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 19, 2013, 07:23
Default
  #41
Senior Member
 
Artur's Avatar
 
Artur
Join Date: May 2013
Location: Southampton, UK
Posts: 226
Rep Power: 6
Artur is on a distinguished road
my run with rotatingMovingWall has now fully converged in terms of forces. I ran it with exact same settings as the previous one for advance coefficient of J = 0.64 (1.601ms-1 advance velocity at ~10 rps). I have experienced pretty much the same rate of convergence and the results accuracy was in of the same order in terms of forces and moments (+/- 2% c.f. the experimental results).

Attached pictures show, in order of appearance:
1. the old case with movingWall BC (already shown a few posts above but included here for consistency)
2. the new case with rotatingMovingWall BC showing Ux velocity using the same scale as the one used for pic 1 -> note the without comparison better representation of the no-slip condition
3. the new case with rotatingMovingWall BC -> note the 5-fold difference in magnitudes of the extreme velocity values and the no-slip condition spread across the blade
Attached Images
File Type: jpg PPTC_Ux_mowingWallBc.jpg (19.4 KB, 63 views)
File Type: jpg PPTC_Ux_rotatingMowingWallBc_largeVarRange.jpg (16.7 KB, 56 views)
File Type: jpg PPTC_Ux_rotatingMowingWallBc.jpg (18.8 KB, 56 views)
kiddmax and snowflying like this.
Artur is offline   Reply With Quote

Old   July 19, 2013, 07:29
Default
  #42
Member
 
Join Date: Apr 2013
Posts: 32
Rep Power: 4
simt is on a distinguished road
Thanks alot for sharing your conclusion, great!
simt is offline   Reply With Quote

Old   July 19, 2013, 07:33
Default
  #43
Senior Member
 
Artur's Avatar
 
Artur
Join Date: May 2013
Location: Southampton, UK
Posts: 226
Rep Power: 6
Artur is on a distinguished road
Just as an add-on, as I feel it is relevant: I am running at maxCo of 2.0 or 2.5, depending on how desperate I am on computational time, which usually yields time steps of 1.5e-4 - 2.0e-4 s for this case. That means the blade moves roughly 0.8 deg/time step.
Artur is offline   Reply With Quote

Old   July 19, 2013, 15:41
Default
  #44
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 tried to handle my case with the method suggested in tut.
I used my mesh and just applied the createAMIFaces.topoSetDict to create the AMI cellzones instead of using
splitMeshRegions -makeCellZones -overwrite

but I am wondering why innerCylinderSmallFace,and the other created Dic in set folder are empty.

Please, Look at the attachment that is made relevant my AMI cylinder.
Best
Reza
Attached Files
File Type: gz createAMIFaces.topoSetDict.tar.gz (680 Bytes, 23 views)
reza1980 is offline   Reply With Quote

Old   July 22, 2013, 03:43
Default
  #45
Senior Member
 
Artur's Avatar
 
Artur
Join Date: May 2013
Location: Southampton, UK
Posts: 226
Rep Power: 6
Artur is on a distinguished road
hmm... I don't see anything standing out that could be wrong with this dict. Have you cleared all the folders properly so that there are not sets present before running topoSet?
Artur is offline   Reply With Quote

Old   August 14, 2013, 10:15
Default
  #46
Member
 
Join Date: Aug 2013
Posts: 50
Rep Power: 3
nash is on a distinguished road
during the sHM there are faceZone as well as cellZone generated for innerCylinderSmall.

can i use this :

  • cellZone for the dynamicMeshDict?
  • faceZone createBafflesDict? which by doing this i can skip the createAMIFaces.topoSetDict.
incase of radial fan, the flow is upwards into fan and then the flow is radial.

i cant figure it out how to set the normalToSurface in createInletOutletSets.topoSetDict since the flow is differ from propeller.


Code:
 {
        name    outletFaces;
        type    faceSet;
        action  subset;
        source  normalToFace;
        sourceInfo
        {
            normal  (0 -1 0);   // Vector
            cos     0.3;        // Tolerance (max cos of angle)
        }
    }

    {
        name    inletFaces;
        type    faceSet;
        action  subset;
        source  normalToFace;
        sourceInfo
        {
            normal  (0 1 0);    // Vector
            cos     0.3;        // Tolerance (max cos of angle)
        }
    }
lets say if i already have the inlet and outlet generated from the sHM from STL , can i skip the part of creating the inlet and outlet patch?

