CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   ANSYS Meshing & Geometry (https://www.cfd-online.com/Forums/ansys-meshing/)
-   -   Meshing Sudden Contraction and Expansion (https://www.cfd-online.com/Forums/ansys-meshing/74024-meshing-sudden-contraction-expansion.html)

carldaru March 23, 2010 01:01

Meshing Sudden Contraction and Expansion
 
Hello,

I am trying to mesh a 2D sudden contraction and expansion using Gambit. However, I am not sure what type of meshing to use. Every type except "Quad Pave" keeps kicking up some sort of error for me. Either it's too skewed, or if I try using triangles, the triangles are too big, or I get a negative volume, etc. When I used "Quad Pave," the analysis that came out was not what was expected. Is it possible to mesh 2D figures that have a conical contraction and sudden expansion with plain cartesian meshes that literally go parallel and perpendicular to the length of the pipe in a perfect grid pattern (i.e. a 10 x 100 grid). If the perfect cartesian grid mesh is not possible, what type of meshing do you guys suggest I use? Also, do I just mesh the face or just the edges, or both?

Also, when I want to turn this into 3D, do I just do a revolve and then use the same type of mesh? Would that work, or is something else needed?

Thank you.

-mAx- March 23, 2010 01:56

you can control the mesh refinment with size functions.
In 2d I assume you can handle your problem with quads. (maybe you need to split your domain to achieve it)
you may post a picture.
Regarding 3d model, then you can revolve your faces, hex-cooper meshing schema should be enabled (just take care with face connectivity)

carldaru March 24, 2010 13:28

1 Attachment(s)
Quote:

Originally Posted by -mAx- (Post 251196)
you can control the mesh refinment with size functions.
In 2d I assume you can handle your problem with quads. (maybe you need to split your domain to achieve it)
you may post a picture.
Regarding 3d model, then you can revolve your faces, hex-cooper meshing schema should be enabled (just take care with face connectivity)

So by "size functions", I assume you are referring to the interval count/interval size controls? If I wanted a grid of say 10 x 100 (100 lines perpendicular to the length of the pipe), then would I select the edges appropriately and just type in 10 and 100?

When you say "split your domain", what are you referring to, and how does one go about doing that?

Once I get the 2D meshing down I will try the 3d model with the hex-cooper meshing. I assume face connectivity has to do with the splitting of the domain as referenced above? Am I correct in saying this?

A picture is posted with this message.

Thank you.

-mAx- March 25, 2010 02:55

1 Attachment(s)
In your case, just split your domain into logical and mappable surfaces.
See the picture (I just meshed one half (upper) side)
Attachment 2678

hassan79 April 13, 2010 13:02

need help
 
which turbulent model used can i have your mobile no

mk091088 January 2, 2017 13:03

Difficulty in cooper mesh hexahedral in sudden contraction
 
1 Attachment(s)
Hi everyone,
I am trying to model oil-water flow through two ducts, encountered a sudden contraction. I attached you my geometry. My intention is to inject oil in face 2 and water in face 1. It is very important to me to have a refined mesh near boundary. if i mesh the upstream pipe with tetrahedral and downstream with hexahedral mesh, everything goes well. however, when I want to use both pipe hexahedral mesh with defining boundary layer, Gambit cannot make it an error occurs regarding to source face. first, I defined two cylindrical geometry, then I split downstream pipe from face3. I meshed face 1 with refining and also face2.then I tried to sweep to these face (as sources) to the upstream pipe, but face 3 does not allow. any help would be appreciated.

mk091088 January 2, 2017 13:10

difficulty in creating cooper mesh in sudden contraction
 
1 Attachment(s)
I also attached you the error associated with cooper mesh.

-mAx- January 4, 2017 02:14

you need to split your domain,
Split it at face 3
Then split the cylinder which contains faces 1 & 2 in 2 concentric cylinders.
The common diameter from those 2 cylinders will be non-constant (use the intermediate edges from face 1 & 2 to create the surface split)

mk091088 January 4, 2017 07:41

1 Attachment(s)
Thank you Max for your response.
I did not understand what you said about concentric cylinders. Let's consider upstream pipe as volume 1, and downstream as volume 2. As you said, I split volume 1 from face 3 to create face 4 so that I am able to define face 3 and 4 as interior and wall, respectively.
You said ''Then split the cylinder which contains faces 1 & 2 in 2 concentric cylinders''. The faces 2 and 3 do not have the same diameters. The faces 2 and 3 have the diameters 15 mm and 21 mm, respectively. Honestly, I did not get what you said about spliting volume 1 into two concentric cylinders.

