Discussion Groups

Simulation Mechanical and Multiphysics

Reply
Distinguished Contributor
jrm_1971
Posts: 112
Registered: ‎03-31-2011

!!!!Simulation Pro 2011 - Stagnation due to oscillations!!!!

829 Views, 23 Replies
06-26-2012 02:46 PM

See thread here. Spencer and Forrest Judd's post is of interest

 

http://forums.autodesk.com/t5/Autodesk-Simulation-Mechanical/Simulation-Pro-2011-Stagnation-due-to-o...

 

#AstroJohn, #Joey.X, any ideas? I've been through letting SIM Pro 2011 automatically place the refinement points. Engineer intuition just screams that the stagnation due oscillations (SDO) is causing the problems with flow, and ultimately, the the coupled heat transfer.

 

I was getting anywhere from 1-6 (SDO) warnings with steady state

 

With unsteady I get 8 (SDO) warnings with 10 load steps.

 

It is a curved conduit (3/8") with turbulent flow. Tet mesh (95%). Maybe SIM Pro just does not like fluid flow in bends?

Please use plain text.
Distinguished Contributor
jrm_1971
Posts: 112
Registered: ‎03-31-2011

Re: !!!!Simulation Pro 2011 - Stagnation due to oscillations!!!! SOS SOS SOS

06-28-2012 07:12 AM in reply to: jrm_1971

SOS Astro and Joey.X. Been looking at this way too long. There should be some fundamental steps to elliminate Stagnation due to oscillations I am just so sure that is corrupting my coupled analysis. The heat just creaps along. No other problems. It's not sonic. 3/8" tube really has a 0.406" ID. I've tried mesh refinement, various meshes. It just won't go away.

 

Theoretical Parameters

V=110 ft/s

 

visc (lbf   s/ft2)
2.84084E-07

 

density   (lb/ft3)

0.22274994

 

Re
       2,923,631

Ma

0.186



Please use plain text.
Distinguished Contributor
jrm_1971
Posts: 112
Registered: ‎03-31-2011

Re: !!!!Simulation Pro 2011 - Stagnation due to oscillations!!!! SOS SOS SOS?

07-01-2012 02:00 PM in reply to: jrm_1971

Hello anybody????

Please use plain text.
Employee
INACTIVE_AstroJohn
Posts: 492
Registered: ‎03-25-2010

Re: !!!!Simulation Pro 2011 - Stagnation due to oscillations!!!! SOS SOS SOS

07-05-2012 08:26 AM in reply to: jrm_1971

Hi jrm,

 

Apologies for being "missing in action". I had a problem with the automatic subscription, so I was not getting email notifications about anyone's post for the last 3 weeks or so. It seems to be fixed now since I just received the first email that someone has posted!

 

I may not understand what you mean by "the heat just creeps along".

  • Do you mean that you applied a temperature to the inlet and expect to see it propogate through the system?
  • Do you have a controlled temperature (I think 2011 called it "applied temperature") at the inlet, or did you use initial temperature (which would be wrong)?

It is hard to "slice" your model to see the internal velocities, but you can use either streamlines or particle paths to check whether the velocity is "continuous" along the entire length. (Streamline is probably better, but particle parths are more fun.) See this page in the documentation if you need help with those commands.

 

Another trick you could use to see what is happening in the cross-section of the tube would be to split the tube into a two part assembly. One part would be the "outside" half of the tube, and the other part would be the inside half. Hiding one of the parts in the Results environment would be just like slicing the model along the centerline with a knife (instead of a plane).

 

Also, I do not remember if you are performing a "Multiphysics > Coupled" analysis type, or a fluid flow analysis in one design scenario and a thermal analysis in another design scenario where you read in the velocity results. If you have not tried both types, performing the other one do something different. Based on your velocities, the two-way coupling that the "Multiphysics > Coupled" gives is probably not important. That is, the buoyancy effects of the fluid do not greatly affect the velocity profile. See Fluid Convection in the documentation if you are not familiar with the second method.

 

Not that it matters, but what is your fluid? Some type of gas is my guess based on the density.

Sincerely,
John Holtz, P.E.
Senior User Experience Designer, Simulation
Autodesk, Inc.

