CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > SU2

Rotating blades linearly installed

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

Like Tree2Likes

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   September 11, 2015, 13:08
Default Rotating blades linearly installed
  #1
New Member
 
Join Date: Sep 2015
Posts: 17
Rep Power: 7
Luca S is on a distinguished road
Hi,

I'm studying an inviscid flow (air) on a blade, which is supposed to be one of a series of blades tested in line (instead of rotating). The mesh is unstructured and created with Pointwise (.su2 format).

I would like to know which kind of configuration file to use and how to set a translational periodic condition for my test.

The inlet and outlet conditions are:
- pressure inlet (153960 N/m^2, 348 K )
- pressure outlet (100000 N/m^2 )

See the attached mesh file, where you can find the boundary conditions inlet, outlet, blade, per1 e per2. The distance between the the upper wall (per2) and the lower wall (per1) is 0.71.

Thank you.
Attached Images
File Type: png mesh.png (40.4 KB, 46 views)
Luca S is offline   Reply With Quote

Old   September 12, 2015, 05:50
Default Convergence problem with 1000 iterations
  #2
New Member
 
Join Date: Sep 2015
Posts: 17
Rep Power: 7
Luca S is on a distinguished road
I tried to adapt the configuration file inv_channel.cfg (from the testcase named 'inviscid bump in a channel'):

% -------------------- BOUNDARY CONDITION DEFINITION --------------------------%
%
% Euler wall boundary marker(s) (NONE = no marker)
MARKER_EULER= ( blade, per1, per2 )
%
% Inlet boundary marker(s) (NONE = no marker)
% Format: ( inlet marker, total temperature, total pressure, flow_direction_x,
% flow_direction_y, flow_direction_z, ... ) where flow_direction is
% a unit vector.
% Default: Mach ~ 0.1
MARKER_INLET= ( inlet, 348, 153960.0, 0.8667, 0.5, 0.0 )
%
% Outlet boundary marker(s) (NONE = no marker)
% Format: ( outlet marker, back pressure (static), ... )
MARKER_OUTLET= ( outlet, 100000.0 )
%
MARKER_PERIODIC= ( per1, per2, 0, 0, 0, 0, 0, 0, 0, 0.71,0, per2, per1, 0, 0, 0, 0, 0, 0, 0, -0.71, 0 )


Then I use this mesh file and configuration file to run SU2_MSH as:
SU2_MSH inv_channel.cfg

The output is a new mesh (by default named mesh_out.su2).

Finally I change the input mesh file in the configuration file as:
MESH_FILENAME = mesh_out.su2

Setting 1000 iterations and running 'SU2_CFD inv_channel.cfg' the solver doesn't converge.

Any suggestions?

Thank you.
Luca S is offline   Reply With Quote

Old   September 15, 2015, 05:13
Default Results with Lax-Freidrich numerical method
  #3
New Member
 
Join Date: Sep 2015
Posts: 17
Rep Power: 7
Luca S is on a distinguished road
I solved the convergence problem setting the convective numerical method Lax-Friedrich:

% -------------------- FLOW NUMERICAL METHOD DEFINITION -----------------------%
%
% Convective numerical method (JST, LAX-FRIEDRICH, CUSP, ROE, AUSM, HLLC,
% TURKEL_PREC, MSW)
CONV_NUM_METHOD_FLOW= LAX-FRIEDRICH


However I can't see the periodicity after plotting Mach contours. See the attached config file that I used and the Mach number contours obtained.

Any ideas?

Thank you.
Attached Images
File Type: png machper.png (69.3 KB, 38 views)
Attached Files
File Type: txt inv_channel.txt (7.7 KB, 11 views)
Luca S is offline   Reply With Quote

Old   September 16, 2015, 10:00
Default
  #4
New Member
 
Salvatore Vitale
Join Date: Aug 2014
Posts: 6
Rep Power: 8
salvovitale is on a distinguished road
Dear Luca,

specify periodic like this:

MARKER_PERIODIC= ( per1, per2, 0, 0, 0, 0, 0, 0, 0, 0.71,0)

remove the periodic boundary from the MARKER_EULER because what you actually are imposing in you simulation is that your periodic boundaries are symmetry BC and not periodic.

MARKER_EULER= ( blade, per1, per2 ) should be MARKER_EULER= ( blade)


I think if you do this modification your test_case should run also with other schemes and converge to a periodic solution.


