Simulation Mechanical Forums (Read-Only)
Welcome to Autodesk’s Simulation Mechanical Forums. Share your knowledge, ask questions, and explore popular Simulation Mechanical topics.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

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

23 REPLIES 23
Reply
Message 1 of 24
jrm_1971
1919 Views, 23 Replies

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

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?

23 REPLIES 23
Message 2 of 24
jrm_1971
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

Message 3 of 24
jrm_1971
in reply to: jrm_1971

Hello anybody????

Message 4 of 24
John_Holtz
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.



John Holtz, P.E.

Global Product Support
Autodesk, Inc.


If not provided already, be sure to indicate the version of Inventor Nastran you are using!

"The knowledge you seek is at knowledge.autodesk.com" - Confucius 😉
Message 5 of 24
jrm_1971
in reply to: John_Holtz

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.

Message 6 of 24
John_Holtz
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.

 



John Holtz, P.E.

Global Product Support
Autodesk, Inc.


If not provided already, be sure to indicate the version of Inventor Nastran you are using!

"The knowledge you seek is at knowledge.autodesk.com" - Confucius 😉
Message 7 of 24
tfjield
in reply to: John_Holtz

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?

Using Autodesk CFD and Fusion 360
Message 8 of 24
Joey.X
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
Message 9 of 24
tfjield
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!

Using Autodesk CFD and Fusion 360
Message 10 of 24
jrm_1971
in reply to: John_Holtz

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.

Message 11 of 24
John_Holtz
in reply to: jrm_1971

JRM,

 

The first question is whether you have the same calculated flow rate going in as flow going out.

 

If they are the same, then my guess is that the difference between the calculated and the expected is due to the mesh size and the expectation. 0.099 ft^3/sec is assuming the flow is constant over the entire area which means a velocity of 110 ft/sec at the wall of the tube. In the simulation, the velocity is 0 at the wall, so all of the elements around the wall have about 55 ft/sec going through them which reduces the total flow.

 

If the flow rate in does not equal the flow rate out, the problem is related to the convergence. If you have an Inlet/Outlet condition applied to the model, try replacing it with a very small pressure (like 1E-6 psf) and run the analysis. After it converges on the first step, you can inquire the flow rate results and compare the inlet and outlet.

 

 

 



John Holtz, P.E.

Global Product Support
Autodesk, Inc.


If not provided already, be sure to indicate the version of Inventor Nastran you are using!

"The knowledge you seek is at knowledge.autodesk.com" - Confucius 😉
Message 12 of 24
jrm_1971
in reply to: John_Holtz

JRM,

 

The first question is whether you have the same calculated flow rate going in as flow going out.

 

If they are the same, then my guess is that the difference between the calculated and the expected is due to the mesh size and the expectation. 0.099 ft^3/sec is assuming the flow is constant over the entire area which means a velocity of 110 ft/sec at the wall of the tube. In the simulation, the velocity is 0 at the wall, so all of the elements around the wall have about 55 ft/sec going through them which reduces the total flow. Astro, the inlet/outlet VFR are almost the same within 0.1% (0.070/0.0699). Even using Results->Sum I get 0.0699 ft^3/s on the outlet,6 with smoothing off, and 25% tet mesh. 29% error is a lot, noting that it will probably never be exact to 0.099 ft^3/s since that is an estimate of Q=VA. Shouldn't I expect an error closer to 1%-5% with "Sum"?

 

If the flow rate in does not equal the flow rate out, the problem is related to the convergence. If you have an Inlet/Outlet condition applied to the model, try replacing it with a very small pressure (like 1E-6 psf) and run the analysis. After it converges on the first step, you can inquire the flow rate results and compare the inlet and outlet.

Message 13 of 24
tfjield
in reply to: jrm_1971

Hey JRM,

 

I hope you don't mind me jumping in here with my 2 cents, but I think the issue that you're having regarding your flow is a result of your boundary conditions.

 

I believe the discrepancy is because you believe you're applying a 110 ft/sec velocity boundary condition over the entire inlet face of your tube.  Because you're in a no-slip condition with the wall, the nodes actually on the wall of the tube must be 0 ft/sec.  The average velocity, then, of the gas flowing through ALL cells touching the wall is only 55 ft/sec.  Depending on your mesh size, the area of all the cells along the circumference can be quite large, percentage wise, and when you integrate and average the velocity over the entire face it is less than 110 ft/sec.

