# Convergence of Radial Turbine Simulation

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

 July 15, 2004, 09:31 Convergence of Radial Turbine Simulation #1 Hugh Guest   Posts: n/a I am undertaking CFX analyses of a nozzleless radial turbine but am having great difficulty in achieving convergence. If I use a high fluid time step then I get a 'fatal overflow' error and if I use a small fluid time step then the error is a problem with a computed static pressure less than or equal to zero with recommendations to use an even smaller time step. Are there any suggestions on how this problem can be solved? Many Thanks!

 July 15, 2004, 18:17 Re: Convergence of Radial Turbine Simulation #2 Glenn Horrocks Guest   Posts: n/a Hi Hugh, Is your mesh fine enough? Are your physical models appropriate for the physics of the simulation? I'll bet the answer to one of those questions is no. Glenn

 June 25, 2010, 01:48 #3 New Member   Karthik Ravishankar Join Date: Jun 2010 Posts: 4 Rep Power: 7 Hi..... I'm new to CFX. I'm trying to simulate a base case for a radial inflow turbine only the runner. The runner is of a turbocharger, inlet area 49mm*26mm Here are my settings: Domain: Fluid domain, rotating, 68K RPM, Axis Z, clockwise rotation, ref pressure 1 atm Init: Rotating, Velocity initialized in cyl. coord. as -30m/s(radially inward) in radial direction in rotating frame, 400'C temp and 0 atm rel. press. Inlet: Rotating frame, 600'c and 2 bar inlet pressure, flow direction cyl coord: 0,-1,0(a,r,t) Outlet: Rotating frame, 0 atm rel pressure(static). Periodicity is ensured 1 to 1 Meshed in ICEM, quality above .25 min angle 18' About solver: High res, 1st order and Phy timescale .5 sec I know a little about most of to params i have given......I am giving all settings so that someone can help me.... Coming to actual prob.....The solver either oscillates very badly and flow reversal error appears to close 80% of both inlet and outlet boundaries. Or sometimes the solver doesnt even start saying a param DOMVEL is uninitialised Someone pls help me....i'm running outta time

 June 25, 2010, 06:39 #4 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 10,823 Rep Power: 85

 June 25, 2010, 11:09 #5 Senior Member     Attesz Join Date: Mar 2009 Posts: 355 Rep Power: 8 My suggestions: - do you calculated the initial values correctly? if not sure, use automatic initialisation instead - first run a simple steady state simulation, but use high resolution. - you can use aggressive time step, and if there isn't any convergence problems, you can increase the scale factor, to 5 or 10. - first run a semi-load operation point, for example on the desired rotating speed but much lower pressure ratio. the convergence of these points are more stable and fast. from the results you can increase the pressure ratio using interpolation. Send picture about the mesh and the conv. curves if you can. Regards, Attesz

 June 26, 2010, 01:43 #6 New Member   Karthik Ravishankar Join Date: Jun 2010 Posts: 4 Rep Power: 7 Hi.... thanks for reply Automatic initialisation does not work. an error: subroutine getVar is not able to retrieve parameter DOMVEL in ZN1 occurs. The values for velocity i have given are tentative only. However 1 of the trials did converge though with high reversal of flows at the outlet. From the post i found out the mass flow rate at inlet and changed the inlet boundary as mass-flow inlet and stat press outlet.... BUT.....this worked for coarse mesh but in the fine mesh....the RMS-P mass oscillated very vigorously after 90 iterations and did not converge......? I also have confusion abt the sign of velocity init. I have given -30m/s radial.....because inward.....is this right? or should i jus give 30m/s ?????? Wall formation at the outlet due flow reversal occurs very frequently upto 80%.... How should i define the outlet boundary frame type: ???? Rotating or stationary?? because i am not defining any flow direction or vectors at the outlet thanks for reply once again Karthi

 June 26, 2010, 07:28 #7 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 10,823 Rep Power: 85 Attila - the FAQ I linked to does not discuss initial guesses or ramping up to full flow. These are both very useful techniques - can you add them to the FAQ? Questions like this get asked very often so let's make the FAQ as good as possible. Karthik - It is common for a coarse mesh to diverge and a fine mesh to diverge. The finer mesh is capturing finer flow features which are more difficult to converge and may also start being transient and therefore require careful consideration. The coordinate system is defined in the documentation. Just output your initial guess and look at it in Post if you don't trust it. The wall formation at outlet indicates you have backflow at the outlet. Can you move your outlet downstream? This is by far the best way to deal with it.

 June 29, 2010, 10:18 #8 New Member   Karthik Ravishankar Join Date: Jun 2010 Posts: 4 Rep Power: 7 Thnks all....ghorrocks.....i found the flaw.....it was with time stepping and inlet total pressure conditions......... Now i need help in one more aspect.........i'm modelling an internal channel to cool the leading edge of the blade... channel dia is 1/3rd blade thickness....i'm using air at 2 bar 150'C as coolant.....i've meshed in ICEM and imported into CFX and made the domains...... My doubt is once i have created a domain interface, an interface boundary is automatically attached to both the domains.......but is it necessary is explicitly define the common wall boundary as CHT boundary........? Secondly.....which parameter that we set in solid domain definition defines the solid to conduct heat inward..... Thirdly....how should i make the surface heat on the blade surface to interract with the cooling effect of the fluid in internal passage? if u can help me......any help....pls do so..... thnks in advance karthi

June 29, 2010, 18:50
#9
Super Moderator

Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,823
Rep Power: 85
Quote:
 is it necessary is explicitly define the common wall boundary as CHT boundary........?
If automatic detection of interfaces is on it will have a go at doing it automatically. Always check that the interface it generates is sensible before using it. Otherwise just generate it manually.

Quote:
 which parameter that we set in solid domain definition defines the solid to conduct heat inward
No such thing. You sent the initial and boundary conditions to have a temeprature field and the heat flows accordingly. You do not define the heat flow to be in a certain direction.

Quote:
 how should i make the surface heat on the blade surface to interract with the cooling effect of the fluid in internal passage?
That is automatically handled in a CHT solution.

These are pretty basic CHT questions. Sounds like you should do the CHT tutorial in the CFX tutorial manual. Have a look at the heater coil example, that will help you.

 June 30, 2010, 03:07 #10 New Member   Karthik Ravishankar Join Date: Jun 2010 Posts: 4 Rep Power: 7 Thnks So basically wat you mean.....is tht domain interfaces are optional .....So i can avoid creating domain interfaces.......instead i can define the blade's interior channel wall as a non-adiabatic wall and give some heat transfer prop to it....right?

 June 30, 2010, 08:08 #11 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 10,823 Rep Power: 85 In that case remove the mesh for the cooling channel and just impose your boundary condition on the coolant channel wall.

 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 cnchilavert CFX 2 October 5, 2011 04:23 Andy QUB FLUENT 4 August 23, 2011 09:49 Petro FLUENT 0 December 29, 2010 09:04 Jonas Pedro Caumo CFX 0 December 9, 2006 14:54 md nizee Main CFD Forum 2 December 6, 2000 03:08

All times are GMT -4. The time now is 08:37.