Current version of Mechanical & Multiphysics: 2013 SP1 (2013.01.00.0012 28-Jun-2012)
Please use plain text.
Distinguished Contributor
jrm_1971
Posts: 112
Registered: ‎03-31-2011

Re: !!!!Simulation Pro 2011 - Stagnation due to oscillations!!!! SOS SOS SOS

07-08-2012 10:10 AM in reply to: INACTIVE_AstroJohn

Hi Astro please see my responses below.

 

I may not understand what you mean by "the heat just creeps along".

  • Do you mean that you applied a temperature to the inlet and expect to see it propogate through the system? The temperature does propogate but the virtual time it takes seems unrealistic. The applied temperature is set at the inlet surface, at 375 F, default nodal temperature at 100 F. The time results in the post-processor are 600 seconds for the temperature to fully propogate. That just seems way too long. Forrest Judd in an earlier thread expressed refinement points to eliminate "stagnation due to oscillations", but I've refined the model to death with several mesh configurations. It just won't go away, and is obviously occuring in the continuous bend. If there was a way to eliminate the "stagnation due to oscillations", this may just free up the flow. (I do recall now from reviewing the streamlines again, they significantly disipate on the discharge). Again, I believe this is due to the  "stagnation due to oscillations"
  • Do you have a controlled temperature (I think 2011 called it "applied temperature") at the inlet, or did you use initial temperature (which would be wrong)? Applied

It is hard to "slice" your model to see the internal velocities, but you can use either streamlines or particle paths to check whether the velocity is "continuous" along the entire length. (Streamline is probably better, but particle parths are more fun.) See this page in the documentation if you need help with those commands.

 

Another trick you could use to see what is happening in the cross-section of the tube would be to split the tube into a two part assembly. One part would be the "outside" half of the tube, and the other part would be the inside half. Hiding one of the parts in the Results environment would be just like slicing the model along the centerline with a knife (instead of a plane). Let me try this but possibly there's a solution for the "stagnation" in the meantime?

 

Also, I do not remember if you are performing a "Multiphysics > Coupled" analysis type, or a fluid flow analysis in one design scenario and a thermal analysis in another design scenario where you read in the velocity results. If you have not tried both types, performing the other one do something different. Based on your velocities, the two-way coupling that the "Multiphysics > Coupled" gives is probably not important. That is, the buoyancy effects of the fluid do not greatly affect the velocity profile. See Fluid Convection in the documentation if you are not familiar with the second method. I've tried both with the same results.

 

Not that it matters, but what is your fluid? Some type of gas is my guess based on the density. Yes, a methane/ethane compound gas.

Please use plain text.
Employee
INACTIVE_AstroJohn
Posts: 492
Registered: ‎03-25-2010

Re: !!!!Simulation Pro 2011 - Stagnation due to oscillations!!!! SOS SOS SOS

07-09-2012 11:16 AM in reply to: jrm_1971

Hi JRM,

 

Something just occurred to me based on your reply. Is the fluid analysis for a short duration (like 1 second) with many timesteps (like 20 or 50 or 100)? The reason I ask is because fluid phenomena usually happen on a very small timescale. If your timestep is large, that may be affecting the results.

 

I created a simple hand-built model using the information that was in the thread. I did not have all of the dimension and cannot spend the time to make it spiral inward, but it should be close.

 

Another advantage of splitting the tube in half is that it provides a "surface" mesh inside the volume, so you have a better control over the element size. Otherwise, you really have very little control over the size of the solid elements, so the solid mesh may have a few larger elements spanning the inside volume which may be affecting the results.

 

The only other suggestion that comes to mind is to increase the convergence tolerance so that each timestep "converges" before it gets to the point where it has stagnation issues. The page "Perform Fluid Flow Analyses" in the Help explains the fluid flow log file.

 

If my model is reasonable, it looks like it takes about 0.15 seconds to help up the entire volume of fluid when the fluid is running at 110 ft/sec.

 

See the attached images.

 

Sincerely,
John Holtz, P.E.
Senior User Experience Designer, Simulation
Autodesk, Inc.