Regards


sv
Luca S likes this.
salvovitale is offline   Reply With Quote

Old   September 16, 2015, 10:24
Default
  #5
New Member
 
Join Date: Sep 2015
Posts: 17
Rep Power: 7
Luca S is on a distinguished road
Hi Salvo,

first I changed the periodic marker, providing the first half of my specification, i.e.,

MARKER_EULER= ( blade, per1, per2 )
MARKER_PERIODIC= ( per1, per2, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, -0.71, 0.0 )

the solver runs but I still can't get a periodic solution.

Then I tried removing per1 and per2 from the euler marker,

MARKER_EULER= ( blade )
MARKER_PERIODIC= ( per1, per2, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, -0.71, 0.0 )

but the solver diverged,

Iter Time(s) Res[Rho] Res[RhoE] CLift(Total) CDrag(Total)
178 0.058369 33.818948 53.467412 -10000.000000 -10000.000000
179 0.058366 33.941822 53.670406 10000.000000 -10000.000000
180 0.058334 34.259249 53.921974 10000.000000 -10000.000000
181 0.058336 34.467027 54.351889 10000.000000 10000.000000
182 0.058333 34.671664 54.904520 10000.000000 10000.000000
183 0.058332 35.136916 55.283411 10000.000000 10000.000000
184 0.058324 35.175393 55.373995 10000.000000 10000.000000
185 0.058325 35.527664 55.746049 -10000.000000 -10000.000000
186 0.058322 35.907650 56.116415 -10000.000000 -10000.000000
187 0.058316 36.114722 57.074697 10000.000000 -10000.000000
188 0.058312 36.495260 57.216966 -10000.000000 -10000.000000

!!! Error: SU2 has diverged. Now exiting... !!!


Thank you very much for your answer.
Luca S is offline   Reply With Quote

Old   September 16, 2015, 10:55
Default
  #6
New Member
 
Salvatore Vitale
Join Date: Aug 2014
Posts: 6
Rep Power: 8
salvovitale is on a distinguished road
Could you post you cfg file and the original mesh before you run SU_MSH so i can have a look and see what is the problem.

sv
salvovitale is offline   Reply With Quote

Old   September 16, 2015, 11:27
Default
  #7
New Member
 
Join Date: Sep 2015
Posts: 17
Rep Power: 7
Luca S is on a distinguished road
Dear Salvo,

here you are the config file that I use before running SU2_MSH and the original mesh.

Thank you
Attached Images
File Type: png mesh.png (40.4 KB, 10 views)
Attached Files
File Type: txt inv_channel.txt (7.7 KB, 8 views)
Luca S is offline   Reply With Quote

Old   September 16, 2015, 11:44
Default
  #8
New Member
 
Giulio
Join Date: Apr 2014
Location: Milano
Posts: 17
Rep Power: 8
LaSerpe is on a distinguished road
Luca I think Salvo means that he needs the SU2 mesh file not the image.

cheers

g
Luca S likes this.
__________________
Giulio Gori
Phd candidate, Politecnico di Milano
LaSerpe is offline   Reply With Quote

Old   September 16, 2015, 12:02
Default
  #9
New Member
 
Join Date: Sep 2015
Posts: 17
Rep Power: 7
Luca S is on a distinguished road
Sorry, I hope this is the mesh file you wanted.

Thank you.
Attached Files
File Type: zip meshok.su2.zip (106.1 KB, 8 views)
Luca S is offline   Reply With Quote

Old   September 16, 2015, 13:50
Default turb_vki.cfg from VKI turbine testcase
  #10
New Member
 
Join Date: Sep 2015
Posts: 17
Rep Power: 7
Luca S is on a distinguished road
I'm trying to adapt the attached config file.

I run SU2_MSH and get the periodic mesh, then when I run SU2_CFD I get this error:

------------------------- Geometry Preprocessing ------------------------
Setting point connectivity.
Renumbering points (Reverse Cuthill McKee Ordering).
Recomputing point connectivity.
Setting element connectivity.
Checking the numerical grid orientation.
Identifying edges and vertices.
Computing centers of gravity.
Errore di segmentazione

Any ideas?
Attached Files
File Type: txt turb_vki.txt (8.8 KB, 4 views)
Luca S is offline   Reply With Quote

Old   September 17, 2015, 05:56
Default
  #11
New Member
 
Join Date: Sep 2015
Posts: 17
Rep Power: 7
Luca S is on a distinguished road
I modified again the config file 'turb_vki.cfg', I set:

% ------------- DIRECT, ADJOINT, AND LINEARIZED PROBLEM DEFINITION ------------%
%
% Physical governing equations (EULER, NAVIER_STOKES,
% TNE2_EULER, TNE2_NAVIER_STOKES,
% WAVE_EQUATION, HEAT_EQUATION, LINEAR_ELASTICITY,
% POISSON_EQUATION)
PHYSICAL_PROBLEM= EULER
%
% Specify turbulent model (NONE, SA, SA_NEG, SST)
KIND_TURB_MODEL= NONE

% -------------------- BOUNDARY CONDITION DEFINITION --------------------------%
%
% Navier-Stokes wall boundary marker(s) (NONE = no marker)
MARKER_EULER= ( blade, per1, per2 )
%
% Inlet boundary type (TOTAL_CONDITIONS, MASS_FLOW)
INLET_TYPE= TOTAL_CONDITIONS
%
% Inlet boundary marker(s) with the following formats (NONE = no marker)
% Total Conditions: (inlet marker, total temp, total pressure, flow_direction_x,
% flow_direction_y, flow_direction_z, ... ) where flow_direction is
% a unit vector.
% Mass Flow: (inlet marker, density, velocity magnitude, flow_direction_x,
% flow_direction_y, flow_direction_z, ... ) where flow_direction is
% a unit vector.
MARKER_INLET= ( inlet, 348.0, 153960.0, 0.8667, 0.5, 0.0 )
%
% Outlet boundary marker(s) (NONE = no marker)
% Format: ( outlet marker, back pressure (static), ... )
MARKER_OUTLET= ( outlet, 100000.0 )
%
% Periodic boundary marker(s) (NONE = no marker)
% Format: ( periodic marker, donor marker, rotation_center_x, rotation_center_y,
% rotation_center_z, rotation_angle_x-axis, rotation_angle_y-axis,
% rotation_angle_z-axis, translation_x, translation_y, translation_z, ... )
MARKER_PERIODIC= ( per1, per2, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, -0.71, 0.0 )
%
% Marker(s) of the surface to be plotted or designed
MARKER_PLOTTING= ( blade )
%
% Marker(s) of the surface where the functional (Cd, Cl, etc.) will be evaluated
MARKER_MONITORING= ( blade )

I attach the config file and the results obtained running SU2_CFD (without creating the periodic mesh).

Thank you.
Attached Images
File Type: png mach.png (55.3 KB, 12 views)
File Type: png pressurecoeff.png (54.1 KB, 8 views)
Attached Files
File Type: txt turb_vki_modif.txt (8.8 KB, 1 views)
Luca S is offline   Reply With Quote

Old   September 17, 2015, 06:28
Default
  #12
New Member
 
Salvatore Vitale
Join Date: Aug 2014
Posts: 6
Rep Power: 8
salvovitale is on a distinguished road
I tryed to run your cases and I also got some troubles. I think the problem is the quality of your mesh. Look at the images attached and try to imporve the mesh.

cheers
sv

PS good that you start as a template from the turb_vki.cgf
Attached Images
File Type: jpg mesh_comments.jpg (89.2 KB, 26 views)
File Type: jpg periodic_mesh_outeltcorner.jpg (53.8 KB, 27 views)
salvovitale is offline   Reply With Quote

Old   September 17, 2015, 06:53
Default
  #13
New Member
 
Join Date: Sep 2015
Posts: 17
Rep Power: 7
Luca S is on a distinguished road
Dear Salvo.

I try to correct my mesh. In the meantime I attach the last config file that I'm using (without running SU2_MSH). I think it works well.

Thank you very much.
Attached Files
File Type: txt turb_vki_def.txt (8.2 KB, 3 views)
Luca S is offline   Reply With Quote

Old   September 17, 2015, 07:26
Default
  #14
New Member
 
Join Date: Sep 2015
Posts: 17
Rep Power: 7
Luca S is on a distinguished road
Salvo, I created a new mesh with the corrections you suggested. However I can run SU2_MSH only removing per1 and per2 from MARKER_EULER, and then when I run SU2_CFD I get again this error:

------------------------- Geometry Preprocessing ------------------------
Setting point connectivity.
Renumbering points (Reverse Cuthill McKee Ordering).
Recomputing point connectivity.
Setting element connectivity.
Checking the numerical grid orientation.
Identifying edges and vertices.
Computing centers of gravity.
Errore di segmentazione

I attach the new mesh file.

