CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Meshing & Mesh Conversion

Odd cyclic boundary... please help!

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

Like Tree1Likes
  • 1 Post By JackW

Reply
 
LinkBack Thread Tools Display Modes
Old   August 15, 2012, 09:32
Default Odd cyclic boundary... please help!
  #1
Member
 
Jack
Join Date: Aug 2012
Posts: 42
Rep Power: 5
JackW is on a distinguished road
Hi,

I am having some trouble with an imported gmsh file for a simpleFoam run on a T106A aerofoil.

I have included the velocity profile photo.

The idea is that the geometry represents a turbine cascade, so the top and bottom both have cyclic boundaries imposed. I started by copying the aerofoil2d example then using my geometry by performing gmshToFoam and altering the files in 0 and the constant/polymesh/boundary.

I use OF 2.1.1, and I changed the type of boundary to cyclic and used the matchNeighbour to associate the two together. I then in 0 set type to cyclic (without specifying any value) for U, p, nut, nuTilda.

After calling simpleFoam I got the error saying the boundaries don't match by nearly 2% (although I know that not to be the case), so I increased matchTolerance appropriately.

The sim runs and produces the attached profile. The flow angle is 45degs above horizontal. I expected the higher speed to continue onto the underside - however there is clearly not a match between the upper and lower surfaces.
________

It looks also as if little pockets of lower speed occur at the boundaries. and get pushed through the flow. I was wondering if most of my problems occur because when I create the mesh in gmsh, gmsh doesn't realise that I intend to use cyclic boundaries and so the points don't match up? Or if I haven't set the case up properly I have used a constant resolution throughout the space to try and minimise this.

Any help would be greatly appreciated, thank you very much!

Jack
Attached Images
File Type: png Screenshot from 2012-08-15 14:15:59.png (56.1 KB, 44 views)
JackW is offline   Reply With Quote

Old   August 15, 2012, 10:08
Default
  #2
Senior Member
 
chegdan's Avatar
 
Daniel P. Combest
Join Date: Mar 2009
Location: St. Louis, USA
Posts: 546
Rep Power: 18
chegdan will become famous soon enough
Jack,

I see that you are using simpleFoam with cyclics. Solvers that use cyclics (like channelFoam) prescribe a body force to maintain flow. With simpleFoam, it will "die out" since it is used to model pressure driven flow. You will need to add a body force. Fortunately there is some help on the forum (How to setup cyclic BCs in simpleFOAM on post 9) but it was found that you have to use Upwind and lower your relaxation factors in order to maintain stability. As an alternative, you can use the mapped boundary condition (example in tutorials/pisoFoam/les/pitzDailyMapped). The difference in the cyclic and mapped is that the cyclic is two way coupled and will require a body force, while the mapped patch is one-way coupled and can be used to set an average velocity/flowrate. Hope this helps.
__________________
Dan

Find me on twitter @dancombest and LinkedIn
chegdan is offline   Reply With Quote

Old   August 15, 2012, 21:03
Default
  #3
Member
 
Jack
Join Date: Aug 2012
Posts: 42
Rep Power: 5
JackW is on a distinguished road
Hi Dan,

Thanks - although this wasn't the problem. It was more a logistical problem with unordered faces (I am new to OF). The channel example uses a PG to drive the flow, in my above example the cyclic directions are not in the direction of the flow, so the flow is still driven by the the inflow. And the cyclics work fine now

Ps. Anyone coming to this thread for problems on cyclics, I found my solution by:
Creating a createPatchDict file in the system folder, via this syntax:

https://unihub.ru/tools/ofservice/br...atchDict?rev=2

run createPatch

Update files in 0/ to use the newly created patches.

Hope this helps anyone struggling to use imported and/or unstructured meshes with cyclic bcs.
wyldckat likes this.
JackW is offline   Reply With Quote

Old   August 16, 2012, 09:51
Default
  #4
Senior Member
 
chegdan's Avatar
 
Daniel P. Combest
Join Date: Mar 2009
Location: St. Louis, USA
Posts: 546
Rep Power: 18
chegdan will become famous soon enough
Excellent that you figured it out and it was simple...and better that you came back and answered your post!
__________________
Dan

Find me on twitter @dancombest and LinkedIn
chegdan is offline   Reply With Quote

Old   August 20, 2012, 02:31
Default
  #5
New Member
 
Thomas S
Join Date: Aug 2012
Posts: 11
Rep Power: 5
Thoma is on a distinguished road
Quote:
Originally Posted by JackW View Post

Ps. Anyone coming to this thread for problems on cyclics, I found my solution by:
Creating a createPatchDict file in the system folder, via this syntax:

https://unihub.ru/tools/ofservice/br...atchDict?rev=2

run createPatch

Update files in 0/ to use the newly created patches.

