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/)
-   -   [ANSYS Meshing] o-grid generation in ANSYS MESHING (http://www.cfd-online.com/Forums/ansys-meshing/106879-o-grid-generation-ansys-meshing.html)

diamondx September 11, 2012 10:14

o-grid generation in ANSYS MESHING
 
I wanna generate a structured mesh in a tube using ANSYS MESHING.
Using the sweep method or Multizone.
for an o-grid, i need to slice the geometry following the picture below:
http://www.cfd-online.com/Forums/att...ubes-ogrid.jpg

How to slice it like that. do i need to go back to designmodeler, and create the square in the middle with the edges then go back to the meshing software ?
Is there another way for that ?

Thanks !!

PSYMN September 12, 2012 09:01

1 Attachment(s)
In ANSYS Meshing, MultiZone figures out the volume subdivision for you...

It just needs you to ask for Inflation layers.

After setting up the MultiZone method...

Left Click on the Mesh Branch to view its Details Panel...

Under "Inflation", set "Use Automatic Inflation" as "Program Controlled"...

This option basically just assumes that you don't want Named Selections inflated (Not INLET, OUTLET, SYMMETRY, etc.) and that most people don't bother putting their walls in Named selections... It works for me because I have the flat ends as my inlet and outlet. If you have a named selection or some other way you want to select the surfaces to be inflated, you can choose "All Faces In a Named Selection". Unfortunately, you can not use "Insert => Inflation" with Multizone because it requires a global definition.

Attachment 15701

One other catch, if your mesh comes out looking swept, you just need to take better control over the mapping using some of the multizone controls...

diamondx September 12, 2012 12:17

Thanks Simon for your reply.
I had to add the mapped face meshing and select the inlet and outlet to get the same elements as yours. below are the some screenshots with and without the face mapped meshing.
https://dl.dropbox.com/u/35161486/with_face_mapping.png

Without face mapped meshing:

https://dl.dropbox.com/u/35161486/wi...ce_mapping.png

May be because of length of the tubes ??? I have one more question, I have version 13, and i just got into ansys meshing, when i tried to get like your mesh, i tought that maybe it's because you have version 14. so i tried it on another pc here in the lab , result was same, but i got into one interesting feature which is the ICEM CFD override , i tried that and i discovered that i can actually mesh it in icem interactively... that was just amazing... so i also discovered that i can create material bodies like in ICEM CFD. that means i don't have to extract an volume of fluid...

If this tube is inside a complicated heat exchanger for example (Because i'm working on one actually), i can combine a hexa mesh in the tube (blocked with icem) and a tetra mesh using material point in ansys meshing... it's something that ICEM CFD CAN'T DO (unless you use non-condormal mesh). are my assumptions correct ? this is what i was trying to do yesterday in icem without successful result even with multizone. So may be it's more easy with ansys meshing ?

Thanks a lot for you answers...

PSYMN September 12, 2012 12:40

It is easy to go from ANSYS Meshing to ICEM CFD... The trick is getting back again. ANSYS Meshing is really picky about the geometry and mesh connection. If you change any of the geometry in ICEM CFD (part names, add a curve, anything), the mesh will not go back...

This option to mesh in ICEM CFD gets better every release. 14.5 is much better than 13.0.


In ANSYS Meshing, you can not combine the concepts of "Assembly Meshing" which uses a material point, and Part by Part meshing methods like MultiZone.

However, we are working on a way to have assembly meshing (material point PI meshing) within specified Mulizone Blocks... Which will be very cool.

In ICEM CFD, you can do this sort of thing, but you need to use "merge mesh".

Many people just use a non conformal mesh and join things in the solver.

diamondx September 12, 2012 12:56

Ok... Until then i'll choose what's best for me.
still it's great to have this interoperability...
Thanks, thanks a lot.

Far September 12, 2012 13:00

Your comments are worth reading the help files ten times. :D

Quote:

Originally Posted by PSYMN (Post 381450)
It is easy to go from ANSYS Meshing to ICEM CFD... The trick is getting back again. ANSYS Meshing is really picky about the geometry and mesh connection. If you change any of the geometry in ICEM CFD (part names, add a curve, anything), the mesh will not go back...

This option to mesh in ICEM CFD gets better every release. 14.5 is much better than 13.0.


In ANSYS Meshing, you can not combine the concepts of "Assembly Meshing" which uses a material point, and Part by Part meshing methods like MultiZone.

However, we are working on a way to have assembly meshing (material point PI meshing) within specified Mulizone Blocks... Which will be very cool.

In ICEM CFD, you can do this sort of thing, but you need to use "merge mesh".

Many people just use a non conformal mesh and join things in the solver.


PSYMN September 12, 2012 16:23

@Far...

Except that I often help the doc team write the Help files :o

martyn88 September 14, 2012 03:18

2 Attachment(s)
Hi Psymn and diamondx. I have a problem that is similar to that explained by diamondx. I wish to create a structured grid for use in a LES simulation.

However my geometry is slightly more complicated than a simple pipe. My domain is a converging-diverging nozzle surrounded by ambient fluid (see below pictures):

Attachment 15747

I really can't afford to model the entire geometry so I am hoping to only model a section (1/8 or 1/4) with periodic side boundaries.

