CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   STAR-CCM+ (http://www.cfd-online.com/Forums/star-ccm/)
-   -   Divergence / Convergence for different inlet extrusion lengths (http://www.cfd-online.com/Forums/star-ccm/93725-divergence-convergence-different-inlet-extrusion-lengths.html)

Janshi October 25, 2011 03:19

Divergence / Convergence for different inlet extrusion lengths
 
3 Attachment(s)
Hello,

Currently I analyse the pressure drop in a very simple pipe system consists of a pipe, a wind box, an outlet and an inlet extrusion.
The dimensions of the pipe, the wind box and the outlet extrusion are fix.
The length of the inlet extrusion will be varied.
Its a steady state calculation with air as an ideal gas. Turbulence model is the k-epsilon model, temperature of the air is 20 °C.

For the extrusion length 0-50 mm everything is fine, the computation reaches convergence after about 10000 iterations.
In the attachment there is a screenshot of the pressure for the length 50mm.

When I rise the length over 50mm, e.g. 60mm, things become weird after about 4000 iterations. The engineering variables are going to oscillate, the residuals are blowing up and then oscillates too.
In the attachment there are two screenshots of the pressure and the residuals.

So, does anybody have an idee what the reason for this very different behaviour could be and why the computation canīt reach convergence for a length higher than 50mm?

Thank you

hamzamotiwala October 25, 2011 09:08

Hey,

Dont you think 10000 iterations is a bit too much for such a simple problem? what is your inlet diameter?

what are your boundary conditions?

What mesh are you using? How many cells?

Janshi October 25, 2011 09:20

Hi,

Thank you for your reply. Iīm not an experienced CFD-User so currently its quite difficult for me to judge if I use efficient settings for a fast and decent convergence.

Inlet diameter (hydraulic diameter): 147.76 mm
Mesh: polyhedral mesh, base size 2mm and about 925000 cells
Turbulence model: k-epsilon

Boundary Conditions:
Inlet: Massflow Inlet, 0.27778 kg/h, turbulent dissipation rate and energy default (0.1 J/kgs and 0.0010 J/kg)

Outlet: Pressure outlet, pressure -5000 Pa, turbulent dissipation rate and energy default


Bye Janshi

hamzamotiwala October 25, 2011 09:30

Quote:

Originally Posted by Janshi (Post 329369)
Hi,

Thank you for your reply. Iīm not an experienced CFD-User so currently its quite difficult for me to judge if I use efficient settings for a fast and decent convergence.

Inlet diameter (hydraulic diameter): 147.76 mm
Mesh: polyhedral mesh, base size 2mm and about 925000 cells
Turbulence model: k-epsilon

Boundary Conditions:
Inlet: Massflow Inlet, 0.27778 kg/h, turbulent dissipation rate and energy default (0.1 J/kgs and 0.0010 J/kg)

Outlet: Pressure outlet, pressure -5000 Pa, turbulent dissipation rate and energy default


Bye Janshi


man!! your mesh is too fine. Generally your base size should be the size of your smallest inlet diameter.

and you have almost 1 million cells for this simple example...

firstly, change your base size to 147 mm.
if you are not comfortable using relative values then use absolute values for your mesh at the begining..

for your case an element lenght of 3-4mm should be good...

fix your mesh and i think you should not have any further problems..

Janshi October 25, 2011 09:32

Thank you, I give it a try!

Greets Janshi

abdul099 October 25, 2011 19:27

hamzamotiwala,

the base size is a nearly meaningless number. Important is not the value of the base size, important are the mesh values resulting from base size and relative sizes.
Further to that, 1 million cells is not much, depending on the geometry. Sure, he might make his mesh coarser, depending on his geometry. But that will not solve his "problem".

To the solution itself: The oscillations in engineering values and residuals suggest, it could be a transient problem. There might be vortices causing an unsteady behaviour of the flow, so the solver can't establish a stable steady state solution.
Such a behaviour can be spotted very often. Usually one would average the values over some hundred iterations, that's should be fine.
The reason why it starts only when the extrusion is larger than 50mm could be quite difficult to find. As it is an extrusion, I would exclude bad cells near the inlet. But depending on your extrusion walls (slip or no slip), the flow changes in different ways when passing the extrusion. A longer extrusion means different state of the flow when arriving at your main region and therefore a different behaviour.
For me that's only an indicator that the extrusion is too short. 50mm extrusion at a 147mm diameter inlet is nothing. Just consider, a pipe flow needs a distance of about 6 - 8 times the hydraulic diameter until a fully developed pipe flow is established.

Further I hope, you got some reliable values for turbulent kinetic energy and dissipation rate. This values can have a quite nice impact on the solution, especially when setting values which don't fit together. If you don't have any reliable values, you should consider to specify turbulence values on a different method.

hamzamotiwala October 26, 2011 05:21

Quote:

Originally Posted by abdul099 (Post 329439)
hamzamotiwala,

the base size is a nearly meaningless number. Important is not the value of the base size, important are the mesh values resulting from base size and relative sizes.
Further to that, 1 million cells is not much, depending on the geometry. Sure, he might make his mesh coarser, depending on his geometry. But that will not solve his "problem".


Hey! thanks for the clarification..I completely misunderstood the problem. I overlooked the sytem part and I thought that it was just a 50mm pipe where janshi was trying to simulate a flow. Thats the reason I thought a million cells in a cylinder of 50mm lenght was too much...and the base is obviously meaningless until you check on the percentage you are alloting to the elements..thats the reason i asked janshi to use absolute values...

abdul099 October 26, 2011 19:55

Yeah, you're right. If it would have been a pipe with 50mm length, a million would be way too much cells.
I also agree, it usually makes sense to set the base size to a characteristic size of the system one wants to simulate, like the hydraulic diameter. But with the default percentages, this would result in a too coarse mesh, therefore I'm using it only for the first shot and reduce either percentages or base size (or both). That's no issue as long as one doesn't forget to set smaller values when needed, but I've already seen anything happen. Including people setting the base size to a big value and wonder why the mesh is just crap. And additionally this guys have been afraid of setting the percentages to appropriate values, because the numbers would have been "too small".

cfdivan October 27, 2011 10:32

Hi,

Janshi

Cell numbers doesnīt matter solely! Important is to fit your mesh to your physical phenomenon in your domain. We can have an millions of cells within your domain and your solution doesn't converge due to the bad mesh distribution. Think about physical phenomenon and after that make considerations about yours mesh requirements.

Outlet pressure: -5000Pa...was measured?Do you measure the velocity in outlet section or other thermodynamics constants?

Instability could be the explanation of unsteady phenomenon...

Do you have some pictures of your geometry? This could help to explain the results...

You can make use of powerfull post processing tools of star to help debug the solution.

When residuals are your concern, donīt forget the meaning of this parameters...2-3 order of magnitue could be enougth to reach a true solution(:rolleyes:)...there are lots of others parameters in cfd simulations that are more important then maginute orders of residuals to evaluate your simulation.

Regards,
IA


All times are GMT -4. The time now is 09:06.