).
First of all I only try to mesh the air (neiter insulation around the air, nor heating element) with a volume mesh.

Is it possible to add surface meshes for contact areas air/insulation and air/heating element???

I've tried to work with blocking and o-grids but awfully failed at the positions where the drill holes are connected to the air volume,
although I spent really much time.
How can I adjust the meshes of the air inlet and outlet and the air volume mesh???
Please help me!

Since the heating element does not belong to that mesh I need to delete the central block.

Aylalisa

[aylalisa]

Hi energy,

thanks too much for your support . 'Face to Surface > Part' and 'Face to Surface > Interpolate' helped me to get the attached models.

I've tried different proceedings:

Strömungsraum_6:
bottom-up
I've generated three blocks and then directly used O-Grid. With help of 'Face to Surface' I've reached that result but still receive quite a couple of bad cells.

Strömungsraum_8:
top-down
I've decomposed one big block in several small blocks, deleted some and finally merged the small ones together again. 'Face to Surface' has provided me that result.

Could you tell me how I can get rid off the ugly cells in Strömungsraum_6?
What strategy is in that case the best?

My final goal is to simulate the heating element (solid) and the air (fluid) that is heated up by convection and radiation. So I will end up with two meshes. Do you know if I have to build two individual meshes or is it necessary to built both in the same model, if that is possible at all.


Aylalisa

[energy382]

I'll check it tomorrow. I'm out of office today.

Regards,
Christoph

[BrolY]

With your project number 6, the main problem is the edge of the O-grid of the cylindrical drill holes. They are associated to a surface (colored in black) but there are inside the fluid (they should be colored in blue).
I think you didn't associate the face to surface in the good way.
So use the tool "Blocking -> Blocking Associations -> Disassociate from Geometry -> Edges" and select those edges. They will turn in blue which will fix your issue

[aylalisa]

Hi Alexandre,

thank u for your help!!! That worked , but still there are (only) a few skewed cells at the intersection where the drill hole meets the main pipe.

Why did that deassociate thing exactly work?

Do you know repair for the remaining skewed cells?
Refining the mesh does not really remove that skewed cells but unnecessarily increase the number of cells I think ...

Plenty of regards
Lisa

[Far]

There is problem in blocking. Did you merge the vertices at some stage? Check through scan plane in the two pipes

[aylalisa]

Hello Far,

thanks a lot for your reply!!!
I've not merged vertices but I've cut one big block in many small ones, deleted some and merged them again before I've used o-grid.
Is there maybe a possiblity to get rid of the bad elements without starting the whole procedure from the beginning?

What kind of proceeding is in that case the best one:
Start with one big block, cut in small ones, delete and merge to adjust the geometry, or
create three blocks: one for the main air volume and two additional small ones for inlet and outlet air pipes???
In each case I end up with a couple of bad cells, even if I don't merge vertices on the way?!
Do I make a principal mistake or could I improve the mesh quality by local adjustments?

Viele Grüße
Lisa

[Far]

Angle > 34 deg
Quality > 0.5

Steps

1. One bigger block and o-grid. Delete inner block and associate edges to curves. Snap vertices.

2. Split at appropriate places (four along bigger pipe and two on two sides of smaller pipes).

3. Draw two curves through centre points in smaller pipes (see in attach files) and use extrude along curve option to extend blocking in smaller pipes and associate curves at the end of pipes and at intersection with larger pipe.

4. Make ogrid for smaller pipes. Select two blocks (one for smaller pipe and one in the larger pipe touching heating pipe and select two end faces)

5. Assign sizes on surfaces through part mesh setup (maximum size 3) and click on update all (blocking>edge mesh parameters> update all). And if necessary set the edge mesh parameters for the o-gird edges in the smaller pipes

genießen

[Far]

Originally Posted by aylalisa

Hi energy,

thanks too much for your support . 'Face to Surface > Part' and 'Face to Surface > Interpolate' helped me to get the attached models.

I've tried different proceedings:

Strömungsraum_6:
bottom-up
I've generated three blocks and then directly used O-Grid. With help of 'Face to Surface' I've reached that result but still receive quite a couple of bad cells.

Strömungsraum_8:
top-down
I've decomposed one big block in several small blocks, deleted some and finally merged the small ones together again. 'Face to Surface' has provided me that result.

Could you tell me how I can get rid off the ugly cells in Strömungsraum_6?
What strategy is in that case the best?

My final goal is to simulate the heating element (solid) and the air (fluid) that is heated up by convection and radiation. So I will end up with two meshes. Do you know if I have to build two individual meshes or is it necessary to built both in the same model, if that is possible at all.


Aylalisa

I didn't follow this thread, so I would like to ask two questions:
1. Your both approaches are producing the problem elements?
2. Do you need solid blocks?

[Pospelov]

Hello everybody.
aylalisa. If it's geometry for CFD calculation I will do enouther blocks for this geometry. 1. You need boundary blocks. In attach file you can fine my solution.
The first errors was in black edges. The second in blocks.

[Far]

Originally Posted by Pospelov

Hello everybody.
aylalisa. If it's geometry for CFD calculation I will do enouther blocks for this geometry. 1. You need boundary blocks. In attach file you can fine my solution.
The first errors was in black edges. The second in blocks.

Better blocking. Well done.

Also check this blocking ...

[aylalisa]

A very big thank you for all your approaches!!!!
I will figure out now to see if I can follow!

