# Flow around a rotor

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

August 16, 2013, 07:31
Flow around a rotor
#1
New Member

Gerrald Gelderblom
Join Date: Nov 2012
Posts: 24
Rep Power: 6
Hi everyone,

I am simulating a rotor, and want to use the characteristics in either a profile boundary condition or a source term in a bigger domain. My idea is to model the rotor in a tube. I use a rotating reference frame for my fluid domain, zero velocity at the rotor relative to the fluid domain and zero absolute velocity at the walls. The inlet and outlet are pressure inlet and outlet.

When I look at results, I find that the velocity is in most of the domain dominated by the axial component. At the rotor I find a high tangential velocity and at the wall I find zero velocity. So far so good, and in correspondence with expectations. Though I find a strange phenomenon; near the wall is a region of high tangential velocity, in the direction of my reference frame motion. Does anyone have an idea of why this happens?

Attached Images
 Velocity at XZ plane.jpg (51.5 KB, 21 views) Velocity at rotor.jpg (21.2 KB, 21 views) Velocity at Wall.jpg (35.5 KB, 19 views)

 August 16, 2013, 07:52 #2 Senior Member     Alex Join Date: Jun 2012 Location: Germany Posts: 1,548 Rep Power: 25 Do you mean the velocity vectors in the second picture? If this is the velocity in the stationary frame of reference, everything is ok.

August 16, 2013, 07:59
#3
New Member

Gerrald Gelderblom
Join Date: Nov 2012
Posts: 24
Rep Power: 6
No I mean the first one, the vectors at the plane aligned with the rotor. The others are just to show that the velocities (indeed in stationary frame) are ok at the wall and rotor.
For more clarity, see the attached image of the vectormap at the inlet. You see some tangential velocity near the wall.
Attached Images
 Velocity at Inlet.jpg (42.5 KB, 8 views)

 August 16, 2013, 09:05 #4 Senior Member     Alex Join Date: Jun 2012 Location: Germany Posts: 1,548 Rep Power: 25 I dont understand the problem. Why shouldnt there be a tangential velocity near the wall?

August 16, 2013, 09:40
#5
New Member

Gerrald Gelderblom
Join Date: Nov 2012
Posts: 24
Rep Power: 6
In my opinion this solution is unlikely. The maps show that there is a zone of very low (tangential) velocity in between the rotor and the wall. So how could the momentum be transported. What is the mechanism that causes the high velocity near the wall?

I'm affraid this proves my approach to be inadequate, but I don't see the problem. Alternatively, if you can argue this solution is credible I'm also happy of course.

To support the statement of the zone of low velocity, see the attached maps. These images don't provide a clear view on velocity in radial and axial direction of course, but I added streamlines to show that the velocity field is really dominated by tangential velocity near the wall throughout the domain. I added the seedpoints at r=2.5m while the tube has r=3m.
Attached Images
 Velocity vertical planes ISO.jpg (71.4 KB, 10 views) Velocity vertical planes Top.jpg (31.3 KB, 12 views) Streamlines.jpg (75.7 KB, 11 views)

 August 16, 2013, 10:10 #6 Senior Member     Alex Join Date: Jun 2012 Location: Germany Posts: 1,548 Rep Power: 25 Now I think I got it. But before blaming your simulation approach and rejecting it, did you make sure that the solution converged properly and that the other parameters of your setup are reasonable? For example, I dont see where you could place a pressure inlet or outlet in the domain. To me, all bondaries should be walls to simplify the model. And about the rotating reference frame for the whole fluid...this seems disputable.

 August 16, 2013, 10:41 #7 New Member   Gerrald Gelderblom Join Date: Nov 2012 Posts: 24 Rep Power: 6 The domain doesn't look like the real domain, for my actual simulation I have to model a very large tank. As a first attempt I used MRF, but in the large domain I didn't manage to find a proper converged solution. In the images, the top is an inlet, the bottom is an outlet. Both have 0Pa Gauge pressure. I did this because in a large tank, the pressure is far from the rotor is equal at both sides of the rotor. As far as I know this approach should in a stationary frame provide exactly the same results as having a stationary domain and a moving wall, isn't it? I used this approach because physically the rotor is moving and not the wall, but maybe I overlooked someting. Which other parameters are you interested in? I use a mesh with +-1.2M cells. For turbulence I use regular k epsilon. I now see that my Y+ values are high, at the rotor they vary between 85 and 1200 (1200 near the tips), and at the wall between 400 and 1000 (I never found a proper explanation of desired values for y+ though). Standard wall functions. The residuals drop to around 4e-4. I also monitored velocity at certain locations, and volume and area averaged monitors of turbulence kinetic energy, and everything stabilized.

 August 16, 2013, 11:42 #8 Senior Member     Alex Join Date: Jun 2012 Location: Germany Posts: 1,548 Rep Power: 25 So let me get this straight: The domain in the pictures is just the rotating part you want to use later in a MRF simulation. The domain in the figures has a rotating reference frame. The outer boundary is a stationary wall with respect to the rotating frame If I got this picture correctly (maybe you could explain it better if I didnt) we are looking at a bucket. Instead of stirring the bucket with a mixer, you just hold the mixer and turn the bucket at the same rotational speed. These two options are not equivalent. As far as the Yplus values are concerned: The fluent theory guide covers this topic. Values of 400-1000 will render any simulation with standard wall functions useless. Maybe with lower values of Yplus, you will get better convergence.

 August 17, 2013, 07:04 #9 New Member   Gerrald Gelderblom Join Date: Nov 2012 Posts: 24 Rep Power: 6 I don't want to do a MRF simulation. I want to study the characteristics of the rotor. This information I will later on use in either: A 'Momentum Source Model' which I am programming in a UDF. This is an alternative to previous MRF attempts. A shared surface with at one side a velocity inlet boundary condition, in which I have to write a UDF for the pressure distribution, and at the other side a pressure outlet boundary condition with a direction vector for velocity. It is not actually a bucket but a pipe section. Where do you find a proper definition of maximum yplus values? I only find that ystar has a maximum dependent on the Reynolds number, which can vary between 100 and a few thousands. Mine has a maximum of 1000. The two options you describe are indeed equivalent in my opinion, though only if you look at the solution from the right reference frame. Is that not true? In my model I rotate the rotor, and hold the pipe. And even than I have two options, use a rotating reference frame (with rotor speed 0rpm, wall speed 42rpm) or use a stationary reference frame (with rotor speed 42rpm, wall speed 0rpm). I chose the first one, because I thought using a rotating wall will probably cause continuity troubles if the boundary is not axisymmetric. Before I used prism meshing (leading to y+ to around 150), but I didn't find a difference in my solution, except increased computational costs.

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post popezmark OpenFOAM 8 February 4, 2014 19:00 tlemonds CFX 3 April 1, 2013 18:49 steamerandy Main CFD Forum 0 October 31, 2011 22:08 CD adapco Group Marketing Siemens 3 June 21, 2011 08:33 cfd_newbie FLUENT 3 September 22, 2007 10:48

All times are GMT -4. The time now is 20:00.