!!! Fluid Flow Q does not equal VA !!!

[Anonymous]

Boundary Conditions

Velocity = 500 ft/s (assigned at inlet)

Prescribed Turbulence (at inlet)

Prescribed Outlet

Mesh: tets & wedges with inlet/outlet removed from boundary layer

Area = 1 ft^2

Length = 1 ft

Material: Air

Q should equal 500 ft^3/s but does not, not even close

Same happens for LES and/or tet mesh only (Presribed Turbulence deactived)

[Joey.X]

Specified velocity at inlet  applies to interior nodes only, and the wall nodes on the inlet surface have zero velocity, so  the effective flow rate can't be simply calculated by velocity by inlet area. The flow rate for element near by wall need apply trapezoid rule with zero velocity for wall nodes and full velocity for interioe nodes. 

[Anonymous]

Joey.X

You are very correct, as lab testing with a metering moved in the stream will demonstrate emperical test results at the conduit wall to be V about equal to zero. Whereas toward the center of the tube stream, it should be expected test results would give as I mentioned in my case, close to 500 ft3/s. I am getting CFD max results 10-18    (at the center) of what they should be. Please review my setup and recommend changes. Maybe the prescribed turbulence settings? Maybe something in the analysis parameters?

Again, how does one achieve turbulence results Y+ of 30 as recommended in the Wiki?

Detailed answers are appreciated.

[Joey.X]

a. Assuming you did math with Reynolds number calculation, Re=3110 is below the critical value Re=3200, so the laminar flow is not necessary to apply turbulence model.

b. To compare experiment or theory result which are usually fully developed flow, your model is too short at length direction so that the result is away from fully developed profile. 

I suggest you check most recent simulation Multiphysics AVE(Accuracy Verification) manual (with archive models), one of the models is laminar pipe flow which has detail velocity profile and pressure drop comparison vs. theory result.

[Anonymous]

Joey.X,

I did check two things. 1. My material viscosity was wrong. Changing that increased Re significantly. 2. The length (L) for the epsilon scale factor should be the inlet characteristic length, not the conduit length.

I am still getting results a magnitude of 10^-3 of what they should be.

I will take your suggestion and lengthen the conduit. In the meanwhile, please answer this:

1. Please provide length for this. Multiphysics AVE (Accuracy Verification) manual

Prescribed Turbulence

1. Best value range for KE intensity  (I) = _________?

2. Best value range for turbulent kinetic dissipation scale factor (SF) = ______________?

Analysis Parameters (Turbulence)

1. Characteristic inlet velocity scale = _________ (ft/s) ?

Analysis Parameters (Formulation Options)

1. Number of pressure smoothing passings = ___________?

Analysis Parameters (Solver Options)

1. SSOR = ___________?

Again, how does one achieve turbulence results Y+ of 30 as recommended in the Wiki?

Detailed answers and special interest to this thread is appreciated! I'm not the only one with this problem as alok, tim.sefton may benefit too! Please collaborate with Astro.John if the communication language is posing difficulty. I am confident by the 8th message, we'll have this solved with this approach.

[Anonymous]

1. Please provide length (should be link, sorry) for this. Multiphysics AVE (Accuracy Verification) manual

[Joey.X]

It appears to me that AVE DVD is not free and no free link avalible, somebody please correct me if I am wrong on this info.

There are no best value for inlet TKE parameters, it depends on the flow turbulence degree from your physical model, it's user's option to apply.

For your specific problen, I would suggest doing it via LES turbulence model first. 

[Joey.X]

A correction for my last reply, here is link for the simulation MP AVE

[Anonymous]

Joey.X

There has to be some range for the TKE parameters, maybe not BEST. I did the LES. The results stink too. I don't know how many times I have to explain that. Please answer the following. If there's no best, then please give examples of what you are talking about. DETAIL  DETAIL  DETAIL PLEASE.

Prescribed Turbulence

1. Range for KE intensity  (I) = _________?

2. Range for turbulent kinetic dissipation scale factor (SF) = ______________?

Analysis Parameters (Turbulence)

1. Characteristic inlet velocity scale = _________ (ft/s) ?

Analysis Parameters (Formulation Options)

1. Number of pressure smoothing passings = ___________?

Analysis Parameters (Solver Options)

1. SSOR = ___________?

Again, how does one achieve turbulence results Y+ of 30 as recommended in the Wiki?

[John_Holtz]

Hi,

Now that I think about it, Mach 0.45 is pretty high for our software to solve! (One of your images implied you were working with air.) Did you get any warnings during the solution? My guess is that the analysis is not converging, in which case the accuracy has nothing to do with turbulence or other setup, per se.

It is difficult to determine a problem without having the actual model "to touch". Please see the post "Create, Post, or Provide an Archive of your model" and attached the archive to your reply.

Thanks.

[Anonymous]

John,

Mach number is a non-issue, as there is convergence and the result is the same for low mach numbers. Q does not equal VA. Also, I ran the AVE 175 as it is the closest scenario. It is fine with brick and tets mesh. I ran the following using the same settings as AVE 175 (but used velocity at one end and prescribed outlet the other instead of the pressures and inlet/outlet) but Q still does not equal VA.

Please find the attached and I have changed the BC's.

Boundary Conditions

Velocity = 10 ft/s (assigned at inlet surface)

Prescribed Turbulence: (none)

Prescribed Outlet (opposite end of velocity surface)

Mesh: bricks and tets

Area = 1 ft^2 (d=1.128 ft)

Length = 10 ft

Material: Water

LES

It is turbulent (Re=1,046,263) so that is set to (1)

Q should equal 10 ft^3/s but does not, not even close, not even in the middle of the pipe. Many different scenarios tried. Q does not equal VA UUUGGGHHH!!!! It should not be this difficult for something this simple.

