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

Propeller case in AMI tutorial

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

Like Tree6Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   July 10, 2013, 16:12
Default Propeller case in AMI tutorial
  #1
Member
 
reza1980's Avatar
 
reza
Join Date: Jan 2013
Location: Goteborg-Sweden
Posts: 79
Rep Power: 4
reza1980 is on a distinguished road
Hi Foamers,
I run the propeller case in AMI tutorial oF2.1x. One odd thing is the back flow on tip of blade and the non zero velocity in y-dir (flow dir) that not satisfy the no slip condition.(Please look the attachments)
I would like to know your comments.
reza1980 is offline   Reply With Quote

Old   July 10, 2013, 16:14
Default
  #2
Member
 
reza1980's Avatar
 
reza
Join Date: Jan 2013
Location: Goteborg-Sweden
Posts: 79
Rep Power: 4
reza1980 is on a distinguished road
The images are as below:
Attached Images
File Type: jpg 1.jpg (46.4 KB, 100 views)
File Type: jpg 2.jpg (43.7 KB, 87 views)
File Type: jpg 3.jpg (40.7 KB, 82 views)
File Type: jpg 4.jpg (41.2 KB, 82 views)
File Type: jpg 5.jpg (39.4 KB, 69 views)
reza1980 is offline   Reply With Quote

Old   July 12, 2013, 04:02
Default
  #3
Senior Member
 
Artur's Avatar
 
Artur
Join Date: May 2013
Location: Southampton, UK
Posts: 226
Rep Power: 6
Artur is on a distinguished road
Hi reza,

I've only started using pimpleDyMFoam to analyse marine propellers recently so I'm definitely not an expert. I've used the modified version of the propeller tutorial to replicate the Potsdam Propeller Test Case (PPTC) results. I didn't notice the thing you pointed out until I saw your post. I looked at my results and found them to have the same features despite a much finer mesh. See the attached pictures 1 and 2 (for advance coefficient J=0.64).

It seems that these values are very small compared to the velocity at the wall originating from the rotational motion of the prop (picture 3) and don't seem to affect the pressure distribution (pictures 4 and 5) nor the forces (for this case I was within 2.5% of Kt, Kq and efficiency w.r.t. the experimental results).

None the less I would love to hear someone more knowledgeable comment on the topic to better understand it.
Attached Images
File Type: jpg PPTC_Ux_J_0.64_suctionSide.jpg (24.4 KB, 70 views)
File Type: jpg PPTC_Ux_J_0.64_pressureSide.jpg (24.1 KB, 57 views)
File Type: jpg PPTC_Umag_J_0.64_suctionSide.jpg (23.7 KB, 57 views)
File Type: jpg PPTC_p_J_0.64_suctionSide.jpg (23.3 KB, 50 views)
File Type: jpg PPTC_p_J_0.64_pressureSide.jpg (23.8 KB, 42 views)
Artur is offline   Reply With Quote

Old   July 12, 2013, 05:26
Default
  #4
Member
 
reza1980's Avatar
 
reza
Join Date: Jan 2013
Location: Goteborg-Sweden
Posts: 79
Rep Power: 4
reza1980 is on a distinguished road
Hi Artur,
I would thank you for your reply.One odd thing in the tutorial is not satisfying no-slip condition on the propeller that I can see same on my case as well.
What motivated me to check out the results of the tutorial is my project. It is related to a tanker propeller model meshed by pointwise that should be compared with the experimental values for open-water and self-propelled case.
The techniques are AMI and MRF ,To approach AMI I did as below:
  • create two parts as rotor(inner cylinder that is rotating)and stator (not rotating outer part) .
  • merge two parts through implement mergeMeshes stator rotor.
  • rename the type of boundary AMI from patch to cyclic AMI and add the neighborhood and tolerance and update 0 folder .
  • use topoSet or splitMeshRegions -makeCellZones -overwrite to create the cellZones and update the dynamicmeshDic.
  • Run pimpleDyMFoam as parallel on network(claster).
For MRF is almost same except the applying stitches ,stitchMesh,instead of split and Remove manually the empty boundaries (0 faces) from constant/boundaries file.
My case includes 3.5 mil cells and the results approaches converged for AMI and MRF. But what I suffers me is to have backflow for two cases on the tip of blades and a noticeable gap between the thrust force
obtained from experimental and numerical values ,around 40%,in AMI.
Furthermore,MRF shows close results to the experiment ,just 12.3% difference,would be agreeable.
reza1980 is offline   Reply With Quote

