Discussion Groups

## Simulation Mechanical and Multiphysics

Employee
Posts: 492
Registered: ‎03-25-2010

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

07-18-2012 12:21 PM 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.

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)
Distinguished Contributor
Posts: 112
Registered: ‎03-31-2011

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

07-18-2012 02:56 PM in reply to: INACTIVE_AstroJohn

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.

Valued Contributor
Posts: 98
Registered: ‎06-19-2012

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

07-18-2012 03:41 PM 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!

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

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

07-23-2012 05:07 AM 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?

Employee
Posts: 492
Registered: ‎03-25-2010

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

07-23-2012 07:50 AM 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.)

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)
Distinguished Contributor
Posts: 112
Registered: ‎03-31-2011

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

07-23-2012 02:56 PM in reply to: INACTIVE_AstroJohn

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?﻿

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

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

07-24-2012 06:36 AM 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!

Employee
Posts: 492
Registered: ‎03-25-2010

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

07-24-2012 06:59 AM 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. 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!

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)
Distinguished Contributor
Posts: 112
Registered: ‎03-31-2011

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

07-26-2012 05:32 AM in reply to: INACTIVE_AstroJohn

Thanks Astro.

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

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

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

08-19-2012 08:28 PM 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?