CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   Pointwise & Gridgen (http://www.cfd-online.com/Forums/pointwise/)
-   -   Volume mesh for Cyclone separator (http://www.cfd-online.com/Forums/pointwise/122503-volume-mesh-cyclone-separator.html)

Rajan August 21, 2013 06:06

Volume mesh for Cyclone separator
 
1 Attachment(s)
Hi Everyone,
I am very new to Pointwise and CFD in general and need to generate a three dimensional structured Volume mesh for cyclone separator as part of a university project.
I have imported the geometry from cad software and attempted a surface mesh by selecting domains on database entities.Now i want to generate volume mesh all over the region.
Any help or advice on how to approach this problem would be greatly appreciated
here i am posting the screen shot of the model.

cnsidero August 21, 2013 07:56

Structured or unstructured?

Unstructured, of course, would be straightforward.

Structured is a little trickier due to the inlet and the cyclone walls being tangent. The quality of the mesh in that region will be marginal because of the tangency.

Outline the type of mesh you want, any particular aspects you want (boundary layer, etc). and the solver you'll use and I'll give you more specific tips.

-Chris

Quote:

Originally Posted by Rajan (Post 447091)
Hi Everyone,
I am very new to Pointwise and CFD in general and need to generate a three dimensional structured Volume mesh for cyclone separator as part of a university project.
I have imported the geometry from cad software and attempted a surface mesh by selecting domains on database entities.Now i want to generate volume mesh all over the region.
Any help or advice on how to approach this problem would be greatly appreciated
here i am posting the screen shot of the model.


Rajan August 29, 2013 03:07

Thanx for the reply.....
 
Hi chris

I am using Fluent as solver.

mesh type - unstructured hexahedral mesh

Boundary layer aspects :-
1. First cell height = 0.5 mm
2. Growth rate= 1.2
3. No. of layers = 10

Rajan August 29, 2013 04:30

Hi chris

I am using Fluent as solver.

mesh type - unstructured hexahedral mesh

Boundary layer aspects :-
1. First cell height = 0.5 mm
2. Growth rate= 1.2
3. No. of layers = 10

cnsidero August 29, 2013 14:46

Quote:

Originally Posted by Rajan (Post 448678)
Hi chris

I am using Fluent as solver.

mesh type - unstructured hexahedral mesh

Boundary layer aspects :-
1. First cell height = 0.5 mm
2. Growth rate= 1.2
3. No. of layers = 10

Pointwise can not make unstructured hexahedral meshes. It's either structured (hexahedral) , unstructured (tets and prisms) or some combination of the two.

FYI, if you make a structured mesh in Pointwise and export it to Fluent, the mesh will then become unstructured within the mesh file but still requires structured techniques to build it within Pointwise.

It sounds like you might want to try unstructured tets with a prism boundary layer. Check the Pointwise tutorial workbook for the appropriate tutorial that covers this (I think it's the 747 nacelle one).

After the tutorial and you have questions about meshing your separator with this technique, don't hesitate to ask questions.

-Chris

Rajan September 5, 2013 03:01

Thnx
 
Hi chris,

The reason for hexahedral mesh requirement is that in swirl motion tetrahedral mesh is very diffusive and gives very inaccurate results.

as you told if i make a structured mesh in Pointwise and export it to Fluent, the mesh will then become unstructured within the mesh file but still requires structured techniques to build it within Pointwise.

please tell me which technique i should follow for structured (hexahedral) mesh with Boundary layer aspects.

1. First cell height = 0.5 mm
2. Growth rate= 1.2
3. No. of layers = 10

cnsidero September 21, 2013 14:46

2 Attachment(s)
Quote:

Originally Posted by Rajan (Post 449989)
Hi chris,

The reason for hexahedral mesh requirement is that in swirl motion tetrahedral mesh is very diffusive and gives very inaccurate results.

as you told if i make a structured mesh in Pointwise and export it to Fluent, the mesh will then become unstructured within the mesh file but still requires structured techniques to build it within Pointwise.

please tell me which technique i should follow for structured (hexahedral) mesh with Boundary layer aspects.

1. First cell height = 0.5 mm
2. Growth rate= 1.2
3. No. of layers = 10

Rajan,

Apologies for the slow reply. To create a structured mesh on cyclonic separate requires a little more than following a "technique".

If the separator is relatively simple in that it's essentially a body of revolution with the only attachment being a tangential inlet, I would suggest creating a structured 2D mesh of the cross-section and then revolve it, dealing with the inlet separately and then stitching the two regions together.

For a structured mesh, the difficult lies in dealing with the tangency of the inlet and body. I have yet to find a structured topology that completely eliminates all bad cells from this type of geometry (see attached images). If someone knows of a better one, please do tell.

