# Step size for sliding mesh...

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 April 6, 2000, 08:55 Re: Step size for sliding mesh... #21 Joakim Majander Guest   Posts: n/a You really need to reduce the time-step in order to get any real time-dependency. 15 degrees is very much, if you wan't time-dependency (I guess you have quite a few blades). You must have many time steps/blade passing in order to see any periodicity. Just as Joern said forget about the absolut/scaled residual values. In the end you must be certain to have enough iterrations/time-step (flow field does not change from iteration to iteration anymore) and enough time-steps (time-dependent flow repeats itself periodically). Certain value of residual has almost nothing to do with this. Residuals can come down and level while the flow field is still far from converged. They can also remain quite high with a converged solution. For a smaller time-step you will need less iterations, since flow field doesn't change that much from time-step to another. There is really no point using over 50 (or even 20) time steps. Sometimes even 5 will do. Yes it is certainly possible, that you'll need quite a few revolutions, but as I said your too large time-step probably kills periodicity. Is your solution now constant, random or constantly going to some direction? If it is constant, you have actually done MRF (MRF is actually sliding mesh, with time step equal to symmetry eq. 4 blades -> 90, 180, 270 etc degrees/time-step). If it is random, your time step is probably too big. If it is constatnly changing to some direction, you need more revolutions. So reduce the time-step, put some monitors (point values, surface integrals, volume integrals) and see how they behave inside a time-step and periodically. Joakim kabz likes this.

 April 6, 2000, 10:03 Re: Step size for sliding mesh... #22 Jack Keays Guest   Posts: n/a As you have gathered, I am not an expert user. I am a degree graduate starting a masters who has been given a package and told use it! No one in the department knows anything about CFD or modelling in this regard so I am entirely on my own. Hence, all and any help is much appreciated. I am using a coupled 2nd order implicit unsteady solver in fluent 5.1. My pressure scheme is 2nd order upwind. I think my grid is fine, but how do I describe it?? Also, how do I locate these regions? My flow is highly unsteady.

 April 6, 2000, 10:06 Re: Step size for sliding mesh... #23 Jack Keays Guest   Posts: n/a How can I ensure my mesh is radially matching at the interface?? Apart from tweaking the mesh??

 April 6, 2000, 10:12 Re: Step size for sliding mesh... #24 Jack Keays Guest   Posts: n/a My solution converges to a value and then it begins to osscillate quiet violently from time step to time step. From maybe e-01 to e-02, up and down. I already monitor the torque, mass flow rates, pressures at inlet and outlet. How do I monitor point values in FLuent 5.1. I don't think I have alphanumeric reporting in this version.

 April 6, 2000, 10:40 Re: Step size for sliding mesh... #25 Joakim Majander Guest   Posts: n/a Are you talking about residuals here? They should be oscillating when you finally reach a periodically steady-state. You can create points from surface/point. Then you can monitor them through solve/monitor/surface. You should be monitoring velocities, k, etc, since your current monitors will probably not change that much from time-step to time-step in a converged solution. It really is hard to give advice without really seeing the case. Too bad you don't have any experienced supervisor.

 April 6, 2000, 11:38 Re: Step size for sliding mesh... #26 Jonas Larsson Guest   Posts: n/a The first thing to try then is the pressure-based solver. It is often better than the coupled solver if you have low Mach numbers. Try getting it to run with the PISO scheme, this should be the best in theory for transient simulations. However, I've often found plain SIMPLE to be more stable and work better. So if PISO gives poor convergence try SIMPLE. Start with 1:st order upwind for the other variables and switch to 2:nd order as soon as you see that it seems to converge well in each time-step. To start the simulations you probably have to reduce the under-relaxation parameters a bit from the defaults. What you are doing is difficult and something that you need CFD experience to do well... so you'd better learn fast ;-)

 April 7, 2000, 09:33 Re: Step size for sliding mesh... #27 Jack Keays Guest   Posts: n/a I will try it as you say with the pressure-veocity coupled using the PISO scheme. Should I set the pressure the 1st order upwind?? Does the fact the I am using a segregated solver not mean that the pressure and velocity should not be coupled??? OBviously not.

 April 7, 2000, 09:50 Re: Step size for sliding mesh... #28 Jack Keays Guest   Posts: n/a Jonas, Do you recommend any good books/papers which I should read as a CFD novice??? I have A book called "An introduction to CFD" by Versteeg. That is it. Hope I'm not cluttering up your form with all my messages. )

 April 10, 2000, 02:43 Re: Step size for sliding mesh... #29 Jonas Larsson Guest   Posts: n/a Start with 1:st order but switch to 2:nd order as soon as you see that it doesn't diverge. The fact that you use the "segregated solver" refers to the way you solve the equations. Most basic CFD books should explain this quite well. You still, of course, have a coupling between velocity and pressure.

 April 11, 2000, 09:24 Re: Step size for sliding mesh... #30 Jack Keays Guest   Posts: n/a My residuals are oscillating, but they are oscillating between 1e-01 and 1e-05 (converged). Is it o.k. for them to oscillate between such extreme values?? I am getting very good results. The mass imbalance is a fraction of one percent and the vaules are repeating themselves revolution to revolution, so it is periodic. Does the range of the residual oscillation say much about the solution??? Is it imprtant? Why?? thanks! )

 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 pUl| FLUENT 31 August 21, 2015 04:46 siw ANSYS Meshing & Geometry 24 August 24, 2010 11:22 panara OpenFOAM 2 February 20, 2008 15:37 skabilan OpenFOAM Running, Solving & CFD 12 September 17, 2007 17:48 msrinath80 OpenFOAM Running, Solving & CFD 9 July 22, 2007 02:58

All times are GMT -4. The time now is 09:27.

 Contact Us - CFD Online - Privacy Statement - Top