Old   July 12, 2013, 05:34
Default
  #5
Senior Member
 
Artur's Avatar
 
Artur
Join Date: May 2013
Location: Southampton, UK
Posts: 226
Rep Power: 6
Artur is on a distinguished road
I do it slightly differently. I mesh an .stl of two cylinders inside and snap the mesh of the inner one to the prop. Then I recreate the patches using topoSet much as it was done in the tutorial. But I don't see how that would affect the velocities.

Can you expand a bit about the backflow you observed? Do you think it should not be there and you think the small Ux components are responsible for it?
Artur is offline   Reply With Quote

Old   July 12, 2013, 06:02
Default
  #6
Member
 
reza1980's Avatar
 
reza
Join Date: Jan 2013
Location: Goteborg-Sweden
Posts: 79
Rep Power: 4
reza1980 is on a distinguished road
It is the recommendation of my supervisor,The attachments is the images from AMI and MRF,-X is the inflow direction .But i more concerned about the big gap between the AMI and experimental values that is constant and fully converged.
In addition ,you can consider the images from the tutorial case to see no slip condition doesn't satisfy in AMI .
Attached Images
File Type: jpg 1.jpg (35.7 KB, 78 views)
File Type: jpg 2.jpg (35.2 KB, 74 views)
File Type: jpg mrf.jpg (34.9 KB, 67 views)
File Type: jpg mrf1.jpg (43.9 KB, 76 views)
reza1980 is offline   Reply With Quote

Old   July 12, 2013, 06:16
Default
  #7
Senior Member
 
Artur's Avatar
 
Artur
Join Date: May 2013
Location: Southampton, UK
Posts: 226
Rep Power: 6
Artur is on a distinguished road
Aren't the +ve Ux values (in your recent pictures, not the tutorial ones) close to the tips of the blades associated with the tip vortex? In which case I feel they should be there.

What sort of magnitudes are the Ux velocities on the blades of the non-tutorial prop you are evaluating? Are they also in the range of 1e-2 - 1e-3 like in the tutorial or much bigger (for my case I found them to be in this range)?

I'm not convinced that the small Ux values on the wall are the root cause of your Kt and Kq being different from the experiment (I have them too and still I get reasonable agreement) although I agree that they shouldn't be there.

Have you tried using different settings, turbulence models, etc.? I run k-omega SST, y+ around 30-40, base cell size 0.125 m refined to level 6 for a prop with 0.25 m diameter. I had to under-relax the k,omega and U field by 0.7 in order to get a stable and reliable solution. I also tend to ramp up the maxCo to 2.5-3.5 as the simulation progresses to make it faster. Apart from that my schemes and settings are not largely different from the tutorial and I observe convergence of forces and moments after about a half to one full revolution.
Artur is offline   Reply With Quote

Old   July 12, 2013, 07:43
Default
  #8
Member
 
reza1980's Avatar
 
reza
Join Date: Jan 2013
Location: Goteborg-Sweden
Posts: 79
Rep Power: 4
reza1980 is on a distinguished road
The images 2&3 concerned about the small positive velocity in +x-dir on the tips .It should filter the minimum velocity to be seen.
I followed the tutorial k-eps turbulent model that satisfies the experimental value for MRF. I think the tip vortex generates after tip and front of the blade not on the tip.
Not satisfying no-slip condition may make not converging to the experimental case. I want to report this as bug.
reza1980 is offline   Reply With Quote

Old   July 12, 2013, 07:50
Default
  #9
Senior Member
 
Artur's Avatar
 
Artur
Join Date: May 2013
Location: Southampton, UK
Posts: 226
Rep Power: 6
Artur is on a distinguished road
Have you tried pushing your tolerances down in the fvSolution? What y+ is your mesh at?
Artur is offline   Reply With Quote

