# Density/Temperature problem

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

 May 28, 2009, 10:08 Density/Temperature problem #1 Senior Member   Join Date: Mar 2009 Posts: 203 Rep Power: 9 Hey guys, I've got a problem and i have no idea what I can do. I have a pipe, in this pipe I have a second smaller pipe. In each pipe is a gas. The gas in the big pipe has 300°C and the gas in the small pipe has 25°C. When I make a run the Energy and the second gas don't converges. When I look at the density or temperature in the geometry scene I see the problem. 3-5 cells after the inlet of the second gas the temperature raises up to 500°C and the density falls down. What is here the problem what I have? The mesh looks really good. The gas is non reacting when this is important. When I find no solution I will ask the support...

 May 28, 2009, 12:32 #2 Senior Member   Aroon Join Date: Apr 2009 Location: Racine WI Posts: 148 Rep Power: 8 Is this a conjugate heat transfer problem? If so you may want to check the solid-fluid interface.

 May 28, 2009, 16:06 #3 Senior Member   Join Date: Mar 2009 Posts: 203 Rep Power: 9 I want to see the "mixing" of the two gases. But I think the problem is maybe the second small pipe for the second gas. I will make a run without the second gas, maybe there is already the problem.

 May 29, 2009, 04:25 #4 Senior Member   Join Date: Mar 2009 Posts: 203 Rep Power: 9 So the run is still working. Energy is still on a high level (1.55...E-01) and didn't change very much. Mesh looks good (had made it very fine around the zone which made problems). I will try to make a run without pipe... or change the AMG solver? What do you think? Any ideas how I can bring the second gas into the middle of the other pipe?

 June 2, 2009, 08:50 #5 Member   Join Date: Mar 2009 Posts: 55 Rep Power: 8 You can remove the cells where the temperature is higher than what is realistic. This will replace these 'offending' cells with symmetry boundary cells. This might get rid of your problem, but only do so if only relatively small number of cells are causing problem.

 June 2, 2009, 13:19 #6 Senior Member   Join Date: Mar 2009 Posts: 203 Rep Power: 9 There were only 3-5 cells where I have the problem. The temperature is lower now. I have made the cell size smaller in this area. Tomorrow I should know if it works. /edit: How can I remove this "bad" cells?

 June 3, 2009, 03:36 #7 New Member   Join Date: Mar 2009 Posts: 20 Rep Power: 8 Hi, my experience is, that AMG is better for such problems than CG. Also always use double precision. If you do not have conjugate heat transfer in solid you can try to switch the bad cells into solid and they will be ignored during the calculation. Regards xamo

 June 3, 2009, 04:01 #8 Senior Member   Join Date: Mar 2009 Posts: 203 Rep Power: 9 With the smaller cells the temperature peak is no problem anymore. But the energy converged very slow, the second gas also converged very slow. What is "CG"?

 June 4, 2009, 02:03 #9 New Member   Join Date: Mar 2009 Posts: 20 Rep Power: 8 Hi, i´m sorry, I thought this is a STARCD problem.... In STARCD under Solution Method (for Scalar Solver Type) you can choose CG (default) and AMG. CG stands for Conjugate Gradient (algorithm). I do not know if you can choose this in CCM+. Regards xamo

 June 4, 2009, 03:02 #10 Senior Member   Join Date: Mar 2009 Posts: 203 Rep Power: 9 Hmm I tried to simulate a test case and there is the same problem. Mesh is very fine, don't have any idea. Will make a "simple" case today and then look if there is the same problem. When I can't get a solution I will speak to the support. Maybe one bug more...

 June 4, 2009, 04:53 #11 Member   Join Date: Mar 2009 Posts: 55 Rep Power: 8 Both in Fluent and STAR CCM+ energy converges slowly. Also, the make note that the residuals are 'normalised' so the actual values may be very small. In STAR CCM+ you do not have the luxury of changing AMG to CG (as far as I know). The reason you have high temperature in those few cells is because the final qulaity of those cells either after finite volume or interface creation were compromised. This is why you can either remove these cells or remesh to create better quality cells (as you have done). To remove these high temperature cells use split by function (temperature in your case, you may have to use derived part to set the criterion you need). Then you can either delete these newly created region or set the physics to null. Also another method to removel bad cells in general is to right click on the region and select remove invalid cells. This process will create a separate region with bad cells and set them to symmetry boundary conditions. You can either delete them or leave them. I found in some cases I have had to use both of the above methods to get the solution to work. In some cases you have to 'initialise' the solution before removing invalid cells and then re-initialise the solution WITHOUT removing solution. This is especially the case when you are creating these bad cells during the 'interface' creation stage as you initialise the solution. Hope this helps.

 June 4, 2009, 06:37 #12 Senior Member   Join Date: Mar 2009 Posts: 203 Rep Power: 9 Thanks for you answer. I have shown it a other guy and I think we have found a solution. I didn't had changed the specific heat etc. in my gas components, we think because of the different density the solver tried to balance this difference with this high temperature.

 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 Wouter Fluent UDF and Scheme Programming 6 June 6, 2012 04:43 Gianni FLUENT 0 April 5, 2008 10:33 Se-Hee CFX 2 June 10, 2007 06:29 ParodDav CFX 5 April 29, 2007 19:13 Thomas P. Abraham Main CFD Forum 5 September 8, 1999 14:52

All times are GMT -4. The time now is 04:38.