Anyway, all the steps to make such a mesh is more than I'm willing to put in a post. Perhaps I will make a video tutorial of this.

lakhi October 16, 2013 15:08

Hi chris,

What I feel is that if we create mesh on a plane and then rotate it, bad quality (highly skewed tet) mesh is generated around the axis of rotation. Moreover, for cyclone, high cell skewness can never be eliminated due to the tangential nature of the inlet. If you happen to find out some solutions regarding this, please do share it.



Lakhi.

cnsidero October 17, 2013 08:35

4 Attachment(s)
Quote:

Originally Posted by lakhi (Post 457341)
Hi chris,

What I feel is that if we create mesh on a plane and then rotate it, bad quality (highly skewed tet) mesh is generated around the axis of rotation. Moreover, for cyclone, high cell skewness can never be eliminated due to the tangential nature of the inlet. If you happen to find out some solutions regarding this, please do share it.

Lakhi.

First, the cells on the axis wouldn't be tets, they would be wedges. Second, the resulting wedges would not necessarily be bad quality. In fact, I exported the mesh I showed in the picture and ran OpenFOAM's checkMesh on it. The only highly skewed cells were at the tangential location (where inlet becomes tangent with main cylinder wall) - none along the axis. Since you're using Fluent, I would expect this to be even less an issue since Fluent tends to be much less sensitive to mesh quality than OpenFOAM. Having said all that, if you were unhappy with this style of mesh you can relatively easily convert it from the O-type topology to an OH-type topology. See first 2 attached images.

I don't agree with your last comment. Completely eliminating the skewed cells at the inlet is tougher but not impossible. With structured meshes, it's generally about how much time you're willing to commit. I spent about 15 mins and came up with another solution for the topology at the inlet to eliminate the skewness. Checkout the before and after in the second 2 attached images.

Just a final note. Just because cells (quads, tris, hexes and wedges) are long and slender doesn't mean their skewness is bad. The shape is also important. Large aspect ratios are OK if one keeps the internal angles low. Notice, I didn't include tets. Slender tets often don't work well in most commercial solvers no matter their shape.

lakhi October 17, 2013 23:34

1 Attachment(s)
Dear Chris,

Thank you for making the things clear. If possible, please share complete video tutorial for cyclone meshing using pointwise (I have no idea how to stitch meshes also). It will be of great help to those who are dealing with cyclone. Image containing the section of (most of) the cyclone(s) is also attached.


Lakhi.

Rajan November 15, 2013 06:48

Hi
 
1 Attachment(s)
Hi chris,

i have tried with the structured 2D mesh of the cross-section.
but have no idea how to populate it. i need minimum spacing of 1 mm between the nodes.


here is the screen shot of geometry created in pointwise.

Rajan November 17, 2013 12:13

hi chris
 
1 Attachment(s)
The surface mesh on cross section is created by creating different domains with the help of connectors.

Now the rotation part is some what tricky.

Here is the screen shot

Rajan December 6, 2013 01:25

hi chris
 
4 Attachment(s)
Thnx for your support. i am able to generate a volume mesh by rotating the cross-section of structured surface mesh.

But after providing the boundary conditions to it when i import it in fluent, it shows in mesh display option the cross-section surface mesh as unspecified surface that is undesirable because i want to study the fluid flow inside the cyclone and i have provided boundary conditions to outer surfaces like (Inlet,outlet and rest of the surfaces as walls).

kindly suggest any solution. Here are the screen shots.

thnx

sarp April 28, 2014 14:13

Hi Chris,

>For the cyclone mesh, now I am trying to create a mesh using pointwise but I can not develop a meshing strategy for cyclone geometry. If the 2D section will be revolved, how can I match the grid with inlet and cyclone body?

cnsidero April 28, 2014 14:41

Quote:

Originally Posted by sarp (Post 488726)
Hi Chris,

>For the cyclone mesh, now I am trying to create a mesh using pointwise but I can not develop a meshing strategy for cyclone geometry. If the 2D section will be revolved, how can I match the grid with inlet and cyclone body?

Yes, this is the most difficult part of meshing a cyclone separator with a structured mesh. To answer your question specifically, refer to my comments and pics in the post #9 in this thread. That's one way to do it. The difficulty with this approach is dealing with the mesh cells where the inlet and cyclone body are tangent.

Of course, you could always try an unstructured mesh with prism inflation and will avoid all these difficulties.

-Chris

sarp April 28, 2014 16:58

Hi Chris, thank u for your quick feedback,

one of the strategy is revolution of 2D section as you mentioned at the previous post but I am trying to merge domains all together ignoring inlet domains, only the cyclone body but at last domains can not be sew together obtain block (volume mesh of interior). As I understood there are only two ways; one is assemble domains and the other one is assemble domains special in order to create structured block and there is no other way to assemble domains to form a structured block.