[John_Holtz · Accepted solution]

Hi,

Unless I overlooked it in one of the posts, the one thing we needed to know is "how are you calculating the total flow rate?".

For your model provided, the theoretical inlet flow rate is 6.81 ft^3/s, and the outlet flow obtained from the software is 6.66 ft^3/s. Since there are 5 warnings in the simulation implying that there may be a problem, I would say that the two flow rates are very close. (My calculations and explanations are below.)

Thanks for the model and thread. I have learned a lot from it! I can see how readers of the documentation might have difficulty understanding what to do, so I will try to update the documentation wiki with some of these findings (as well as enter some software change requests).

1. I suspect that you are looking at the flow rate ("Results Contours > Velocity and Flow > Flow Rate Through Face") and have the smoothing turned on ("Results Contours > Settings > Smooth Results" is selected blue) and are looking at the results at the nodes. It is complicated to explain why, but these results are so misleading or not useful at all that you can consider them to be "wrong". 
2. The settings you want are smoothing turned off ("Results Contours > Settings > Smooth Results" is not selected) and inquire on the results at the faces ("Selection > Select > Faces" or "Selection > Select > Surfaces").
3. To get the flow rate out, use surface selection ("Selection > Select > Surfaces"), click on the outlet face, and "Results Inquire > Inquire > Current Results". This will list the flow rate through each selected face. In the "Summary" drop-down, choose "Sum". If you are looking at the last time step, the sum will be 6.66 ft^3/s.
4. Not surprising, the inlet flow rate given by the software is 6.65 ft^3/s: a "perfect" match. The theoretical inlet flow rate is not 10 ft^3/s; the answer is the integral of V*A. Since the velocity at the wall is 0, the average velocity in the outer ring of elements would be 5 ft/s. The velocity in the inner ring of elements is 10 ft/s. From Figure 1, I get the flow rate 6.81 ft^3/s.
5. To view the warnings, click the Report tab ("Tools > Environments > Report") and click the entry under "Steady Fluid Flow > Log". This displays the log file. Click in the log file, then press Ctrl+F to bring up the find dialog. The warning message is "Warning: Converge with stagnation due to oscillation". I do not know the details of stagnation, but basically the simulation got as far as it could on that step. Performing more iterations would just return the same result. Based on the default setting, the simulation prints a warning and continues to the next step. Since this warning occurred on all 5 time steps, no results in your analysis are a converged solution. In situations where convergence problems occur in a steady fluid flow, you may have better success with an unsteady fluid flow.
   

Figure 1: Teoretical Inlet Flow Rate

Let us know if you have any questions.

[Anonymous]

John,

Thanks. I'm on 2011 and don't have some of the features described but got through it. I did get the 6.65 ft^3/s after following your instructions and by inquiring sum on the inlet/outlet surface.

Just a couple more questions and a comment. Does your integral look like the one below? I'm not getting the theoretical answer of 6.81 ft^3/s. And I am guessing the screen scale shown means nothing?

Also, I re-ran the analysis with tets/wedges mesh, the sum on the faces is now 9.60 ft^3/s? Strange!

[John_Holtz · Accepted solution]

Sorry. "Theoretical Inlet Flow Rate" shown in my Figure 1 in the previous post would be more accurate if it had read "Hand Calculated Flow Rate". For the inner "circle" of 17 faces, the area is 0.402 ft^2 times a uniform flow rate of 10 ft/s gives 4.02 ft^3/s. Likewise for the outer annulus of faces, I assumed that the flow rate is based on the average velocity (0 at the wall, 10 on the inside of the annulus, giving an average of 5 ft/s). 2.79 ft^3/s + 4.02 ft^3/s = 6.81 ft^3/s. (I calculated by areas by drawing two sketches and "tracing" the inner and annulus areas using construction lines, and then using the software to calculate the cross sectional area of the sketch.)

When I got into the office this morning, the developer explained how my "hand calculation" was too simple. The software is doing a more sophisticated calculation of the average flow rate across the face of a given element. So the "average" flow rate in the annulus is smaller than 5 ft/s, so the flow rate in the annulus is smaller than 2.79 ft^3/s, and the total flow rate is smaller than 6.81 ft^3/s. So the flow rate given by the software, 6.65 ft^3/s, is the correct hand calculation.

The Flow Rate scale shown in the Results environment essentially has no physical meaning IF smoothing is turned on ("Results Options > Smooth Results" in 2011, "Results Contours > Settings > Smooth Results" in 2012). When smoothing is turned off, the flow rate values shown in the legend are the flow through each face of the elements. Thus, you can select the outlet by surface, inquire on the results (the flow through each face), and sum them to get the total flow through the face.

When you say that you created a simulation using tets and wedges, I think you are saying that you created a boundary layer mesh. By making the other annulus of elements smaller, the calculation gets closer to the theoretical result of 10 ft/s over the entire face (just like your integral). So I am not surprised that the new analysis gives 9.60 ft^3/s.

[Anonymous]

Thanks John and Joey.

This thread will be helpful for most as a guide for closed channel CFD problems. I'd agree with John the software and documentation needs updating. Would be nice if the legend reported the sum flow rate and if probing reported flow rate throughout the conduit. Also, would be nice if the documenation update included how to reach the theoretical solution through integration. Videos would be nice too!