
[Sponsors] 
April 10, 2017, 11:46 
3D DES simulation of turbulent jet

#1 
New Member
Join Date: May 2015
Posts: 22
Rep Power: 11 
Hello all,
Im a beginner in Fluent and CFD so please bear with me. Im trying to run a DES simulation for a 3d turbulent jet. I want to visualize the velocities (x,y,z), vorticities (x,y,z) etc. I am trying to simulate a duct (0.35mx0.35mx0.25m). The duct is seperated by a wall which has a sharpedged rectangular orifice configuration(70 mm x 7 mm). My inlet is 0.1 m before the wall that has the orifice and my outlet 0.15m after the wall. My mesh consists of tetrahedrons everywhere exccept where i used inflation. There are 1.6 million elements total. Given data was ony the Reynolds number at the orifice (Re=23000 or Re hydrolic diamaterer=42000). It is calculated that the velocity at the orifice is v2=50m/s and so the velocity at the inlet has to be v1=0.133m/s. Also the simulation is done as incompressible. In Fluent my inputs are: Pressurebased solver Transient Energy off Delayed Detached Eddy Simulation (DES) with the SpalartAllmaras model Boundary Conditions: for walls i used default options for outlet i used default options for interior i used default options for inlet i used massflow inlet mass flow rate = 0.19958 kg/s z component of flow direction = 0.133m/s turbulence specification method = turbulent viscosity ratio turbulence viscosity ratio=10 SIMPLE scheme was selected. Gradient: Least square cell based Pressure: Second Order Momentum: Second Order Upwind Modified Turbulent viscosity: Second Order Upwind Transient Formulation: Bounded Second Order Implicit UnderRelaxation factors were left default except for: pressure: from 0.3 (default) > 0.4 momentum: from 0.7(default) > 0.8 All Residuals were changed to 1e05 Using Standard Initialization, the solution was initialized as zeros (0) everywhere For time step i choose Dt=5e04 and max iterations/time step= 10 I use solution animations to check the results while running the simulation and the results are very close to what was expected...but the residuals are not willing to go down and converge Do you have any changes to propose for all the above settings ? Did i make a mistake somewhere ? Sorry for the long thread. Any help will be greatly appreciated Thank you. Kostas 

April 11, 2017, 01:43 

#2 
Senior Member
Lucky
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 5,703
Rep Power: 66 
Do you mean residuals are stuck at high values or are they decreasing but not enough to meet your convergence criteria? If it's the 1st, then it hints at a problem with the setup. If it's the 2nd...
I think it is because you are using SIMPLE which needs many iterations to converge (because the urf's are not 1). You can verify this by increasing the number iterations per timestep to a really high number like 50 or 100 (just to check). Just do it for a few timesteps to test. You can change it back later. Also have you tried a smaller timestep? Since you don't have coupling with any other equations, I highly recommend PISO. The disadvantage is you'll need small timesteps. The advantage is, you can get away with as few as 2 iteration per timestep. You should be able to take a bunch of smaller timesteps faster. SIMPLE is great when you are also solving a lot of other equations, because coupling between equations is what slows convergence. If you're only solving continutiy & momentum, it's probaby the PV coupling that's limiting. You could also give the COUPLED solver a whack, but it has urf's and so it's behaves more like SIMPLE. But definitely do the check using SIMPLE with 100 iterations to make sure. Btw I highly recommend you always use the bounded central differencing whenever possible (momentum especially). But maybe it's not available for DES. 

April 11, 2017, 01:48 

#3 
Super Moderator
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 3,297
Rep Power: 41 
If you are a beginner, I would:
*run a steady state case first *set all underrelaxation parameters to default settings *set all numerical schema to default *set turbulent model to default (keps?) I would modify some parameters if you get bad results or poor convergence What is for you the default BC for outlet? I would also extend your domain , inlet and outlet are to close to the restriction
__________________
In memory of my friend Hervé: CFD engineer & freerider 

April 11, 2017, 07:41 

#4 
New Member
Join Date: May 2015
Posts: 22
Rep Power: 11 
Hello LuckyTran,
Thank you for your answer When the simulation begins the residuals decrease. After a few hundreds iterations they stop decreasing or they decrease with a very slow rate. The residuals of x,y,z velocities and nut oscilate between 1e04 and 1e06. Only continuity stays between 1e02 and 1e03. For my mesh i used body of influence to create the fine areas. I put 2mm for the element sizes as an input so i calculated the timestep like this: Dx/v=Dt => 0.002/50=0.00004=4e05. But I also tried to run a simulation with 2e05 which is half of the above. But i couldn't get a good result. Maybe because the solution advances very slow and I didn't let it run for more than a coyple days. I will try what you said about simple and piso scheme and let you know. 