But when we revolve the 2D section about an axis how can we merge inlet to main cyclone body? Is there any specific way or some tricks that you may recommend?
thanks,

cnsidero April 29, 2014 14:40

Quote:

Originally Posted by sarp (Post 488761)
Hi Chris, thank u for your quick feedback,

one of the strategy is revolution of 2D section as you mentioned at the previous post but I am trying to merge domains all together ignoring inlet domains, only the cyclone body but at last domains can not be sew together obtain block (volume mesh of interior). As I understood there are only two ways; one is assemble domains and the other one is assemble domains special in order to create structured block and there is no other way to assemble domains to form a structured block.

But when we revolve the 2D section about an axis how can we merge inlet to main cyclone body? Is there any specific way or some tricks that you may recommend?
thanks,

You don't need to "merge" all the blocks together in Pointwise. The "merging" of the blocks is taken care of by CAE Volume Conditions*. For example, you have 5 structured blocks that represent 1 fluid region. You would create a CAE VC, assign all 5 blocks to it (give it a name and type). Finally, select the blocks and export them to the CAE type. The process of setting up a VC and exporting to the CAE type will create one unified mesh, even though it exists as 5 blocks in Pointwise.

* - some solvers have no notion of a volume condition. Therefore it is uncessary to create a VC and assign blocks to it. Simply selecting the blocks and exporting them to the CAE type will create a single unified mesh.

-Chris

pdp.aero May 4, 2014 05:38

4 Attachment(s)
Quote:

Originally Posted by Rajan (Post 447091)
Hi Everyone,
I am very new to Pointwise and CFD in general and need to generate a three dimensional structured Volume mesh for cyclone separator as part of a university project.
I have imported the geometry from cad software and attempted a surface mesh by selecting domains on database entities.Now i want to generate volume mesh all over the region.
Any help or advice on how to approach this problem would be greatly appreciated
here i am posting the screen shot of the model.

Hi ,

From what I had seen in your geometry picture, I am suggesting you three ways. I personally go for the third way, it will be more convenience.

1-For not losing orthogonality at the tangent portion of the channel's entry, you need to create unstructured block in the channel and create structured block in your body. For linking these blocks, you need to define grid interface. Because you are connecting unstructured block to structured block the grid interface will be non-conformal.

1-1 Create your structured block in the body which includes the structured tangent boundary at the entry from the channel (you can use revolve for creation or follow my way for structured block creation explained in the second way).

1-2 Split your tangent interconnection boundary from your structured body block

1-3 Go to the Create>Diagonalize>Initialize and select the split boundary. In this way you will have an unstructured surface mesh which matches exactly to you structured surface mesh at the entry.

1-4 Create your unstructured block in the channel which includes the unstructured tangent boundary at the entry to the body.

1-5 Set the boundary condition for the structured and unstructured tangent surface mesh to the interface.

1-6 Set two separate zone for your unstructured channel block and structured body block in the CAE>volume condition.

1-7 Go to the Fluent. From Define>Grid Interface. Create an interface between two zones. For this purpose, just select the tangent structured surface mesh at the entry from structured zone and tangent unstructured surface mesh at the entry from unstructured zone and type a name for it.

Note: Using grid interface means that you are creating hanging node and your cell value will be interpolated between zones.

2- I assumed that you are not supposed to define boundary condition at the interconnection between the channel and body. If it is true you may follow this way, otherwise you need to use the first way.

2-1 Divide the body into 3 parts. One part at the top, one at the bottom and the last one exactly fit to the interconnection's entry. After you divide your surface mesh, you will have four horizontal sections. One locates at the top, next at the top of the interconnection's entry, one at the bottom of the interconnection's entry, and the last one at the bottom of the body.

2-2 You will create your structured surface mesh at each horizontal section. First, you need to mesh the sections at the top and the bottom of the interconnection. For this please refer to the picture 1.

2-3 You will create your surface mesh for the section at the top of the body.

2-4 You will create your surface mesh for the section at the bottom of the body.

2-5 Define interface grid surface. Because the topology of the surface mesh at the top and bottom of the interconnection differ from the topology of the body you need to define non-conformal structured grid interface between mesh surfaces at the bottom. For this purpose, just mesh a circle that fits at the bottom section of the interconnection. Then, set the boundary condition of the surface mesh that covers each other to interface. Define a separate zone for the interconnection portion and bottom of your body in CAE>Volume condition. Go to the Fluent and then "Define>Grid Interface". Create an interface between domains that covers each other.

Note: For creating your structured mesh as described in picture 1, you need to use grid>solve, select Steger-Sorenson boundary control function and select float for inner connection, then iterate for 30 steps as an example.
For creating your structured mesh at the top and bottom sections as described in “1stway”, you need to define a diameter connector, split two edge connectors at the 25 and 75 percent of the length. Distribute your nodes on the edge, create your domain and run the solver.

3-For escaping from using non-conformal grid interface, there is another way. From this point, in the first way you need to create unstructured channel block by selecting the structured tangent surface and assemble your domain. In this way Pointwise will define a pyramid cells between the structured and unstructured block.

All the Bests,
Payam


All times are GMT -4. The time now is 02:39.