CFD Online URL
[Sponsors]
Home > Forums > ANSA

ANSA 2D Meshing?

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   March 24, 2012, 12:10
Default ANSA 2D Meshing?
  #1
Member
 
Join Date: Jun 2011
Posts: 48
Rep Power: 5
eishinsnsayshin is on a distinguished road
Hello All,
This might sound like a stupid question. I'm an undergrad who has co-oped in the automotive industry doing CFD. I've used ANSA for lots of 3D meshing. For school projects, is there any way ANSA can be used to mesh for a 2D problem (like flow over a 2D airfoil)? I was thinking about it and I'm not sure how I would do that...The ANSA I'm familiar with is only 3D...is there a 2D version or something?

Thanks for any help!
eishinsnsayshin is offline   Reply With Quote

Old   March 26, 2012, 12:06
Default
  #2
Member
 
Join Date: Jun 2011
Posts: 48
Rep Power: 5
eishinsnsayshin is on a distinguished road
OK, so I figure no one has responded because I'm not specific enough or something. That's usually the case. Let me try something else:

Let's say I have a circular surface (cross section of a cylinder) floating in space that I want to run a simulation in fluent around. So I make a circle in ANSA in the x-z plane. I then make a rectangular surface for the domain in the same plane around the circle. I mesh both surfaces, so everything is still just in the x-z plane.

Now I don't know what to do. To use 2D FLUENT, do I extrude these two surfaces in the Y direction by one step (using volumes>extrude), then use elements>vol-shel along the outer boundaries to make shells for an inlet, and the outlets to assign PID's? I can't get the .msh file to read into FLUENT.

The other option is to use trasf.>copy and make a duplicate translated copy some distance in the y direction. Then close the surface using surf>coons or something, then do a volume mesh for the inside and create an STL, but this doesnt seem to work either. Any ideas? I would imagine someone out there has probably done something like this! How do you create something 3d in ANSA be able to be read in 2D fluent?

Thanks!
eishinsnsayshin is offline   Reply With Quote

Old   March 27, 2012, 05:01
Default
  #3
Senior Member
 
Vangelis Skaperdas
Join Date: Mar 2009
Location: Thessaloniki, Greece
Posts: 160
Rep Power: 8
vangelis is on a distinguished road
Hi there,

In order to prepare a model in ANSA for Fluent 2D
you need first of all to draw your model in
XY plane (not along Z axis).

For a flow past a cylinder example, you need to
draw a rectangular domain and in it the circle which you will Project and cut on the domain.
You will delete the Face inside the circle and mesh the outer with a nice ADV.FR or CFD mesh.

You should activate the FLUENT 2D Deck in ANSA
so that you can also assign the Boundary Conditions along the boundary CONS. Please refer to section 23.3.3 of the ANSA Users Guide.

Let me know if there is a problem.
Best regards
Vangelis
vangelis is offline   Reply With Quote

Old   March 27, 2012, 18:27
Default
  #4
Member
 
Join Date: Jun 2011
Posts: 48
Rep Power: 5
eishinsnsayshin is on a distinguished road
Hey thanks for the reply, I got everything working now!
eishinsnsayshin is offline   Reply With Quote

Old   March 28, 2012, 08:10
Default
  #5
Senior Member
 
Vangelis Skaperdas
Join Date: Mar 2009
Location: Thessaloniki, Greece
Posts: 160
Rep Power: 8
vangelis is on a distinguished road
glad it worked for you
vangelis is offline   Reply With Quote

Old   August 26, 2013, 11:55
Default
  #6
New Member
 
Join Date: Aug 2013
Posts: 3
Rep Power: 3
marios is on a distinguished road
Hi,

I followed the same steps in order to create a 2d car, and it worked for me as well. I have managed to read successfully the model in Fluent.
However, I don't know how to create inflation layers, because the Volume>Layers will create layers in the Z direction.

Any help would be appreciated.
marios is offline   Reply With Quote

Old   August 27, 2013, 04:17
Default
  #7
Senior Member
 
Vangelis Skaperdas
Join Date: Mar 2009
Location: Thessaloniki, Greece
Posts: 160
Rep Power: 8
vangelis is on a distinguished road
Hi Marios,

You can use the function SHELL MESH>ZONECUT GRADUAL
to generate layers in 2D, available in ANSA v14.x

Vangelis
vangelis is offline   Reply With Quote

Old   August 27, 2013, 06:04
Default
  #8
New Member
 
Join Date: Aug 2013
Posts: 3
Rep Power: 3
marios is on a distinguished road
Hi Vangelis,

thanks for the quick reply.
I have ANSA v13.2.2. I used SHELL MESH>ZONE CUT, and for the Mesh Parameters I chose: "General" Mesh with "Quad" elements and created high aspect ratio elements. However, I am not sure about the quality of my layers. Do you think there is a better approach?

Marios
Attached Images
File Type: jpg car2d_1.jpg (64.6 KB, 19 views)
File Type: jpg car2d_2.jpg (54.1 KB, 13 views)
marios is offline   Reply With Quote

Old   August 27, 2013, 06:39
Default
  #9
Senior Member
 
Vangelis Skaperdas
Join Date: Mar 2009
Location: Thessaloniki, Greece
Posts: 160
Rep Power: 8
vangelis is on a distinguished road
Hi Marios

The function I suggest is only available in v14.x

If you have to work in v13.x then your alternative is to work
in TOPO menu, use FACEs>ZONECUT to make an all around
cut at the distance of the total layers height.

Then make some normal cuts and then mesh with MAP
mesh these areas.

You should also use PERIMETERs>SPACING to define the
mesh distribution in the layers zone

Hope this helps

Vangelis
vangelis is offline   Reply With Quote

Old   August 27, 2013, 18:29
Default
  #10
New Member
 
Join Date: Aug 2013
Posts: 3
Rep Power: 3
marios is on a distinguished road
Hi Vangelis,

your reply was very helpful. I struggled, but I managed to make a good mesh.

Best regards,
Marios
marios is offline   Reply With Quote

Old   August 28, 2013, 02:56
Default
  #11
Senior Member
 
Vangelis Skaperdas
Join Date: Mar 2009
Location: Thessaloniki, Greece
Posts: 160
Rep Power: 8
vangelis is on a distinguished road
Hi Marios,

Glad it worked for you.

Have in mind that if you upgrade to the current ANSA version, v14.
then 2D layers generation will be much easier as the function
MESH>SHELL MESH>ZONECUT Gradual does exactly this.

Best regards

Vangelis
vangelis is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
ANSA hexblock mesh to OpenFOAM yosuu OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 7 October 22, 2011 07:18
Best Meshing scheme for Cylinder Nutrex Main CFD Forum 4 July 29, 2008 12:03
Meshing locks workbench window. andy2o CFX 0 February 1, 2008 06:01
Singularity of grid?Volume meshing vs face meshing Ken Main CFD Forum 0 September 4, 2003 12:09
Volume Meshing & Face Meshing? singularity of grid ken FLUENT 0 September 4, 2003 12:08


All times are GMT -4. The time now is 19:35.