Hope this helps anyone struggling to use imported and/or unstructured meshes with cyclic bcs.

Can you please post here the syntax for your createPatchDict? I am not able to open the link.

Thank you!
Thoma is offline   Reply With Quote

Old   August 20, 2012, 20:12
Default
  #6
New Member
 
Thomas S
Join Date: Aug 2012
Posts: 11
Rep Power: 5
Thoma is on a distinguished road
Here it is:

| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 1.7.1 |
| \\ / A nd | Web: www.OpenFOAM.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object createPatchDict;
}


// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //


// Tolerance used in matching faces. Absolute tolerance is span of
// face times this factor. To load incorrectly matches meshes set this
// to a higher value.
matchTolerance 1E-3;


// Do a synchronisation of coupled points after creation of any patches.
// Note: this does not work with points that are on multiple coupled patches
// with transformations.
pointSync true;


// Patches to create.
patchInfo
(
{
name topAndBottom;
dictionary
{
type patch;
}
constructFrom patches;
patches ( auto0 auto2 );
}


{
name inlet;
dictionary
{
type patch;
}
constructFrom patches;
patches ( auto1 );
}


{
name outlet;
dictionary
{
type patch;
}
constructFrom patches;
patches ( auto3 );
}


{
name wing;
dictionary
{
type wall;
}
constructFrom patches;
patches ( auto4 );
}


{
name back;
dictionary
{
type empty;
}
constructFrom patches;
patches ( auto5 );
}


{
name front;
dictionary
{
type empty;
}
constructFrom patches;
patches ( auto6 );
}
);
Thoma is offline   Reply With Quote

Old   May 9, 2013, 22:49
Default
  #7
Member
 
sqing
Join Date: Sep 2012
Location: Dalian
Posts: 77
Rep Power: 4
Sunxing is on a distinguished road
Quote:
Originally Posted by JackW View Post
Hi,

I am having some trouble with an imported gmsh file for a simpleFoam run on a T106A aerofoil.

I have included the velocity profile photo.

The idea is that the geometry represents a turbine cascade, so the top and bottom both have cyclic boundaries imposed. I started by copying the aerofoil2d example then using my geometry by performing gmshToFoam and altering the files in 0 and the constant/polymesh/boundary.

I use OF 2.1.1, and I changed the type of boundary to cyclic and used the matchNeighbour to associate the two together. I then in 0 set type to cyclic (without specifying any value) for U, p, nut, nuTilda.

After calling simpleFoam I got the error saying the boundaries don't match by nearly 2% (although I know that not to be the case), so I increased matchTolerance appropriately.

The sim runs and produces the attached profile. The flow angle is 45degs above horizontal. I expected the higher speed to continue onto the underside - however there is clearly not a match between the upper and lower surfaces.
________

It looks also as if little pockets of lower speed occur at the boundaries. and get pushed through the flow. I was wondering if most of my problems occur because when I create the mesh in gmsh, gmsh doesn't realise that I intend to use cyclic boundaries and so the points don't match up? Or if I haven't set the case up properly I have used a constant resolution throughout the space to try and minimise this.

Any help would be greatly appreciated, thank you very much!

Jack
Hi Thomas,

May I know your inlet and outlet boundary conditions of your case? I'm also simulating a turbine cascade with the following BCs:
inlet: fixed total pressure and total temperature
outlet:fixed static pressure
I'm not sure that I have set the P file correctly. So I want to know your bcs and how you set them.

regards
Sunxing
Sunxing 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
Wind turbine simulation Saturn CFX 34 October 16, 2014 05:27
cyclic boundary conditions tuulio OpenFOAM Running, Solving & CFD 0 April 6, 2012 12:07
cyclic boundary conditions tuulio Main CFD Forum 0 March 31, 2012 06:47
Cyclic Boundary furkan CD-adapco 1 November 28, 2005 10:12
Trimmed cell and embedded refinement mesh conversion issues michele OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 2 July 15, 2005 04:15


All times are GMT -4. The time now is 16:16.