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

Underwater Propeller CFD analysis with Ansys CFX

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   March 13, 2014, 05:42
Post Underwater Propeller CFD analysis with Ansys CFX
  #1
New Member
 
Trabelsi Alaeddine
Join Date: Feb 2014
Posts: 3
Rep Power: 7
Alaeddine is on a distinguished road
Hello,

I'm new to CFD analysis. My first application consist of an underwater 3 bladed propeller analysis in order to determine its thrust and get its characteristics (Kt=f(J), 10Kq=f(J) and η=f(J) where: J=advance ratio; Kt=thrust coefficient; Kq=torque coefficient).

I will show you how I proceeded and give you some screenshots illustrating my work and I hope you can guide me in order to improve my result (which looks not really reasonable).Because attatchments are limited in size you can download them from this link: http://www.2shared.com/file/nxFfFIlN/Screenshots.html (file size=3.25 Mo)

Step 1: I created the propeller geometry then I defined the rotational domain and the stationary domain with Solidworks.

Step 2: I exported the geometry to Pointwise in order to mesh the domains.

Step 3: I exported the mesh to Ansys CFX-Pre

STEP 4: I defined the analysis mode type as transient (see attatchment)

Step 5: I set up the boundary conditions as follows:

-The stationary domain entrance is defined as Inlet (velocity component U=V=W=0 m.s^-1) and turbulent intensity 5%.

-The top, bottom and side walls are defined as Opening Pres. and Dirn. with pressure = 0.

-The exit also is defined as Opening Pres. and Dirn. with pressure = 0.

-The propeller surfaces were defined as a rotating non slip wall.

-I defined the rotational domain motion with 2500 RPM.

-I defined fluid-fluid interfaces between the stationary default domain and the small rotating propeller domain.

-The frame change option is set on both fluid-fluid interfaces to frozen rotor.

STEP 6: I set up the global initialisation as shown in the attatchment

STEP 7: I run the solver then I launched CFX-Post to visualise results (see attatchments)

Now my questions are as follows:

*Any comments on the meshing quality ?
*Are the Pre-settings correct ?
*Why the streamline don't seem to be reasonable ? What should I change ?
*How can I get the plots I mentioned above from CFX-Post ? (please have a look at the last page of the attatched PDF where you can find an example of what I intend to get )
*Does the values shown in the image called "CFX-Post Thrust" really present the thrust and torque produced by the propeller ?

Any help would be great! Thanks

Waiting for your replies

Trabelsi Alaeddine
Alaeddine is offline   Reply With Quote

Old   March 13, 2014, 08:07
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 15,849
Rep Power: 122
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Lots of things to fix in your analysis. You have a bit of work to do before you get an accurate result.

* Why is the inlet U=V=W=0? Surely you want to model the prop in a flow, so U should be the speed you wish to model.
* Your simulation has not converged very well. See FAQ: http://www.cfd-online.com/Wiki/Ansys...gence_criteria
* Why have you modelled this as transient? If you are using a frozen rotor approach use a steady state simulation.
* Why have you modelled 3 blades? Why not model 1 blade with periodic boundaries?
* If you must use a transient simulation, then use adaptive time steps, homing in on 3-5 coeff loops per iteration. Make sure the max and min values are wide enough to not restrict the time step size, let it find the time step size it needs.
* You need to do sensitivity studies on convergence and mesh size (especially mesh size). See FAQ for details: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F and http://journaltool.asme.org/Template...umAccuracy.pdf
ghorrocks is offline   Reply With Quote

Old   March 13, 2014, 12:29
Default
  #3
New Member
 
Trabelsi Alaeddine
Join Date: Feb 2014
Posts: 3
Rep Power: 7
Alaeddine is on a distinguished road
Thanks a lot ghorrocks for your pieces of advice. I'm working to improve my results following your recommendations. However, I found a tutorial in which the transient type, the frozen rotor option and the U=V=W=0 condition are used but the result seems to be logic. You can download the tutorial from this link:

http://www.mediafire.com/download/kk...rial_elica.zip (file size:22.95 Mo)

I'm wondering why the simulation in the tutorial gives a good result.

Anyway, I will be back with the new results as soon as possible.

A last question: how can I model 1 blade with periodic boundaries ? have you any documents or links that could help me to try it ?