-mAx- January 4, 2017 08:13

1 Attachment(s)
Quote:

Originally Posted by mk091088 (Post 631969)
I am able to define face 3 as interior

you don't need to set it as interior since it will automatically done

Regarding the split I mentionned, create an edge from both vertices as mentionned in the picture
Attachment 52987

Once it is done, split each circular edge in its middle and create another straight edge.

Now you can create the conical surface with help from both straight edges and 2 semi-circles.

Split the volume with the conical surface

It should do the job

mk091088 January 4, 2017 15:13

1 Attachment(s)
As I mentioned before, I want to model two phase flow in contraction pipe. Thus, the transport equation in volume 1 must be solved for mixture (1 fluid). The method that you suggested is perfect, but I am curious because creating the conical surface would create an extra surface inside the volume 1 (there are two volumes in volume 1 which included the annular between wall and conical surface and another inside the conical surface), and definitely it should not be wall and it must be interior, according to my physical problem. I focused first on volume 1, I was properly able to separate face 1 from 2 and face 3 from face 4. Furthermore, I created two semi-circles on face 1 and face 3 and two straight edges as you said. but I do not know how to make a conical surface. It must be two semi-conical surfaces and then should be united, right?
Sorry to ask you two many questions, I am new to Gambit.

-mAx- January 4, 2017 15:18

If you split the volume as I described, don't set anything on the conical surface.
Fluent will treat it as interior.
So it will understand you only have 1 fluid volume.
(the split is only here for enabling you a full hex mesh)

In your picture delete your 2 straight lines, and create 2 new ones using the vertex (already existing)

mk091088 January 4, 2017 15:34

1 Attachment(s)
Thank you. I do know if it is true. Please verify. I deleted previous edges, and created two straight edges with vertexes and I used two semi-circle on two different edges and two straight lines to create one conical surface as you said. I used Geometry/Face/Wireframe.

-mAx- January 4, 2017 15:37

yes
now check if topology is proper by meshing this surface (map)
it will give you a good idea (sometimes Gambit creates disturbed topology )

If it is correct, do the same with the other surface. And finally split the volume with those 2 surfaces

mk091088 January 4, 2017 16:13

3 Attachment(s)
I meshed the conical surface with mapped mesh, it is ok. Thus, I start meshing the domain. first I created a boundary layer for annulus in face 1, then I used a mappable quad for face 1. I used a paved quad mesh for face 2. For volume mesh, I still have problem because when I swept all the surface meshes face 1 and 2 through the domain by cooper mesh, the edges (which was used to create conical surfaces) does mot allow to mesh the volume properly. Moreover, the pannel related to source faces is deactivated and I needed to define manually which I do not know which source face I must use. It is worth noting that I did not unit two semi-conical surfaces before meshing.

-mAx- January 4, 2017 16:21

first don't use (yet) any BL

delete all mesh
Mesh one annulus face with quad
Mesh the conical face with quad
Mesh the volume (annulus), enforce the cooper scheme if necessary by picking both annulus surfaces as source.
If you still have problems, I will check it when I go back to the office (monday)

mk091088 January 4, 2017 17:37

It is done. some important points to be addressed: I did what you said with interval count=42 for faces and volumes. here are the results of meshes:

For volume 1 (annulus)=21,168
For volume 1 (conical volume)=26,586
For volume 2=322,197

I do not know why there is a significant difference between upstream and downstream mesh in terms of the quantity with the same interval count.
Most importantly, I still need to apply boundary layers to my walls in volumes 1 and 2.

-mAx- January 4, 2017 19:06

If your volumes are well meshed (good quality); save your *.dbs file and add the BL.


Sent from my iPhone using CFD Online Forum mobile app

mk091088 January 5, 2017 08:25

2 Attachment(s)
These are final questions, Max:

1)Boundary layers must be added to faces 1 and face 3 at the inlet and the point of singularity, right? In this case how boundary layer can be swept all along the wall inside the volumes? I mean the boundary layer can be only applied to specific faces not the whole volume.

2)After adding boundary, should I export mesh, right?

3)The second question is regarding the difference between the number of elements in volume 1 and 2. Why there is so much difference. According to your method (Upstream pipe, volume 1 is so coarse and downstream is fine). The mesh quality, however, is good.

-mAx- January 5, 2017 08:42

1) No. BL have to be attached to the walls
2)Once BL have been created, remesh the volumes to be sure that BL are included in the volume mesh.
Once it is checked (examine mesh), you can export the mesh
3)check the node distribution along the axis of the volume with higher cells number.
The cells distribution in the section is given because of the first volume (annular and conical)


All times are GMT -4. The time now is 04:42.