# Recommended convection schemes for swirling flow in diffuser

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

 August 23, 2005, 05:17 What convection schemes for U, #1 Senior Member   Håkan Nilsson Join Date: Mar 2009 Location: Gothenburg, Sweden Posts: 196 Rep Power: 10 What convection schemes for U, k, epsilon would you recommend for swirling flow in diffusers, in simpleFoam? It should be at least second order, yet being numerically stable. I am not familiar with all of the impressive amount of convections schemes that are available in OpenFOAM. I have so far been able to compute a reasonable solution using Gauss upwind for all variables. When I restart from this solution using Gauss vanLeer or Gauss MUSCL the solution diverges rapidly. Are there any special precautions that should be made when changing schemes? Håkan.

 August 23, 2005, 05:57 I would choose limitedLinearV #2 Senior Member   Join Date: Mar 2009 Posts: 854 Rep Power: 15 I would choose limitedLinearV 1.0 for U and limitedLinear 1.0 for k and epsilon unless you experience further divergence problems in which case I would revert back to upwind on those two. limitedLinear is a new scheme in version 1.2 released yesterday. kiddmax likes this.

 August 23, 2005, 07:37 What about linearUpwind? Is it #3 ghanshyam Guest   Posts: n/a What about linearUpwind? Is it second order upwind? If so why document(user guide) shows "First/second order". I am confused? Please clarify. Regards GS

 August 23, 2005, 07:43 The linear upwind scheme is fo #4 Senior Member   Join Date: Mar 2009 Posts: 854 Rep Power: 15 The linear upwind scheme is formally second-order but it is implemented in OpenFOAM via limited weighting factors rather than a deferred correction and it is the application if the limiter that reduces the order of the scheme where the limiter is required. If you would like a formally second-order version of linear upwind take a look at the cubicCorrection scheme and implement an equivalent for linear upwind. The reason we haven't bothered doing this is that linear upwind isn't a very good scheme and we offer better alternatives.

 August 23, 2005, 07:56 Thanks Henry for the clarifica #5 ghanshyam Guest   Posts: n/a Thanks Henry for the clarification. So you mean "limitedLinearV" is equivalent to "second order upwind"? Regards

 August 23, 2005, 08:06 limitedLinearV is TVD limited #6 Senior Member   Join Date: Mar 2009 Posts: 854 Rep Power: 15 limitedLinearV is TVD limited version of central-differencing where the limiter is formulated taking into account the direction of the change in velocity. As with all TVD and NVD schemes the limiter introduces a first-order contribution to the basic scheme and so second-order behaviour of the limited scheme cannot be guaranteed, it depends on the case and the way in which the limiter is applied as a consequence of the particular field and flow distributions.

 August 23, 2005, 08:33 Does that mean that as of now #7 ghanshyam Guest   Posts: n/a Does that mean that as of now OpenFOAM is not having any "strictly second order upwind" scheme? Regards

 August 23, 2005, 08:49 No and I guess nor does any ot #8 Senior Member   Join Date: Mar 2009 Posts: 854 Rep Power: 15 No and I guess nor does any other code because as soon as the mesh is skewed the second order upwind face interpolate is not in the centre of the face, i.e. not at the Gauss point in which case the scheme is not actually second-order unless a strictly second order skewness correction is applied.

 August 23, 2005, 08:57 If you are particularly keen o #9 Senior Member   Join Date: Mar 2009 Posts: 854 Rep Power: 15 If you are particularly keen on having the linear upwind scheme implemented as a deferred correction on either upwind (as in commercial CFD codes) or central differencing we would be happy to implement either or both for you as part of your support contract.

 August 23, 2005, 10:23 Should it be possible to resta #10 Senior Member   Håkan Nilsson Join Date: Mar 2009 Location: Gothenburg, Sweden Posts: 196 Rep Power: 10 Should it be possible to restart a solution from version 1.0.2 in version 1.2 (simpleFoam)? I get the following error message when I try to do so. keyword pRefCell is undefined in dictionary "../sdTc1/processor0/../system/fvSolution::SIMPLE"

 August 23, 2005, 10:28 Generally yes but for some cas #11 Senior Member   Join Date: Mar 2009 Posts: 854 Rep Power: 15 Generally yes but for some cases you might have to make small changes to fvSchemes and/or fvSolution. For various good reasons I have changed the way in which the pressure reference cell and value are specified to make it more transparent and flexible. In your case simply add pRefCell 0; pRefValue 0; to fvSolution::SIMPLE and then the case should run as before. I have setup FoamX to insert these specifications automatically if they are not present.

 August 23, 2005, 10:56 Then I have a question on how #12 Senior Member   Håkan Nilsson Join Date: Mar 2009 Location: Gothenburg, Sweden Posts: 196 Rep Power: 10 Then I have a question on how the pRefCell and pRefValues are treated when using a constant pressure outlet boundary condition. Are they neglected? In my case I try to avoid the constant pressure outlet, but it would help me understand OpenFoam better if I knew the answer to this question. Is it a good choise to add div((nuEff*dev(grad(U).T()))) Gauss linear; to divSchemes, which was also not present before? It's great that you make the code more transparent, I was wondering about where and to what value the reference pressure was set before. Now I can clearly see it in the setup files.

 August 23, 2005, 11:05 pRefCell and pRefValues are no #13 Senior Member   Join Date: Mar 2009 Posts: 854 Rep Power: 15 pRefCell and pRefValues are not used when using a constant pressure outlet boundary condition which is the same as in previous versions. > Is it a good choise to add div((nuEff*dev(grad(U).T()))) Gauss linear; Yes. Look at the tutorial cases if you are unsure about these choices. > I was wondering about where and to what value the reference pressure was set before. It would have defaulted to a value of 0 in cell 0.

 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 sek OpenFOAM Running, Solving & CFD 38 July 31, 2017 14:30 christian OpenFOAM Running, Solving & CFD 3 December 17, 2007 09:21 Felix CFX 3 February 27, 2007 22:03 Joseph FLUENT 1 October 21, 2003 05:53 Olu Bolumole CFX 1 March 28, 2000 17:24

All times are GMT -4. The time now is 20:28.

 Contact Us - CFD Online - Privacy Statement - Top