April 11, 2017, 08:13 

#5 
New Member
Join Date: May 2015
Posts: 22
Rep Power: 11 
Hello Max,
Thank you for your answer *I have already tried running a steady state simulation. And then when the residuals were flat (not converged) i changed the solution to transient and used the steady state values an initials. *Also i had the urf's at their default values. Only in the last case that i posted about had i changed them. * The schemes were also default *I can not use the ke model because i want to visualize vorticity and the ke doesn't show it. Only with LES or DES could i see the vorticity. And the LES is more demanding than the DES Also i used to have a bigger domain but it reached about 45 million elements and my computer wasn't able to solve it. So i was forced to make it smaller. The default BC for the outlet is type  Pressure outlet at momentum tab gauge pressure (pascal)  0 constant backflow direction specification method  normal to boundary turbulence specifiction method  turbulent viscosity ratio backflow turbulent viscosity ratio  10 constant 

April 11, 2017, 10:25 

#6  
Senior Member
Lucky
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 5,703
Rep Power: 66 
Quote:
Quote:
Honestly I think your simulation is fine and you only need to do some sanity checks. Make some point monitors at interesting points (like where you expect the shear layer) and check that the xvelocity, yvelocity, zvelocity, & pressure are converged to #.### decimals at every time step. You can also probe the vorticity since that's what you're interested in. Rather than worry about how much residuals are dropping, you should start postprocessing and check whether the result makes any sense. I.e. verify that you have the expected turbulence. 

April 13, 2017, 13:33 

#7 
New Member
Join Date: May 2015
Posts: 22
Rep Power: 11 
No my courant number is not 1. It would be if i hab used for a time step 4e05 but i used 5e04. Because it would take too much time otherwise.
Also i just started testing what you said for PISO because for 2 days now i have been running another simulation. I started with DES model and steady solution to get a initial value for my case (i know that DES model is only meant for transient solution). After 1600 iterations when the residuals were flat (not converged) i changed the solution to transient and used the steady state values an initials. The results in comparison with the experiment for z velocity and z vorticity can be seen in the pictures. The only problem are the residuals. Can i say that my solution is converged ? 

April 13, 2017, 14:08 

#8 
Senior Member
Lucky
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 5,703
Rep Power: 66 
If you want to know if your solution is converged, then look at the solution, not residuals! Look at velocities, etc. Make a plot of velocity vs iter.
Also you need to verify that your DES is actually DES. I am worried that because you did not apply any perturbations (i.e using initinstantaneousvelocity or something equivalent) that you do not have a turbulent flow. Check the spectrum and verify that it is indeed turbulent and not laminar. It is not wrong to do so, but I hope you are aware of the implications of using a very large timestep in DES/LES. Your temporal bandwidth is now extremely limited. 

April 14, 2017, 07:34 

#9  
New Member
Join Date: May 2015
Posts: 22
Rep Power: 11 
Quote:
Also if i do have a laminar flow how can i apply some pertrubations using ansys in order to make it turbulent and get the right solution ? 

April 14, 2017, 09:19 

#10  
Senior Member
Lucky
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 5,703
Rep Power: 66 
Quote:
https://www.cfdonline.com/Forums/blogs/sbaffini/ How to check... Well how do you verify that any flow is turbulent? I.e. forget that you are doing CFD but you are just an observer or experimentalist. If I set up this problem in a lab, how do you verify that it is indeed turbulent? Well one way is to get the spectrum of the the turbulent kinetic energy and show that it is broadband and looks like a typical turbulent spectrum. 

Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Water jet simulation  harry123  STARCCM+  10  November 28, 2020 18:51 
Jet fan and Tunnel simulation  ahlo7  CFX  9  November 13, 2019 04:54 
LES of Turbulent Jet  knuckles  OpenFOAM Running, Solving & CFD  1  March 31, 2016 19:33 
Impinging Jet simulation with rhoSimpleFoam  dappe  OpenFOAM Running, Solving & CFD  7  December 1, 2015 03:42 
Unsteady RANS simulation of Jet in crossflow  harshad88  FLUENT  0  June 2, 2013 13:29 