 

Based on your results, SIM is reporting 0.070 ft^3/sec at the inlet, not the 0.099 that that you expect based on Q=VA, because the number you're plugging in for V is wrong:  it's not 110 ft/sec averaged over the entire face, it's lower because of the wall contact.

 

In the images of flow velocity that John produced earlier, from his example model, you can see that the cross sectional velocity profile took some distance from the inlet to stabilize, and the velocity at the outlet in the center was quite a bit higher than the 110 ft/sec.

 

What i've done in similar situations is to add an inlet region to my model, usually hemispherical, much larger than the diameter of the tubing, with a large surface that I can apply my bondary condition to.  This geometry gives it a change to enter the tube with a cross-sectional profile comparable to the exit profile.

 

I hope that helps!

Using Autodesk CFD and Fusion 360
Message 14 of 24
jrm_1971
in reply to: jrm_1971

Astro,

 

1. On the heat transfer part of your coupled analysis, was the applied temperature applied to both inlet faces of each half or just one face of a half? When I apply applied temperature to each inlet face half, the analysis does not finish. When I apply to only one inlet face (one of the halves), the analysis finishes.

 

2. Please see the attached. How did you get this graph? Also, is it implying that only near the inlet does the group of plots reach 375F after 0.08 seconds and the full volume/outlet never approaches 375 F?

Message 15 of 24
John_Holtz
in reply to: jrm_1971

Hi,

 

1. I applied the temperature to both halves of the inlet.

 

In my sample, I used the "one-way coupling" (or uncoupled analyses) method by running an unsteady fluid flow analysis in design scenario 1, then I ran a transient heat transfer analysis in design scenario 2 and imported the fluid velocities from design scenario 1.

 

Is this the methodology that you are using? Or are you running a "Multiphysics > Transient Coupled Fluid Flow and Thermal" analysis type? See Help > Analysis Types > Multiphysics.

 

I did not see that you indicated what happened to cause the analysis to not finish. Transient heat transfer should not be performing iterations in this case, so there is no problem with convergence. It should run to completion or cause a crash. A crash is something that we can deal with.

 

2. The graph is showing 11 nodes along the length of the coil. I created the graph by selecting nodes, right-click > Create Graph. Naturally, this was done from my transient heat transfer design scenario while displaying the temperature results. The attached revised plot will make it clearer as to what is being plotted. After 0.08 seconds, a point just downstream of the inlet heats up from 100 F to 375 F. After 0.14 to 0.16 seconds, the entire length has heated to 375 F (and the entire cross-section, too.)

 



John Holtz, P.E.

Global Product Support
Autodesk, Inc.


If not provided already, be sure to indicate the version of Inventor Nastran you are using!

"The knowledge you seek is at knowledge.autodesk.com" - Confucius 😉
Message 16 of 24
jrm_1971
in reply to: John_Holtz

1. I applied the temperature to both halves of the inlet.

 

In my sample, I used the "one-way coupling" (or uncoupled analyses) method by running an unsteady fluid flow analysis in design scenario 1, then I ran a transient heat transfer analysis in design scenario 2 and imported the fluid velocities from design scenario 1.

 

Is this the methodology that you are using? Or are you running a "Multiphysics > Transient Coupled Fluid Flow and Thermal" analysis type? See Help > Analysis Types > Multiphysics.

 

I did not see that you indicated what happened to cause the analysis to not finish. Transient heat transfer should not be performing iterations in this case, so there is no problem with convergence. It should run to completion or cause a crash. A crash is something that we can deal with. I did on-way coupled. I had time steps but after this, set the time step to "1". That worked.

 

2. The graph is showing 11 nodes along the length of the coil. I created the graph by selecting nodes, right-click > Create Graph. Naturally, this was done from my transient heat transfer design scenario while displaying the temperature results. The attached revised plot will make it clearer as to what is being plotted. After 0.08 seconds, a point just downstream of the inlet heats up from 100 F to 375 F. After 0.14 to 0.16 seconds, the entire length has heated to 375 F (and the entire cross-section, too.) How did you get the curvature of your graph? Mine looks linear. I selected 11 nodes on the outside wall like it looks in yours.

 

3. New: To get the true Heat Flux and Heat Rate of Face  is that done with smoothing options off or on? Also, is that done with Range, Mean, or Sum? I don't remember if that was specific to the fluid flow or if it applies to the heat transfer analysis too?

Message 17 of 24
jrm_1971
in reply to: jrm_1971

OK Astro,

 

Could it be possible I am getting a linear graph because the coordinate system needs to be set to a local point on the coil since this is a time base analysis? See TIP here http://wikihelp.autodesk.com/Simulation_Mechanical/enu/2013/Help/0031-Autodesk31/0533-Results533/053...