Thank you
Attached Files
File Type: zip mesh_buona.su2.zip (115.7 KB, 3 views)
Luca S is offline   Reply With Quote

Old   September 17, 2015, 07:52
Default
  #15
New Member
 
Join Date: Sep 2015
Posts: 17
Rep Power: 7
Luca S is on a distinguished road
To get results with the new mesh I created running SU2_CFD (without creating the periodical mesh), I have to change the Convective numerical method from ROE to LAX-FRIEDRICH

CONV_NUM_METHOD_FLOW= LAX-FRIEDRICH

I attach the new results.

Thank you.
Attached Images
File Type: png mach.png (62.8 KB, 11 views)
File Type: png pressurecoeff.png (58.3 KB, 6 views)
Luca S is offline   Reply With Quote

Old   September 17, 2015, 10:01
Default
  #16
New Member
 
Salvatore Vitale
Join Date: Aug 2014
Posts: 6
Rep Power: 8
salvovitale is on a distinguished road
You cant get a periodic solution without running SU2_MSH, because you must first create a periodic mesh with halo nodes on one side. With this new mesh I get to drop down 2 order the residuals. However, I think with that trailing-edge it s pretty difficult to get a good convergence with an Euler solver. Anyway your case now works and you can start build up on that. You may still improve your mesh though.

Attached my working cfg file. Change the name of the mesh on the config file, run SU2_MSH, then change again the name of the mesh file and run SU2_CFD.

cheers

sv
Attached Images
File Type: jpg periodic_sol.jpg (48.8 KB, 22 views)
Attached Files
File Type: txt inv_channel.txt (7.7 KB, 16 views)
salvovitale is offline   Reply With Quote

Old   September 17, 2015, 10:48
Default
  #17
New Member
 
Join Date: Sep 2015
Posts: 17
Rep Power: 7
Luca S is on a distinguished road
Thank you very much Salvo, I try to work on this to get better residuals.
Luca S is offline   Reply With Quote

Old   September 17, 2015, 12:33
Default
  #18
New Member
 
Join Date: Sep 2015
Posts: 17
Rep Power: 7
Luca S is on a distinguished road
I tried to run the viscous case (running SU2_MSH and SU2_CFD) and this time the vki turbine config file worked very well.
I attach the results and the config file.

Of course I modified also the mesh (see attached image) creating a structured zone around the blade.
Attached Images
File Type: png machdim.png (84.7 KB, 20 views)
File Type: png pressurecoeffdim.png (77.5 KB, 13 views)
File Type: png meshNS.png (49.1 KB, 15 views)
File Type: png meshNSzoom.png (50.0 KB, 19 views)
Attached Files
File Type: txt vki.txt (8.7 KB, 10 views)
Luca S is offline   Reply With Quote

Old   September 18, 2015, 05:58
Default Pressure coefficient wrong values?
  #19
New Member
 
Join Date: Sep 2015
Posts: 17
Rep Power: 7
Luca S is on a distinguished road
Does anyone know if the pressure coefficients values I get in both inviscid and viscous cases are ok?

Maybe it is a pressure coefficient definition problem?

Thank you
Attached Images
File Type: png pressurecoeffdim.png (77.5 KB, 16 views)
File Type: png Cp.png (77.9 KB, 12 views)
Luca S is offline   Reply With Quote

Old   September 18, 2015, 08:11
Default Scale Problem
  #20
New Member
 
Join Date: Sep 2015
Posts: 17
Rep Power: 7
Luca S is on a distinguished road
How can I scale the mesh with a scale factor of 0.048?

Thank you
Luca S is offline   Reply With Quote

Reply

Tags
boundary condition, periodic condition, pressure drop

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Rotating blades of a fan by Fluent? guillaume1990 FLUENT 17 June 22, 2016 04:01
Rotating blades of a fan Fluent? guillaume1990 ANSYS 1 March 21, 2014 04:15
Moving Meshes or Rotating Refrence frame is suitable for Rotating Blades? arash_7444 FLUENT 3 March 21, 2011 02:07
Rotating blades fan problem Luk FLUENT 1 June 27, 2006 10:56
Rotating blades blower Luk FLUENT 0 June 27, 2006 10:54


All times are GMT -4. The time now is 17:21.