# problems with solution convergence

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

 October 24, 2000, 12:00 problems with solution convergence #1 Roberto Ciardulli Guest   Posts: n/a I would like to study the steady-state intake flux of a 4-valves cylinder head, but calculations don't seem to give a stable solution when I use some types of boundaries. According to the experimental method I've defined two boundaries: 1. INLET boun. at the beginning of the intake arm; 2. PRESSURE boun. at the bottom of the cylinder (instead of the piston surface) After more than 1000 iterations residual values are still high and don't seem to get lower. Since I'm a newbie with Star, I'm afraid I could have made many mistakes setting the values of the various parameters (e.g.: initialization; monitoring and reference; turbulence intensity and mixing lenght; etc.). I have chosen the SIMPLE algoritm and the UD diff. sch.; is it ok ? And what about underrelaxation factors? As you can see I still have to learn many things, but if anybody could answer to some of these questions it would be of great help for me. Thanks in advance, Roberto

 October 24, 2000, 16:10 Re: problems with solution convergence #2 John C. Chien Guest   Posts: n/a (1). Run a flow through a cylinder case first. (2). Then run a flow through a sudden pipe expansion case. (3). Put the valve face in the center of the inlet pipe to simulate the valve inlet condition. Then run a case. (4). At that point, you should be able to find out why you are having trouble in getting converged solution. (5). Don't forget about the mesh independent solution issue when you are creating meshes. (6). Also pay attention to the locations of the pipe inlet and the cylinder outlet, especially the flow separations.

 October 25, 2000, 03:59 Re: problems with solution convergence #3 A.Hassaneen Guest   Posts: n/a How are simulating the valve? is it just an orifice? How much is the pressure boundary at the piston (the bottom of the cylinder)? try to use another differencing scheme instead of UD, try the MARS.

 October 25, 2000, 05:59 Re: problems with solution convergence #4 J. Y. Luo Guest   Posts: n/a Hi, Roberto, One likely possibility for non-convergence is that you may have reverse flow at the pressure boundary which is very common for this type of flow because the exit is very large - you should be able to see it in PROSTAR. If this is the case, changing pressure boundary to environmental pressure could solve your problem - there is an option for this when you define pressure boundary.

 October 25, 2000, 10:43 some more questions #5 Roberto Ciardulli Guest   Posts: n/a what do you mean with "mesh independent solution issue"? why should I pay attention to the locations of boundaries and especially the flow separations? what problem is related to them? thanks a lot for your help Roberto

 October 25, 2000, 10:48 Re: problems with solution convergence #6 Roberto Ciardulli Guest   Posts: n/a what does environmental pressure mean? what's the difference between the environ. press. boundary and the STAGNATION boundary? thanks for your hints...I'll try them Roberto

 October 25, 2000, 10:53 Re: problems with solution convergence #7 Roberto Ciardulli Guest   Posts: n/a answers: -I've built the complete mesh of the cylinder+cylinder head using ProICE; - for the the pressure boundary I've set 90 kPa what's the difference between UD and MARS? thanks for your interest, Roberto

 October 25, 2000, 11:11 Re: problems with solution convergence #8 J. Y. Luo Guest   Posts: n/a For incompressible flow, the total pressure = static pressure + 0.5 *density*Vel^2. The stagnation boundary assumes flow always goes into the computational domain. In your case, I think part of flow goes out and part of flow goes in. The environmental pressure option means that for outflow, the pressure specified by you is staic pressure, but for the inflow part, the pressure specified by you is treated as total pressure - thus the flow can be stablised.

 October 26, 2000, 04:49 Re: problems with solution convergence #9 A.Hassaneen Guest   Posts: n/a More question: How much is the reference pressure in PROSTAR? and how much is the pressure at the inlet?? You may ask STAR-CD people about the difference between UD and MARS but difinitely there is a difference in the solution.

 October 26, 2000, 10:29 Re: problems with solution convergence #10 Roberto Ciardulli Guest   Posts: n/a Reference press in Prostar is 100 kPa ; at the INLET I have set just the velocity since it's an INLET bound. By the way, is it possible to set the pressure for that type of boundary? Bye, Roberto

 October 26, 2000, 23:20 Re: problems with solution convergence #11 Chung Guest   Posts: n/a You should have strong vortices in the cylinder, which could be very unstable. Try to reduce relaxation factor for "pcor" from default 0.2 to 0.1, or even smaller. Another thing is to extend cylinder longer to put your pressure boundary far away from valve (anyway, it is not a real). Finally, you may still have the residual hanging around 0.01, and that maybe what you can get and it is good enough.

 October 27, 2000, 09:18 Re: problems with solution convergence #12 Roberto Ciardulli Guest   Posts: n/a Before reading your message I had tried to lower relaxation factors for density and viscosity (their default value was 1!!!) and the convergence criterion has been satisfied after only 800 iterations. Thanks anyway for your hints. Bye, Rob

 October 29, 2000, 04:36 Re: problems with solution convergence #13 A.Hassaneen Guest   Posts: n/a Roberto, If the reference pressure is 100 kpa and you assign boundary pressure at the piston surface 90 kpa that means the absolute pressure at the piston is 190 kPa which is higher than the inlet pressure (supposidely that pressure at the inlet is 0 kPa , the ambient pressure). Try to set the boundary pressure at the piston to 0 kPa and see what happens.

 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 anbuselvan FLUENT 1 January 18, 2009 05:00 Ken Adams FLUENT 10 May 17, 2007 05:48 Freeman Main CFD Forum 0 December 7, 2005 18:08 julie FLUENT 4 November 14, 2005 09:35 nick FLUENT 2 February 26, 2001 13:41

All times are GMT -4. The time now is 19:06.