# Determine the torque of a turbine

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

 April 4, 2014, 05:43 Determine the torque of a turbine #1 New Member   Simon Join Date: Apr 2014 Location: Stuttgart, Germany Posts: 22 Rep Power: 3 Hello, I have got some problems to determine the torque of an axial turbine. Because when I´m choosing the mesh goemetrie on the blade (pic 1), the power is about 310W. When I´m choosing the mesh geometrie for the blade (pic 2), hub and shroud, the power is about 90W. The Volume on the pictures is the fluid volume and between is the blade (invisible). Pic1.PNG Pic2.jpg Has somebody the solution? Thx error404

 April 4, 2014, 08:52 #2 Senior Member   Bruno Join Date: Mar 2009 Location: Brazil Posts: 241 Rep Power: 12 If what you are modelling is an axial turbine and you pictures show your entire domain, then your simulation is incorrect, unless you have some really unconventional turbine. You should simulate the entire blade, including leading and trailing edges, plus some region up and downstream of the blade to allow the fluid to "settle" (I don't know what the correct word should be here). Take a look at the tutorial 'Flow in an Axial Turbine Stage'. It covers everything related to your simulation.

 April 4, 2014, 11:27 #3 New Member   Simon Join Date: Apr 2014 Location: Stuttgart, Germany Posts: 22 Rep Power: 3 Thank you for the information, but the tutorial is done with a turbogrid mesh. I made the mesh with ICEM. I have got the "problem" that I haven´t got any gap between the stages. So I have to split it up, in a left and right fluid volumen??

 April 7, 2014, 04:24 #4 New Member   Simon Join Date: Apr 2014 Location: Stuttgart, Germany Posts: 22 Rep Power: 3 Hello, here is a picture of the turbine. blades.jpg

 April 7, 2014, 07:26 #5 Senior Member   Bruno Join Date: Mar 2009 Location: Brazil Posts: 241 Rep Power: 12 Then you might have to model the stator upstream and downstream to your rotor. My guess is that the flow on your geometry will be very tightly coupled, so if you plan on using 'Frozen Rotor' for the interface, be sure to sweep across several different rotor positions. But a transient run with 'Transient Rotor Stator' would probably be a better idea.

 April 7, 2014, 18:22 #6 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 11,057 Rep Power: 86 This looks like a very unusual machine. The "blades" are big blocks which will produce torque when the passages align, but the flow will just about stop when they do not align as the flat front of the blade just about blocks the entire passage. The result of this is I would expect this machine to have a very variable torque versus angle curve (high torque when the passages align, low torque when they do not) and a very pulsey flow rate (high flow when the passages align, low flow when the do not). Where did this design come from? For most applications this is a very poor machine design. But assuming you still want to simulate it, you are going to have to take account of this very pulsey flow. If you are using frozen rotor you are going to need to run lots of angles to get the full flow curve.

 April 8, 2014, 06:53 #7 New Member   Simon Join Date: Apr 2014 Location: Stuttgart, Germany Posts: 22 Rep Power: 3 Thank ghorrocks, I´ll expect the same, regarding the torque plot. When I want to simulate transient and the frequenz is 100 000rpm, very fast. Which time step size should I choose? Is there any flashover value? I know some flashover value. It´s: 1/omega^2, it´s very small--> much calculationtime

 April 8, 2014, 07:20 #8 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 11,057 Rep Power: 86 Why is flashover relevant to this model? What gas is flowing through this thing? CFD = long simulation time. Get used to it Yes, it is very small, but the time for each revolution is very small too. I should write an FAQ on this bit: To set the time step use adaptive time steps homing in on 3-5 coeff loops per iteration. Make sure the max and min time step size are wide enough that it never hits it. And that your initial time step is in the ball park (read the documentation for a guide to setting time step size in turbomachinery). Then the solver will find its own time step. error404 likes this.

 April 8, 2014, 07:28 #9 New Member   Simon Join Date: Apr 2014 Location: Stuttgart, Germany Posts: 22 Rep Power: 3 The fluid is ideal air, compressible. 600 000Pa (Inlet) 101 325Pa (Outlet)

 April 8, 2014, 07:35 #10 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 11,057 Rep Power: 86 So if it is air (ideal gas) then what does flashover got to do with it? Your pressures mean you should be using a reference pressure of 101325Pa, an inlet pressure of 498675Pa and an outlet of 0Pa.

 April 8, 2014, 07:38 #11 New Member   Simon Join Date: Apr 2014 Location: Stuttgart, Germany Posts: 22 Rep Power: 3 The flashover is from a student. He had seen this flashover in the www. for trubomachinery.

 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 Anonymized_JL1 FLUENT 14 September 26, 2013 03:35 sedongjjang FLUENT 0 August 24, 2012 14:13 sedongjjang FLUENT 0 August 24, 2012 14:12 pa-dundas FLUENT 3 August 30, 2011 12:25 manish CFX 4 March 15, 2007 03:57

All times are GMT -4. The time now is 17:07.