Originally I swept a 2-D grid through the wedge but the cells near the centreline were tet prisms with very high aspect ratio, and were affecting my solution. Therefore I need to use an O-grid.

I tried following your steps above but ran into some problems when trying to mesh the wedge region:

Attachment 15746


Is there a way of creating a more symmetrical mesh on the wedge face? Also what is the best way to refine it? Can I specify edge sizings?

Thanks,

Hugh

PSYMN September 14, 2012 09:04

You can select any geometry edge, right click => Insert => Sizing. You can set the element size or you can set a "number of divisions" with a bias, etc.

For something like a 30 degree wedge, MultiZone doesn't really give you a way to create a quarter OGrid automatically. You could go to ICEM CFD and mesh this model with all the control you could ever want (and some learning curve) or you could figure out how to slice the model in DM...

Sorry, I am not really very expert at slicing in DM and don't have time to try it out to be sure I am giving you the right info ;^)

diamondx September 14, 2012 09:27

there you go, made in Icem:
https://dl.dropbox.com/u/35161486/LES.png
Here is the project file:
https://dl.dropbox.com/u/35161486/LES.zip

diamondx September 14, 2012 09:37

Here is a small video on how to do that :
http://youtu.be/InyeCmEuUVM

Far September 14, 2012 13:54

Quote:

Originally Posted by diamondx (Post 381801)
there you go, made in Icem:
https://dl.dropbox.com/u/35161486/LES.png
Here is the project file:
https://dl.dropbox.com/u/35161486/LES.zip

similar thread ;) http://www.cfd-online.com/Forums/ans...tml#post381851

martyn88 September 16, 2012 05:23

Wow thankyou so much Ali, you have been a massive help! I will have a play around in ICEM tomorrow and try and get my head around it. You have given me a big head start though :)
Really appreciate it.

Hugh

PSYMN September 20, 2012 16:57

Hey DiamondX, FAR or anyone else who wants to make a video...

If you would like to share it with a larger audience, please email your youtu.be link to "social@ansys.com" and tell them they are welcome to post it in the user generated content area of the ANSYS youtube site. If it is a technical demo, ask them to put it under tech tips. ANSYS can hit the "like" button and add it to their favorites so it shows up on the ANSYS channel. Of course, there is no guarantee they will like your video ;^).

One other thing, please make sure that the description of your video clearly states what the demo shows so that people can find the right ones...

Far September 21, 2012 01:33

Quote:

Originally Posted by PSYMN (Post 382854)
Hey DiamondX, FAR or anyone else who wants to make a video...

If you would like to share it with a larger audience, please email your youtu.be link to "social@ansys.com" and tell them they are welcome to post it in the user generated content area of the ANSYS youtube site. If it is a technical demo, ask them to put it under tech tips. ANSYS can hit the "like" button and add it to their favorites so it shows up on the ANSYS channel. Of course, there is no guarantee they will like your video ;^).

One other thing, please make sure that the description of your video clearly states what the demo shows so that people can find the right ones...

Fantastic. ;)

Omish June 25, 2016 06:31

Quote:

Originally Posted by diamondx (Post 381445)
Thanks Simon for your reply.
I had to add the mapped face meshing and select the inlet and outlet to get the same elements as yours. below are the some screenshots with and without the face mapped meshing.
https://dl.dropbox.com/u/35161486/with_face_mapping.png

Without face mapped meshing:

https://dl.dropbox.com/u/35161486/wi...ce_mapping.png

May be because of length of the tubes ??? I have one more question, I have version 13, and i just got into ansys meshing, when i tried to get like your mesh, i tought that maybe it's because you have version 14. so i tried it on another pc here in the lab , result was same, but i got into one interesting feature which is the ICEM CFD override , i tried that and i discovered that i can actually mesh it in icem interactively... that was just amazing... so i also discovered that i can create material bodies like in ICEM CFD. that means i don't have to extract an volume of fluid...

If this tube is inside a complicated heat exchanger for example (Because i'm working on one actually), i can combine a hexa mesh in the tube (blocked with icem) and a tetra mesh using material point in ansys meshing... it's something that ICEM CFD CAN'T DO (unless you use non-condormal mesh). are my assumptions correct ? this is what i was trying to do yesterday in icem without successful result even with multizone. So may be it's more easy with ansys meshing ?

Thanks a lot for you answers...

Hi
I want to make exactly the mash you made, but my geometry is a little different. As you see I have a 90 degree bend (made by "revolve").
2 problems:

1- when I use face meshing it doesn't appear as a "Mapped Face Meshing" although I made the square and 4 lines in the middle (by using Tools>splite face), and in the setting for face meshing, the "mapped" option is set as "yes". how did you exactly made it that way?

2- when I insert a mesh method as "multizone" it first gave me an error, something like: could not automatically find source. Then I manually added it (in the picture in RED color. again it gave a new error which you can see in the same picture: "Multizone found free blocks in swept body"
Please help me with this.


my automatic mesh with Inflation ( not what I want, too messy)
https://i.imgsafe.org/e5bdff2922.png

This is face I chose for Mapped face mesh, Which doesn't actually turn out as "MAPPED face mesh"
https://i.imgsafe.org/e5c77ee88d.png

the error with "Multizone Method" after selecting SOURCE manually.
https://i.imgsafe.org/e5ca4e4878.png


All times are GMT -4. The time now is 15:04.