CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   ANSYS Meshing & Geometry (http://www.cfd-online.com/Forums/ansys-meshing/)
-   -   CHT - interface regions? (http://www.cfd-online.com/Forums/ansys-meshing/67895-cht-interface-regions.html)

rogbrito August 30, 2009 08:24

CHT - interface regions?
 
Hi:confused:,

i want to create the hexahedrical mesh on this geometry (http://www.4shared.com/file/71710815...8_SW_2006.html
). How to do that? I don´t know how to make the 2D interface regions, among the solids (fins) and the fluid (air) inside the cubic cavity.

Thanks.

Others meshes of mine:

http://www.4shared.com/file/57934957...111111111.html
http://www.4shared.com/file/71167794...hexa_mesh.html
http://www.4shared.com/file/70268973..._Mr_Brito.html
http://www.4shared.com/file/11759512...rito_2009.html
http://www.4shared.com/file/57352579..._1st_2008.html
http://www.4shared.com/file/70335966..._by_Brito.html
http://www.4shared.com/file/58521065...r2Dregion.html
http://www.4shared.com/file/55934769...008_Brito.html
http://www.4shared.com/file/55730476...ly18_2008.html
http://www.4shared.com/file/55948235...July_2008.html
http://www.4shared.com/file/67475430...R_A_Z_I_L.html
http://www.4shared.com/file/67653540..._aplicado.html
http://www.4shared.com/file/65772301..._Mr_Brito.html
http://www.4shared.com/file/94218856...des_Brito.html
http://www.4shared.com/file/10301785...009_Brito.html
http://www.4shared.com/file/94665973...march2009.html
http://www.4shared.com/file/65770211..._Mr_Brito.html
http://www.4shared.com/file/52225485...com2RevOK.html
http://www.4shared.com/file/68085677.../Femlab1D.html
http://www.4shared.com/file/80227608...ical_Mesh.html
http://www.4shared.com/file/68472455...Benchmark.html
http://www.4shared.com/file/58440306...transient.html
http://www.4shared.com/file/52194930...rogeriow1.html
http://www.4shared.com/file/52205921...rogeriow2.html
http://www.4shared.com/file/52185334...rogeriow3.html
_mesh_28_11_2008.html

PSYMN August 31, 2009 09:29

Naturally...
 
I didn't actually open your model since I don't have solid-works... Often attaching a quick image would be better than sending the models.

You don't specifically mention ICEM CFD Hexa, but I will assume...

If you want node for node connections, just block it all at once. Create a fluid material and start the blocking with that. Create a second material for the solid region and right click on that material for "add to part", make sure you are selecting blocks (not geometry or mesh) and select the blocks in the blades. ICEM CFD Hexa will handle the rest automatically.

If it is difficult to block at once, you can block separately and merge the blocking topologies... Ask if you need more details on that.

If you are working with ANSYS Meshing (Workbench), then you need to go into DM and make these two parts into a multi-body part so it will maintain node for node connections.

If you are not interested in node for node, but just want to interpolate for CHT, then that would be a different question, more solver based then mesher...

rogbrito August 31, 2009 11:28

Hi Mr. Pereira :),

I´m using ANSYS ICEM CFD 12 software. I found very difficult to do that. I spent around 10 hours to do this (a cavity and one fin only). I did a cavity with only a fin, but it didn´t work out at ANSYS CFX Pre. I will intend to use ANSYS CFX 12 to compute the wall (or external) heat transfer coefficient h [W m^-2 K^-1], on the top of the fin. The files are in:


http://rapidshare.de/files/48255799/cavity_with_one_a_fin_Problems_at_CFX_Brito_2009.r ar.html

(Size: 21,102 KB)


Is there another way to do that (this hexahedrical mesh), without as such difficults?


Thanks for you attention,

Rogerio.

Quote:

Originally Posted by PSYMN (Post 228022)
I didn't actually open your model since I don't have solid-works... Often attaching a quick image would be better than sending the models.

Quote:

Originally Posted by PSYMN (Post 228022)

You don't specifically mention ICEM CFD Hexa, but I will assume...

If you want node for node connections, just block it all at once. Create a fluid material and start the blocking with that. Create a second material for the solid region and right click on that material for "add to part", make sure you are selecting blocks (not geometry or mesh) and select the blocks in the blades. ICEM CFD Hexa will handle the rest automatically.

If it is difficult to block at once, you can block separately and merge the blocking topologies... Ask if you need more details on that.

If you are working with ANSYS Meshing (Workbench), then you need to go into DM and make these two parts into a multi-body part so it will maintain node for node connections.

If you are not interested in node for node, but just want to interpolate for CHT, then that would be a different question, more solver based then mesher...


PSYMN September 1, 2009 17:14

One Blocking, 2 materials.
 
5 Attachment(s)
Hello…

So I took a few minutes to check this out…

I saw a very simple blocking, basically a box in a box. I guess you wanted the conjugate heat transfer between these. I am guessing the larger box was the Socket (CAVIDADE_ and the smaller box was the Wing (ALETA).

However, these were not node for node connected… If you want a mesh independent CHT, then talk to the solver people.