Thanks a lot another time.
Alaeddine is offline   Reply With Quote

Old   March 13, 2014, 17:34
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 15,849
Rep Power: 122
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Your link is to an executable. I do not run executables from download sites.

Have a look at the tutorials on modelling single blade passages. There are a few examples of this in rotating machinery.
ghorrocks is offline   Reply With Quote

Old   March 14, 2014, 10:49
Default
  #5
New Member
 
Trabelsi Alaeddine
Join Date: Feb 2014
Posts: 3
Rep Power: 7
Alaeddine is on a distinguished road
You can download the tutorial as *.SWF file from this link:

http://www.mediafire.com/download/7o...r6j0o/Tuto.swf
Alaeddine is offline   Reply With Quote

Old   March 15, 2014, 05:31
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 15,849
Rep Power: 122
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
The SWF did not work for me but don't worry about fixing it, I do not wish to see it. The whole point of a frozen rotor approach is that you can model it is steady state. If your tutorial uses a transient model then it has missed the point.

So I would start by doing a steady state model with a frozen rotor frame change model. This might not correctly account for the rotation of the disc, so you will probably need to use the stage frame change model for a better result. But you should not need to use transient rotor/stator which is good because that will take a LONG time to run.

If you have no idea what I am talking about with frozen rotor and stage interfaces then you better look in the documentation. This is all explained in the modelling guide, section 5.3.3 (General Connection and frame change models).
ghorrocks is offline   Reply With Quote

Old   March 30, 2018, 00:57
Default
  #7
New Member
 
arman
Join Date: Feb 2016
Posts: 11
Rep Power: 5
armanpournasiri is on a distinguished road
hello to all
Im new to cfd too
my problem is same Alaeddine but my U=9.39 m/s and rotational velocity is 46.95 rps.
I'm simulating surface propellers. Simulation should be done in a transient way, but I'm not familiar with this method. I'm still analyzing the MRF(frozen approch) technique, but the required values are not right.
You can guide your servant.
thanks
armanpournasiri is offline   Reply With Quote

Old   March 30, 2018, 02:37
Default
  #8
Senior Member
 
urosgrivc
Join Date: Dec 2015
Location: Slovenija
Posts: 334
Rep Power: 6
urosgrivc is on a distinguished road
forces on the surface piercing propellers will fluctuate grately and are dependant upon rotatinoal angle, either if the propeler is in the water or in the air.
forces on the blade vhich is in the air will be totaly diferent from those in the water (like 1000 times diferent).
Which is why steady state doesent work for this case, Steady state will also not capture water splashing around and water mixing with air or surface being efected by the rotation which is like the main thing here.

Water mixing with air is jet a nother big problem. I can see results changing grately with mesh size, turbulent models and surface tention models.

And what about cavitation, air bubles, water splashing, water sticking to the propeller while in air and hull influence on the flow and its properties.

This is a wery chalanging thing to model.
Well you can get cool movies and pictures wery easely but true results will be wery hard to obtain indeed.

I am not saying you cant get true or good results you definitly can
But you need to be an expert with a lot of expirience to model something like a surface piercing propeller.
if you are new to CFD you will soon found out that it is a wery hard topic indeed.

I am using CFD for 5 years now on a daily basis and I am scared of surface piercing propellers, would awoid them if possible.
If you will be doing cfd for the rest of your life than go for it if not you will just die trying with this example.
If you are new to cfd just do something like 100 times simpler, almost any case will be simpler than this.
There are CFD competitions you know, this case might win you a reward if done corectly.
Complexity is much much less if the propeller is not surface piercing (totaly diferent case)
Wish you best of luck

Last edited by urosgrivc; March 30, 2018 at 09:43.
urosgrivc is offline   Reply With Quote

Reply

Tags
advance ratio, cfx, propeller, thrust, transient

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
[Commercial meshers] ICEM CFD and ANSYS CFX tutorials Hutaru OpenFOAM Meshing & Mesh Conversion 1 November 21, 2011 03:38
how to map resultd from cfx to ansys? ritesh CFX 2 June 1, 2011 08:52
Ansys CFX vs CFD for multiphase+particle zeitoun ANSYS 1 June 4, 2010 04:58
Will the ANSYS - FLUENT- CFX kill freedom of CFD? Ben Main CFD Forum 17 September 20, 2006 04:36
FSI using CFX and ANSYS Bi Chang CFX 2 May 10, 2005 05:47


All times are GMT -4. The time now is 21:26.