Old   July 12, 2013, 07:55
Default
  #10
Member
 
reza1980's Avatar
 
reza
Join Date: Jan 2013
Location: Goteborg-Sweden
Posts: 79
Rep Power: 4
reza1980 is on a distinguished road
I didn't make the mesh.This is my fvSoloutionDic:
//
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.1.x |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

solvers
{
pcorr
{
solver GAMG;
tolerance 1e-7; // 1e-5;
relTol 0.001; //0;
smoother DICGaussSeidel;
cacheAgglomeration no;
nCellsInCoarsestLevel 10;
agglomerator faceAreaPair;
mergeLevels 1;
maxIter 50;
}

p
{
$pcorr;
tolerance 1e-8;
relTol 0.001; //0.01;
}

pFinal
{
$p;
tolerance 1e-8;
relTol 0;
}

"(U|k|epsion)"
{
solver smoothSolver;
smoother GaussSeidel;
tolerance 1e-8;
relTol 0.01;
}

"(U|k|epsilon)Final"
{
solver PBiCG;
preconditioner DILU;
tolerance 1e-8;
relTol 0;
}
}

PIMPLE
{
correctPhi yes;
nOuterCorrectors 3;
nCorrectors 2; //1;
nNonOrthogonalCorrectors 2;
}

relaxationFactors
{
p 0.2;
"(U|k|epsilon).*" 0.5;

}

cache
{
grad(U);
}

// ************************************************** *********************** //
reza1980 is offline   Reply With Quote

Old   July 12, 2013, 08:18
Default
  #11
Senior Member
 
Artur's Avatar
 
Artur
Join Date: May 2013
Location: Southampton, UK
Posts: 226
Rep Power: 6
Artur is on a distinguished road
It's very similar to mine in terms of the tolerances and settings except for the 0.2 relaxation factor on p. Are you sure that it is not too low? I've found that setting it to anything below 0.5 may affect your results slightly. Maybe try with these just to make sure:

Code:
 p              1.0
 "(U|k|omega).*"   0.7;
To check your y+ use the yPlusRAS utility from OpenFOAM.

Other than that I suppose it's either the mesh or something I am not aware of..
Artur is offline   Reply With Quote

Old   July 12, 2013, 08:25
Default
  #12
Member
 
reza1980's Avatar
 
reza
Join Date: Jan 2013
Location: Goteborg-Sweden
Posts: 79
Rep Power: 4
reza1980 is on a distinguished road
These values are the recommended by my supervisor for K-ep model.I think mesh is quite OK if we conciser the MRF is quite reasonable.
reza1980 is offline   Reply With Quote

Old   July 15, 2013, 06:42
Default
  #13
Senior Member
 
Artur's Avatar
 
Artur
Join Date: May 2013
Location: Southampton, UK
Posts: 226
Rep Power: 6
Artur is on a distinguished road
Hi,
Any progress on your side with figuring out why the no-slip condition in the flow direction is not satisfied? I have been thinking about it and I have noticed that this occurs mainly in the regions where the prop blade is becoming very thin in the direction parallel to the onset flow, probably due to an incorrect interpolation scheme selected. I'll try running a few cases with some other schemes than linear and will get back to you with my findings. Before I do that I want to run a case with a cylinder instead of the prop to see if the Ux velocity will be zero on the wall perpendicular to the flow given the much higher thickness of the body c.f. that of the prop.
Artur is offline   Reply With Quote

Old   July 15, 2013, 09:23
Default
  #14
Senior Member
 
Artur's Avatar
 
Artur
Join Date: May 2013
Location: Southampton, UK
Posts: 226
Rep Power: 6
Artur is on a distinguished road
Here is the picture of a rotating cylinder with flow parallel to the x axis. Free stream fluid velocity is (-1.602 0 0). You can still see regions of non-zero axial velocity on the wall of the cylinder despite:
- increased no. PIMPLE runs / timestep
- reduced tolerances on all variables to 1e-12
- adoption of smooth solver for U instead of PBiCG used in the propeller tutorial
- usage of linearUpwind and cubicCorrection schemes for U field interpolation
- reduced AMI tolerance in createBafflesDict from 1e-4 to 1e-6 (wirte precision)
- increase of the under-relaxation factors on all variables back to 1.0 (used to be 0.7 on the U, k and omega fields)

In the final attempt I tried increasing the domain size even more (it was over 6D of the cylinder in diameter and of about the same length upstream and downstream of the body). Then I also increased the AMI cylinder radius and length to move the interphase from the cylinder. Didn't help either.