Current version of Mechanical & Multiphysics: 2013 SP1 (2013.01.00.0012 28-Jun-2012)
Please use plain text.
Valued Contributor
tfjield
Posts: 98
Registered: ‎06-19-2012

Re: !!!!Simulation Pro 2011 - Stagnation due to oscillations!!!! SOS SOS SOS

07-09-2012 03:17 PM in reply to: INACTIVE_AstroJohn

Hi guys,

 

I was getting a Stagnation Due to Oscillation warning in my steady state model as well.  (Multiphysics 2013)  I refined and refined with no luck.  At first I thought I must have some oscillation or flapping, but that doesn't seem to be the case at my geometry/velocities.

 

What I did was go into Analysis Parameters -> Solution -> Formulation Automatic (>>) and under Relaxation Control changed the setting for Detect Stagnation Due to Oscillation from "Continue to Next Step" to "Perform Maximum Iterations."

 

Now I no longer get any warnings, and while it is performing more iterations, it is not just hitting the maximum every time.  It appears, based on the residuals, that I'm getting a good convergence.  As a secondary test, my results are within a couple percent of an independent analysis of the same geometry using another CFD package.

 

Is it possible that it's just too sensitive with it's stagnation detection and it's giving up too early?

Current version of Mechanical & Multiphysics: 2013 SP2 (2013.02.00.0010 2-Oct-2012)
Please use plain text.
Employee
Joey.X
Posts: 259
Registered: ‎06-14-2010

Re: !!!!Simulation Pro 2011 - Stagnation due to oscillations!!!! SOS SOS SOS

07-10-2012 08:12 AM in reply to: tfjield

 hi, tfjield

Your observation is under design,  there are no single solution handling all cases in CFD. Stagnation detection depends on model behaviors.

In some cases, if user changes to "Perform Maximum Iterations", the solution will iterate forever without reaching specified convergence criteria or iterate to maximal iteration numbers.

Here are user's options to compromise the solution accuracy, solution iteration numbers, convergence. The current default values are used for majority cases.

- Switch between "Continue to Next Step" to "Perform Maximum Iterations." for "detec stagnation due to oscillation",  that's turns on/off stagnation detection.

- Adjust convergence criteria from setup/parameter/load curve tab/custom load-stepping settings/velocity norm and pressure norm

- Adjust relaxation control from setup/parameter/solution tab/formulation >>/segregated options/Relaxation control/velocity, pressure, inertial relaxation factor.



 

Jianhui Xie, Ph.D
Principal Engineer
MFG-Digital Simulation
Please use plain text.
Valued Contributor
tfjield
Posts: 98
Registered: ‎06-19-2012

Re: !!!!Simulation Pro 2011 - Stagnation due to oscillations!!!! SOS SOS SOS

07-10-2012 09:18 AM in reply to: Joey.X

Hi Joey.X,

 

Thanks for the reply and the great summary.  I had read many of the other threads regarding this issue, and I expected my problem to be similar, perhaps with flapping or turbulence, or perhaps the unrefined mesh...

 

To an experienced Simulation user, I expect one of the first things to try would be to turn oscillation detection off and see what happens, but I hadn't noticed that in any of the threads.  I was fortunate that's all it took in my case.  In fact, the number of iterations and solver time didn't increase much when I turned checking off.

 

Anyway, thanks again!

Current version of Mechanical & Multiphysics: 2013 SP2 (2013.02.00.0010 2-Oct-2012)
Please use plain text.
Distinguished Contributor
jrm_1971
Posts: 112
Registered: ‎03-31-2011

Re: !!!!Simulation Pro 2011 - Stagnation due to oscillations!!!! SOS SOS SOS

07-17-2012 09:37 AM in reply to: INACTIVE_AstroJohn

Dear Astro,

 

I got rid of the Stagnation due to oscillations but now I've been chasing the volumetric flow rate. Should be getting about 0.099 ft^3/s. I have used a refined mesh with mesh size down to 25%. I've gotten the flow rate to 0.07.... ft^3/s, which is quite a big error. Tet mesh, smoothing options off, Sum (inquire results on outlet). I've tried pseudo time of 1 second with anywhere from 10-50 steps, velocity norm=0.003, pressure norm=0.003, perform max iterations on, etc.

 

Did you check your volumetric flow rate? What mesh did you use? I've tried different ones.

Please use plain text.