CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > ANSA

ANSA mesh for sliding meshes (pimpleDyFoam

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

Reply
 
LinkBack Thread Tools Display Modes
Old   July 11, 2014, 09:19
Default ANSA mesh for sliding meshes (pimpleDyFoam
  #1
New Member
 
Join Date: Nov 2010
Posts: 9
Rep Power: 6
yosuu is on a distinguished road
Dear users,

I was wondering if you could give me some tips/"best practices" to create a mesh for OpenFOAM with a cylindrical interface where a fan lies in it. I have used the this method:

- I meshed everything and define the interface as baffles, then exported to OpenFoam case. Then in the polyMesh/boundary I change manually the baffles patches to cyclicAMI type. I use then the pimpleDyMFoam solver for the simulation, it works perfectly when I start from 0, but then if I write the solution and I restart the simulation, it is not possible due to some error in the interpolation between the faces. (this is due to the following: when I export the mesh to openfoam, the faces of the two patches that baffles creates share the same points instead of one duplicating these points, so writing the solution with the moved mesh does not modify the points of the patches but the points of the cells inside the moved mesh are updated).

- I use then the tool of OpenFOAM to duplicate the points (mergeOrSplitBaffles -split -overwrite), it duplicates the points but then I cannot even run the solver.

Is there a good method to create sliding meshes for OpenFOAM with ANSA? I think I am doing something wrong.

Kind regards,

yosuu

pd; ansa support in my country cannot give me any tips since they don't have any experience in such meshes.
yosuu is offline   Reply With Quote

Old   July 14, 2014, 05:14
Default
  #2
Senior Member
 
Tom Fahner
Join Date: Mar 2009
Location: Delft, Netherlands
Posts: 226
Rep Power: 10
tomf is on a distinguished road
Send a message via MSN to tomf Send a message via Skype™ to tomf
Hi yosuu,

Our workflow is a bit different: Define the interface as a wall, so you get two different volumes in ANSA. Next do the meshing of both volumes, with the volumes having a different PID. Only show one of the volumes and all the boundaries (including the interface) of only that volume and use save visible as function. Press invert, show the interface again, rename the interface as interface_slave and use save visible as again. Now open the first "save visible as" saved file and use merge to include the second saved ansa file. You should now have the complete mesh with the interface split in 2 equal patches (interface and interface_slave), which can be wall in ANSA. Now export to OpenFOAM and again manually change the interface patches to cyclicAMI and off you go.

I hope this is clear enough?

Kind regards,
Tom
tomf is offline   Reply With Quote

Old   July 15, 2014, 09:29
Default
  #3
Senior Member
 
Vangelis Skaperdas
Join Date: Mar 2009
Location: Thessaloniki, Greece
Posts: 165
Rep Power: 9
vangelis is on a distinguished road
Hi there
I just want to add that you can set these two properties
as cyclicAMI type in the PID list in ANSA and output the mesh ready to run
without need for manual changes afterwards.

Then in auxiliaries>Interface
create a new interface of type AMI
and set it to noordeting type

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
Moving mesh Niklas Wikstrom (Wikstrom) OpenFOAM Running, Solving & CFD 122 June 15, 2014 06:20
ANSA mesh quality report bondmatt ANSA 2 February 18, 2013 07:35
[ICEM] Problem making structured mesh on a surface froztbear ANSYS Meshing & Geometry 4 November 10, 2011 09:52
Check the skewnesses of your face meshes and make sure the face mesh sizes are not to sophie-l Main CFD Forum 1 April 13, 2009 19:16
Check the skewnesses of your face meshes and make sure the face mesh sizes are not to sophie-l ANSYS Meshing & Geometry 0 April 13, 2009 17:27


All times are GMT -4. The time now is 00:50.