There were so few differences between each combination that I am pretty convinced that the problem is someplace else.
Attached Images
File Type: jpg rotatingCylinder_Ux.jpg (17.0 KB, 52 views)
Artur is offline   Reply With Quote

Old   July 15, 2013, 09:41
Default
  #15
Member
 
reza1980's Avatar
 
reza
Join Date: Jan 2013
Location: Goteborg-Sweden
Posts: 79
Rep Power: 4
reza1980 is on a distinguished road
Artur
I want to run my case by MRFSimpleFoam .
Please look at this
stitchMesh problem
I look forward to know your idea.
reza1980 is offline   Reply With Quote

Old   July 15, 2013, 09:56
Default
  #16
Senior Member
 
Artur's Avatar
 
Artur
Join Date: May 2013
Location: Southampton, UK
Posts: 226
Rep Power: 6
Artur is on a distinguished road
I haven't got any experience in MRFSimpleFoam. It is not useful for what I am evaluating as I focus on unsteady flow, sorry.
Artur is offline   Reply With Quote

Old   July 16, 2013, 04:50
Default
  #17
Member
 
reza1980's Avatar
 
reza
Join Date: Jan 2013
Location: Goteborg-Sweden
Posts: 79
Rep Power: 4
reza1980 is on a distinguished road
Artur,
I did my best to make close the my result to experimental value but there is still a big gap.The positive velocity and non-overlapped cells are still alive.
In this regard I need to review what I did:
* Export two parts like Stator and Rotor from pointwise to OpenFoam
* Merge to parts as mergeMeshes Stator Rotor
* Update Boundary (Add cyclicAMi and tolerance)
* Use splitMeshRegions -makeCellZones -overwrite to make cellZones

could you please let me know your implement to make AMI
Regards
Reza
reza1980 is offline   Reply With Quote

Old   July 16, 2013, 04:57
Default
  #18
Senior Member
 
Artur's Avatar
 
Artur
Join Date: May 2013
Location: Southampton, UK
Posts: 226
Rep Power: 6
Artur is on a distinguished road
I follow the same approach as the tutorial except I use .stl files instead of .obj files. So:
1. snap mesh to a big cylinder, a small cylinder (AMI) and prop
2. select outer faces using topoSet and create outer patches
3. create the cellZones for AMI using the small cylinder
4. call createBaffles and mergeOrSplitBaffles to create the AMI interface

I don't think, however, that the way you do it is in any way inferior and so should lead to similar if not the same results..
Artur is offline   Reply With Quote

Old   July 16, 2013, 05:00
Default
  #19
Member
 
reza1980's Avatar
 
reza
Join Date: Jan 2013
Location: Goteborg-Sweden
Posts: 79
Rep Power: 4
reza1980 is on a distinguished road
But I am more intersted to use my mesh since the other parts of projects is related to this mesh and i need to compare them.
reza1980 is offline   Reply With Quote

Old   July 16, 2013, 05:05
Default
  #20
Senior Member
 
Artur's Avatar
 
Artur
Join Date: May 2013
Location: Southampton, UK
Posts: 226
Rep Power: 6
Artur is on a distinguished road
In that case your initial approach is the only way I can think of. Sadly, I haven't got much experience in using externally generated meshes though so perhaps someone else could help you with that issue...
Artur 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
MRF and employing on a propeller case reza1980 OpenFOAM 9 June 12, 2013 09:27
A questionable Tutorial test case immortality OpenFOAM Running, Solving & CFD 0 December 5, 2012 09:40
propeller tutorial openfoam_user OpenFOAM Running, Solving & CFD 0 February 8, 2012 05:02
tutorial copying troubles / new case Gabbee90 OpenFOAM Running, Solving & CFD 0 June 3, 2011 21:50
FoamX refuses to open an interFoam tutorial case vrecha OpenFOAM Pre-Processing 5 March 12, 2008 13:36


All times are GMT -4. The time now is 05:44.