 

The coordinate system is set to local in the post-processor, but possibly a New local needs to be created?

 

I think I found my answer here regarding Smoothing Heat Transfer results. http://wikihelp.autodesk.com/Simulation_Mechanical/enu/2013/Help/0031-Autodesk31/0533-Results533/053...

 

I'll be looking later for exactly how to get the correct Btu/ft^2 s but if you want to provide that, that would be great! Smiley Happy

 

Message 18 of 24
John_Holtz
in reply to: jrm_1971

Hello,

 

2. =====

I did not do anything to create the curvature in the temperature plot; the software did it for me. Smiley Wink Keep in mind that my analysis is only an example since the complete input or model has not been provided (unless I overlooked it somewhere in the thread). My material properties for the thermal analysis may be affecting the shape of the curve. For reference, I used

  • mass density = 0.223 lbm/ft^3   [3.57 kg/m^3]
  • thermal conductivity = 5.1E-6 BTU/(ft*s*F)   [0.032 W/(m*C)]
  • specific heat = 0.54 BTU/(lbm F)   [2240 J/(kg*C)]

One way to share the input that may be acceptable in situations where their is proprietary information (usually in the model itself) that cannot be shared is to

  • create a report  (of the fluid flow and thermal analyses in this case)
  • save them to HTML (from the Report tab, "Save As > HTML")
  • zip the file and folder that are created
  • post the zip file to the forum

Before doing all of that, you can use the "Report > Setup > Configure" to hide parts of the report that cannot be shared or to add additional information. Naturally, this "input only" information will only be helpful in situations where the model can be described verbally (or shown in images) and a similar model recreated by the reader. Obviously, an archive of the model ("File > Archive > Create") is always more helpful.

 

If it is of any use, I can archive my example and post it. But it can only be opened with version 2013, and having a model that "works" doesn't always guarantee that  the problem in a model that doesn't work can be found.

2. =====

 

3. =====

The "Heat Flux" results are calculated at a point in space (at the center of the element). So there should not be a large difference between using "Results Contours > Settings > Smooth Results" and having "Smooth Results" turned off. The result is as follows:

  • With "Smooth Results" off, each element is colored with the result.
  • With "Smooth Results" on, the value in an element is used at all of its nodes. Then the value from all of the elements at a node are smoothed according to "Results Contours > Settings > Smoothing Options".

When "Smooth Results" is on, you normally want the "Results Contours > Settings > Smoothing Options > Smoothing function" set to "Mean". This averages the results between adjacent elements and tends to "smooth" the discrepancies that occur in finite element analysis. "Range" can be used to show large changes between adjacent elements which may indicate the mesh is too coarse. I cannot think of a case where "Sum" has any physical meaning.

 

The "Heat Rate Through Face" (or "Flow Rate Through Face" in fluid flow analysis) are calculated at each face of each element. That is, it integrates the heat flux (or velocity in fluid flow) over the area of the element. Therefore, it does not make sense physically to distribute the flow through a face to each of nodes at the corners, and then smooth them with adjacent faces. Therefore, "Results Contours > Settings > Smooth Results" must be off when viewing these results. If you then select the faces and "Results Inquire > Inquire > Current Results", you can use any of the functions in the "Summary" to as desired.

3. =====

 

I better do some more work while the creative juices are flowing!

 

 

 



John Holtz, P.E.

Global Product Support
Autodesk, Inc.


If not provided already, be sure to indicate the version of Inventor Nastran you are using!

"The knowledge you seek is at knowledge.autodesk.com" - Confucius 😉
Message 19 of 24
jrm_1971
in reply to: John_Holtz

Thanks Astro.

 

What kind of values are you getting on your heat flux and heat rate?

Message 20 of 24
jrm_1971
in reply to: jrm_1971

Astro,

 

1. The pictures on the left show just the fluid without the tubing in the model. The fluid looked nice. The temperature propagated quickly ( in under a second). But looking at the heat transfer, it looks really, really low.

 

2. So I put a model together with tubing in the model (with the tubing deactived after meshing). It finishes with no result with tet mesh, and give the results shown with tet/wedges. The faces of the mating halves are excluded as well as the inlete/outlet before tet/wedges mesh. It gets some dead elements and nodes.

 

Does 1. seem low to you? Instead of sending it through tube, maybe I should mesh the helical fluid into a big "reservoir" of fluid for the BTUs/s of heat transfer?

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Autodesk Design & Make Report