I am happy !

Lisa

[aylalisa]

Originally Posted by Far

Angle > 34 deg
Quality > 0.5

Steps

1. One bigger block and o-grid. Delete inner block and associate edges to curves. Snap vertices.

2. Split at appropriate places (four along bigger pipe and two on two sides of smaller pipes).

3. Draw two curves through centre points in smaller pipes (see in attach files) and use extrude along curve option to extend blocking in smaller pipes and associate curves at the end of pipes and at intersection with larger pipe.

4. Make ogrid for smaller pipes. Select two blocks (one for smaller pipe and one in the larger pipe touching heating pipe and select two end faces)

5. Assign sizes on surfaces through part mesh setup (maximum size 3) and click on update all (blocking>edge mesh parameters> update all). And if necessary set the edge mesh parameters for the o-gird edges in the smaller pipes

genießen

There is still potential for mistakes that I always manage to make out.
May I ask you for detailed hints, especially according to the first three steps?

1. O-Grid
( ) without selection of top and bottom faces
( ) with selection of top and bottom faces
I've decided for the latter option.

Association:
outer edges of remaining blocks will be associated to outer circle
inner edges of remaining blocks will be associated to inner circle (center drill hole)

2. split at appropriate places
why 'four along bigger pipe'?
After 'snap vertices' it seems that there is only need for two splits along
bigger pipe?
--> screenshot
I understand 'two on two sides of smaller pipes'.

3. extrusions for smaller pipes
no problem with creation of two points,
no problem with creation of two curves,
BUT: I always receive an error message if I try the 'extrusion of faces'
--> screenshot
This also happend all the time during earlier attempts.

Why?

Finally I gave up to try using the extrusion command.
I use ICEM v14 on Windows 7

I thought I make some mistake but according to your description the usage of this command seems to be all right in this context.

Can anybody help???

Lisa

[Far]

1. Are you using extrude along curve option?

2. Are you selecting the correct face?

t seems that there is only need for two splits along
bigger pipe?

correct

I use ICEM v14 on Windows 7

So do I.

[aylalisa]

I've always tried the steps in the wrong order!

WRONG:
I've split the o-grid --> fine
I've tried to extrude faces before I've associated the edges to curve of small pipes

WORKING VERSION:
I've split the o-grid --> fine
I've associated the edges to curves (edges of new faces, generated by splits - curves of pipe)
then 'extrude faces' works

I really don't miss any chance to create problems .

Super!!!!

Viele Grüße
Lisa

[aylalisa]

Hello Far,

I got a really good result !

Could you tell me where the difference is between

a) right mouse button click on Pre-Mesh --> convert to Unstruct Mesh
and
b) Mesh > Compute Mesh > Volume Mesh > Hexa-Dominant > Compute

I will need a volume mesh which I can import in OpenFoam. OF makes a volume rendering with help of cell points. That should happen after correct conversion from, for example, a volume fluent mesh to OpenFoam. The volume rendering in OpenFOAM fails because the cell points are missing. Maybe I create the mesh in ICEM in the wrong way.

In the Output tab > Solver Setup there are three different Output Solvers listed up that contain 'fluent' in its name:
Ansys fluent
Fluent_V4
Fluent_V6


Do you know the difference between these solvers?

Viele Grüße
Lisa

[Far]

Originally Posted by aylalisa

Hello Far,

I got a really good result !

Could you tell me where the difference is between

a) right mouse button click on Pre-Mesh --> convert to Unstruct Mesh
and
b) Mesh > Compute Mesh > Volume Mesh > Hexa-Dominant > Compute

I will need a volume mesh which I can import in OpenFoam. OF makes a volume rendering with help of cell points. That should happen after correct conversion from, for example, a volume fluent mesh to OpenFoam. The volume rendering in OpenFOAM fails because the cell points are missing. Maybe I create the mesh in ICEM in the wrong way.

In the Output tab > Solver Setup there are three different Output Solvers listed up that contain 'fluent' in its name:
Ansys fluent
Fluent_V4
Fluent_V6


Do you know the difference between these solvers?

Viele Grüße
Lisa

Correct options are :

a) right mouse button click on Pre-Mesh --> convert to Unstruct Mesh
Ansys fluent

[Far]

Originally Posted by aylalisa

Hello Far,

I got a really good result !

Could you tell me where the difference is between

a) right mouse button click on Pre-Mesh --> convert to Unstruct Mesh
and
b) Mesh > Compute Mesh > Volume Mesh > Hexa-Dominant > Compute

I will need a volume mesh which I can import in OpenFoam. OF makes a volume rendering with help of cell points. That should happen after correct conversion from, for example, a volume fluent mesh to OpenFoam. The volume rendering in OpenFOAM fails because the cell points are missing. Maybe I create the mesh in ICEM in the wrong way.

In the Output tab > Solver Setup there are three different Output Solvers listed up that contain 'fluent' in its name:
Ansys fluent
Fluent_V4
Fluent_V6


Do you know the difference between these solvers?

Viele Grüße
Lisa

Hi Lisa

I saw one thread in Openfoam forum, where it is discussed in detail how to export mesh for OF from ICEM. Check it.http://www.cfd-online.com/Forums/ope...-openfoam.html

[Pospelov]

Originally Posted by Far

Better blocking. Well done.

Also check this blocking ...

Yes. This blocking is good too. And it's more easy to create it. ;-)