# looks simple,but confusing,a pipe flow problem!

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

 March 11, 2003, 22:55 looks simple,but confusing,a pipe flow problem! #1 W.Z.H Guest   Posts: n/a Recently, i am using a pipe flow case to test fluent's calculation. size of the pipe: D =23mm,L=0.1m; boundary condition:velocity inlet1.5m/s; pressureoutlet:0pa(gauge pressure) i have tried two turbulent models(standart k-e and RSM),but neither leads to the just result(mainly the pressure drop ) corresponds to the empirical formulas(this is a typical case,you can find the relative fomulas in the literatures). i have check the mesh carefully,and also adapt the cells near the wall,but it seems nothing favors the final results . what is wrong?? is it possible the cassical emprical correlations are wrong? or the fluent model are not exact? thanks for any suggestion!

 March 12, 2003, 03:55 Re: looks simple,but confusing,a pipe flow problem #2 HVN Guest   Posts: n/a Are you sure that your flow is turbulent?

 March 12, 2003, 04:35 Re: looks simple,but confusing,a pipe flow problem #3 W.Z.H Guest   Posts: n/a wether it is turbulent or laminar can be easily judged by the Re number,(>2320),surely it is turbulent.

 March 12, 2003, 04:46 Re: looks simple,but confusing,a pipe flow problem #4 Christian Guest   Posts: n/a Hm. I get Re=u*dh/vis=1.5*0.023/1.7e-5=2030 i.e. transition if disturbed and laminar if not disturbed. If you use the length (L=0.1m) to calculate the Re you get a larger number, but I dont think that would be correct. The diameter is the correct "length".

 March 12, 2003, 05:12 Re: looks simple,but confusing,a pipe flow problem #5 HVN Guest   Posts: n/a It isn't so easily to judge if a flow is turbulent or not when you are in the transition domain (see your Re number). Increase your velocity inlet to be sure to have a turbulent flow and normally you will find the same results as the theory.

 March 12, 2003, 08:51 Re: looks simple,but confusing,a pipe flow problem #6 Tom Guest   Posts: n/a The classical empirical correlations are correct, no doubt about that. Turbulence models are never completely exact, so you always find some deviations. The question is if the deviations are large in your case. Perhaps the Reynolds is low and low Reynolds turbulent flows are quite difficult to predict. Tom

 March 12, 2003, 11:03 Re: looks simple,but confusing,a pipe flow problem #7 Christian Guest   Posts: n/a The classical correlations may be correct, but you have to know how to use them. One has to be very careful to choose the correct correlation for the setup. And as I and HVN have pointed out the flow is in a Re area where it is difficult to determine if it is laminar or turbulent. If WZH uses the wrong correlation for the setup, strange results may be expected.

 March 12, 2003, 12:17 Re: looks simple,but confusing,a pipe flow problem #8 Erwin Guest   Posts: n/a Also: the pipe length is too small to set up a developed flow. Generally the empirical relations apply for pipes that are longer than 10 times the diameter. So make your pipe at least this long and then postprocess your run for the piece of pipe after that.

 March 12, 2003, 22:19 Re: looks simple,but confusing,a pipe flow problem #9 W.Z.H Guest   Posts: n/a the flow in that is turbulent,get the Re=u*dh/vis=1.5*0.023/1.007e-6=34260(you got the wrong viscosity?) , maybe Erwin is right,for a fully develop flow ,the pipe length should be more than 10 times of the tube diameter

 March 13, 2003, 03:30 Re: looks simple,but confusing,a pipe flow problem #10 Christian Guest   Posts: n/a ny=1.007e-6 ??? My book ("introduction to heat transfer" by Incropera & DeWitt) says that the kinematic vis. is : ny=11.44e-6 @ T=250, ny=15.89e-6 @ T=300, ny=20.92e-6 @ T=350, and I dont recall WZH mentioned a temperature so I assumed that it was in that range. Where do you find your viscosity ? I agree that the flow isnt fully developed and that most correlations assume fully developed flow, but it is possible to compensate for this (empirically also). This, of course, adds an additional "error" to the result. But it can be estimated.

 March 13, 2003, 04:03 Re: looks simple,but confusing,a pipe flow problem #11 Christian Guest   Posts: n/a And I assume that the fluid is air, btw.

 March 13, 2003, 04:52 Re: looks simple,but confusing,a pipe flow problem #12 W.Z.H Guest   Posts: n/a sorry, i have not made it clear that the fluid is water. and when the fluid is water, the Re number is much more than that results from air. anyway,thank you, Christian.

 March 13, 2003, 05:54 Re: looks simple,but confusing,a pipe flow problem #13 Christian Guest   Posts: n/a Oh. Water. Hm. I should have thought of that possibility. Guess that I am too accustomed to deal with air If you decide to follow Erwins suggestion or try to compensate for the inlet conditions in your analytical calculation it would be nice to know about the result. Good luck.

 March 14, 2003, 05:12 Re: looks simple,but confusing,a pipe flow problem #14 Volker Pawlik Guest   Posts: n/a Hi, or set a fully develloped velocity (and if necessary kand eps-) profile at your inlet! You can do that by an UDF or by a translatoric periodic calculation (setting inlet and outlet as periodic). Unfortunately there is a bug in fluent 6.0 with that model, it gives divergence. But with fluent5.5 it works fine. Volker

 March 14, 2003, 08:27 Re: looks simple,but confusing,a pipe flow problem #15 v. price Guest   Posts: n/a I'd try looking at the fanning friction factor at a 'point' in the pipe where the flow is fully developed. Get that agreeing with empirical then start to consider the accuracy of the developing inlet section.

 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 keng Main CFD Forum 1 March 5, 2010 11:40 vismech STAR-CCM+ 1 August 11, 2009 10:38 Munni Main CFD Forum 5 April 20, 2007 03:15 sudha FLUENT 3 April 28, 2004 08:40 Tom Cloutier Main CFD Forum 0 April 20, 2003 13:19

All times are GMT -4. The time now is 15:00.