Code:
Adding patches for surface regions
 ----------------------------------  
Patch    Type    Region 
-----    ----    ------ 
fan:  
5    wall    fan_rotor-layersides 
6    wall    fan_rotor-mrf-02 
7    wall    fan_casing-schwarz-03 
8    wall    fan_rotor-mrf-layer-02 
9    wall    fan_rotor-mrf-01 
10    wall    fan_casing 
11    wall    fan_plane 
12    wall    fan_inlet 
13    wall    fan_outlet 
14    wall    fan_channel 
15    wall    fan_casing-outter 
16    wall    fan_casing-mrf 
17    wall   fan_casing-02 
18    wall   fan_rotor--mrf-layer-01  

mrfDomain:  
19    wall    mrfDomain_frameboarder-interior 
20    wall    mrfDomain_frameboarder-interior_slave
but i'm not sure wether it is patch or just a region with the name fan_outlet and fan_inlet.

thank you in advance
nash is offline   Reply With Quote

Old   August 14, 2013, 11:41
Default
  #47
Senior Member
 
Artur's Avatar
 
Artur
Join Date: May 2013
Location: Southampton, UK
Posts: 226
Rep Power: 6
Artur is on a distinguished road
1. I think you can use the cellzones created by sHM, I recall that I did it some time ago and it worked but there was something about it that made me stick to the approach proposed by the tutorial (I'm really sorry but I can't recall what it was). So my answer would be: you can do it but be careful.

2. I'm not sure what you mean by:
Quote:
i cant figure it out how to set the normalToSurface in createInletOutletSets.topoSetDict since the flow is differ from propeller.
The normal vector is just a surface normal of the faces being selected. For instance, if the flow is parallel to x axis in the -ve direction and I want to select the inlet faces then I use:
Code:
normal  (1 0 0);
The cosine of angle is the tolerance of how closely the faces need to conform to the normal vector criterion in order to be selected. For a reasonably orthogonal mesh 0.3 or even less seems to work O.K. for me.

3. If you create your patches otherwise then I don't see why you shouldn't use them as they are. Be careful though, sometimes it is necessary to call
Code:
createPatch -overwrite
in order to remove empty patches from the boundary file (whether you do need it or not depends on how you go about things).

4. I'm not sure what you mean by the last question. The best way to check what patches you have is to a) check your boundary file b) misspell one patch name deliberately and try to run your case: all available patches should be printed on the screen together with the error message.
Artur is offline   Reply With Quote

Old   August 14, 2013, 12:00
Default
  #48
Member
 
Join Date: Aug 2013
Posts: 50
Rep Power: 3
nash is on a distinguished road
in the boundary i can see the listed patches by log.sHM, so they are patch and type wall. am i correct?

Last edited by nash; August 15, 2013 at 03:32.
nash is offline   Reply With Quote

Old   August 23, 2013, 19:01
Default
  #49
Member
 
Join Date: Aug 2013
Posts: 50
Rep Power: 3
nash is on a distinguished road
Hi everyone,

Just a quick view of what i have done so far..
after reading this thread and also the thread here
Problem using AMI

i tried to prepare case for simulation of centrifugal fan.

i'm using sHM from my simpleFoam MRF case. (2 stl file: for the geometry (fan and casing or rotor and stator; and AMI which is cylinder covering the rotor part)

to create AMI:
1) i removed the faceZone and cellZone created by sHM (patches like inlet outlet etc. generated within sHM)
2) followed the step using topoSet dict except for the createPatch for inlet outlet since i already have the patches. Instead of using cylinderToCell ( i dont know the p1 p2 and radii), i used surfaceToCell from the stl file.
3) createBaffles using the faceZone for AMI and cellZone for dynamicMesh.

after that used paraView to have a look at my AMI.

1) should the AMI looks the same as what in STL file?? because i got a cylinder but the bottom side is open ( i will include the image next week since now i dont have access to the file)

i hope someone can help me
thank you in advance
nash is offline   Reply With Quote

Old   August 24, 2013, 10:55
Default rotatingWallVelocity or movingWallVelocity
  #50
Senior Member
 
stephane sanchi
Join Date: Mar 2009
Posts: 300
Rep Power: 9
openfoam_user is on a distinguished road
Hi,

in the following tutorial

~/OpenFOAM/OpenFOAM-2.2.x/tutorials/multiphase/interDyMFoam/ras/mixerVesselAMI

the rotatingWallVelocity BC is used.

Stephane.
openfoam_user is offline   Reply With Quote

Old   October 1, 2013, 10:53
Default cavitation steps
  #51
New Member
 
samir
Join Date: Sep 2011
Location: Algeria
Posts: 11
Rep Power: 5
samir_cfd is on a distinguished road
Send a message via MSN to samir_cfd Send a message via Skype™ to samir_cfd
Hello !!

Please I am simulating cavitation of full 5 bladed marine propeller using Ansys Fluent, with sliding mesh

I am new in simulating multiphase flow, and i need if it is possible steps to simulate cavitation using Fluent

Best regards

Samir
samir_cfd is offline   Reply With Quote

Old   October 1, 2013, 11:47
Default
  #52
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,

You will note that this thread is a part of the OpenFOAM users' forum. I think you will get much more feedback if you post your question in the Fluent section.

Regards,

A
Artur is offline   Reply With Quote

Old   October 1, 2013, 12:06
Default
  #53
New Member
 
samir
Join Date: Sep 2011
Location: Algeria
Posts: 11
Rep Power: 5
samir_cfd is on a distinguished road
Send a message via MSN to samir_cfd Send a message via Skype™ to samir_cfd
Thanks Artur

I found just one commenter who work with fluent for marine propeller
samir_cfd 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 01:25.