If you want these node for node connected, just block them together…

I took your blocking file and reduced the index control so that I could see just the plane with the inner box missing. Your blocking was very strange for such a simple model (I guess you permanently deleted all the vorfn blocks at one point), so this was O4, but with a simple Hgrid blocking, it would have just been J. I had planned to just restore that inner block to the ALETA part and be done with it, but since this was fairly ugly (see first pic), I just decided to quickly re-block (just a couple minutes for this model).

While reblocking, I used “Add to part => Blocking Material” to select the middle block and put it into the ALETA part. This creates a single blocking with 2 materials. (see other pics)

You don’t need two super imposed interface surfaces in one model. That can only confuse the mesh. I recommend deleting one set.

Done.

I am attaching the blocking and the 4 pics.



If I am answering the wrong question, please restate...

rogbrito September 1, 2009 18:10

Hi Pereira,

Why did you say this:

"... You don’t need two super imposed interface surfaces in one model...."

On the AEA CFX-v5.6, i didn´t need to build these 2D interface regions. Since CFX version 10, i´ve got to build them. If i have two domains (solid plus air)...

And how about the 1:1 interfaces in CFX-Pre?
You sent me the block file made by you. Is this correct now?

Thanks (a lot) for your answer.

Rogerio.

Quote:

Originally Posted by PSYMN (Post 228165)
Hello…

So I took a few minutes to check this out…

I saw a very simple blocking, basically a box in a box. I guess you wanted the conjugate heat transfer between these. I am guessing the larger box was the Socket (CAVIDADE_ and the smaller box was the Wing (ALETA).

However, these were not node for node connected… If you want a mesh independent CHT, then talk to the solver people.

If you want these node for node connected, just block them together…

I took your blocking file and reduced the index control so that I could see just the plane with the inner box missing. Your blocking was very strange for such a simple model (I guess you permanently deleted all the vorfn blocks at one point), so this was O4, but with a simple Hgrid blocking, it would have just been J. I had planned to just restore that inner block to the ALETA part and be done with it, but since this was fairly ugly (see first pic), I just decided to quickly re-block (just a couple minutes for this model).

While reblocking, I used “Add to part => Blocking Material” to select the middle block and put it into the ALETA part. This creates a single blocking with 2 materials. (see other pics)

You don’t need two super imposed interface surfaces in one model. That can only confuse the mesh. I recommend deleting one set.

Done.

I am attaching the blocking and the 4 pics.



If I am answering the wrong question, please restate...


PSYMN September 2, 2009 11:10

Take it one more step...?
 
If you create two surfaces and then one mesh with coincident nodes, there will only be one layer of elements between the volume regions. That is the interface... Having two surfaces just confuses the issue. You never send surfaces to CFX, you send mesh.

If you want to mesh this as two separate models, with or without coincident nodes, then that is a different question... I was working with the assumption that you wanted conformal nodes.

I am not a CFX expert, so you need to tell me what you need. Let’s see if one wants to comment here (or ask your question over in that area of the forum).

In the mean time, assuming you are right, let’s take it one more step and split these interface nodes into two.

Starting from my previous blocking file which only gives one layer between the volumes, generate an unstructured mesh.

Then go to Edit Mesh => Split Mesh => Split Nodes. Use the selection toolbar to select the elements in your interface part.

This splits the interface elements in two. One set are attached to the socket volume, the other to the wing volume. But the interface surfaces attached to each body have a common name. This may be enough for CFX, but if not, here is how you change the name on one side;

Use the subset tool to select either one volume element or one shell element near this area (but not on the interface.) Then modify the subset to add some layers (not volume elements)… You will see that since the nodes are split, it will only add one side of the interface… Then you can select those elements and add them to the other interface part…


In the mean time, assuming you are right, lets take it one more step and split these interface nodes into two.

rogbrito September 2, 2009 11:25

Hi. PSYMN,

I will read with care.

I thank you kindly!

Rogerio.

Quote:

Originally Posted by PSYMN (Post 228296)
If you create two surfaces and then one mesh with coincident nodes, there will only be one layer of elements between the volume regions. That is the interface... Having two surfaces just confuses the issue. You never send surfaces to CFX, you send mesh.

If you want to mesh this as two separate models, with or without coincident nodes, then that is a different question... I was working with the assumption that you wanted conformal nodes.

I am not a CFX expert, so you need to tell me what you need. Let’s see if one wants to comment here (or ask your question over in that area of the forum).

In the mean time, assuming you are right, let’s take it one more step and split these interface nodes into two.

Starting from my previous blocking file which only gives one layer between the volumes, generate an unstructured mesh.

Then go to Edit Mesh => Split Mesh => Split Nodes. Use the selection toolbar to select the elements in your interface part.

This splits the interface elements in two. One set are attached to the socket volume, the other to the wing volume. But the interface surfaces attached to each body have a common name. This may be enough for CFX, but if not, here is how you change the name on one side;

Use the subset tool to select either one volume element or one shell element near this area (but not on the interface.) Then modify the subset to add some layers (not volume elements)… You will see that since the nodes are split, it will only add one side of the interface… Then you can select those elements and add them to the other interface part…


In the mean time, assuming you are right, lets take it one more step and split these interface nodes into two.



All times are GMT -4. The time now is 01:02.