Laminar pipe flow

[Anonymous]

Hello,

I have been trying to simulate a simple laminar flow in a pipe, however the pressure drop is resulting to be much higher than the analytical value.  my Reynolds number is approx 2000, so i have been selecting laminar flow, and ticking the fully developed when selecting the flow rate at the inlet.  The solution monitor was put to tight, choosing Advection 2.  I have tried both the solution both with automatic mesh using 5 enhancement layers;  as well as with manual mesh using 32 nodes on surfaces and 16 nodes on the volume and 5 enhancement layers.  however they are both resulting to the same solution which is much larger than the simple analytical value.  comments or thoughts? thanks! rob

[Anonymous]

Hello, just wondering if someone can help on this issue please. It seems very hard to match a simple laminar pipe simulatio to analytical values, even when in 2D. thanks

[OmkarJ]

Few basice things come to mind:

1) Is the solution adequately mesh independenet?

2) Are you sure you are measuring the pressure drop over same length of the pipe?

3) Have you tried ADV 5 discretization scheme? If you have treid ADV2, both should be close though.

Regards

OJ

[Anonymous]

Dear Omkar, 

Thanks for your reply.  It seems that the mesh independence is playing a huge role.  But on a pipe 10mm diam, 500mm length i am ending with more than 3M elements, tight settings with pressure and velocity settings put down to 0.2.  I though is was too much for the simplicity of the geometry and was wondering if there is a better way.   Ive also tried a 2D simulation but which was resulting in a ridiculously high pressure.  

Is there a suggested meshing scheme for laminar flows (100<Re<1000) ?

rob 

[OmkarJ]

I see a bit contradiction in your information as you mention in earlier post that Reynolds number is 2000, while in this post, you mention it is less than 1000. Typically, for Reynolds number between say 1500 to 4000, it may help to simulate using Low Re. Care should be taken here since the wall log laws are abolished and you need to make sure that the mesh enhancement is turned on, with preferably 5 layers. Also, you may want to see that Y+ values over the solution walls are close 1, to fully resolve the boundary layers.

Though, this may be a bit overkill if you are merely interested in the area-averaged pressure drop nad not flow separation, reattachment etc. 

Also, is there a reason to reduce the under relaxation factors to 0.2? Why not 0.4/0.5 etc? Higher value of line-search should help you get to the covnergence faster and also recognize if you are reaching the asymptotic range of average results in the plots. For low factors, the slopes may be smaller and may fool the automatic convergence assessment settting in the software into assuming the convergence. I personally turn off the convergence assessment and rely on assessing the parameters of interest at monitor points, resid out/resid etc to judge the covnergence.

Regards

Omkar

[Anonymous]

Hi Omkar,

No contradiction, I am trying to get a chart of flow vs pressure not just simulate one condition.  I understand that between 1500-4000 there may be a transition and that low RE may be a better model.  thanks for advice on Y+

However for low Re values between 100-1000 i am using the laminar model but still endingup with about 25% error.  Can you advice on the correct procedure for this type of simulation please?

thanks. rob

[Anonymous · Accepted solution]

hi Omkar, 

It seems that when you are investigating a developed flow and apply a flow rate boundary condition, you need to have an additional length to the pipe you are investigating to allow the flow to develop.  This despite the fact that SimCFD2013 has a new "developed flow" tab in the boundary conditions which you can check.  This tab will still provide you with an over estimation when compared to the analytical solution - and is likeley to be due higher pressure in the entry length.

[OmkarJ]

Glad it worked out. When you say additional length, do you mean at outlet or inlet. You will always need an additional length at the outlet, irrespective of how you specify inlet, fully developed flow with smaller inlet or uniform flow with longer inlet! Or, are you saying that fully developed flow specified at inlet  with smaller and longer  lengths of inlets yield different results? Now that will be a news, and a serious concern!!

Typically, even if the empirical formulae are used to estimate the lengths required for fully developped flow, it always helps to check this by plotting the velocity in streamwise direction to ensure there are no gradients in both inlet and outlet directions. 

OJ

[Anonymous]

Hi Omkar,

additional length means, that if you need to analyze the pressure drop for a developed flow in 500mm pipe you must have an additional lenth to before that to allow the flow to become developed and compare well to theory.

Can you please advice on how to plot velocity profile in stream wise direction? Also are you able to give me more information (or a link) on what the Advection models 1-5 do?

thanks - rob

[OmkarJ]

I understand what you meant and I clarified the same thing earlier. What I was asking is, did you get different results with different lengths of inlets even after specifying fully developed flow 🙂

You can find the help documentation here:

Advection schemes: 

http://wikihelp.autodesk.com/Simulation_CFD/enu/2013/Help/0138-The_Proc138/0347-Solving_347/0357-Sol...

XY plot for velocity in streamwise direction:

http://wikihelp.autodesk.com/Simulation_CFD/enu/2013/Help/0138-The_Proc138/0384-Results_384/0387-Pla...

Cheers 

OJ

[Anonymous]

Hi OJ,

I didnt try different lengths.  I made sure its long enough (twice as much as what the entrance length equation says) to be on the safe side.  My guess is that as long as you have it longer than the entrance length you should not see a difference.

Thank you very much for the links! very helpful indeed!

Rob