Reynolds Number < 70 flow

[prashanth]

Hello people,

If we are working on the flow with reynolds number less than 70 as we all know the flow will be laminar in pipe. Now if the flow continues to flow through elbow fittings like 90 degrees, will we get any turbulence because of the elbow bend ? How to deal with this problem in ansys fluent like while selecting the flow condition? IF the flow is laminar i will select the laminar flow but even if there is a slight turbulence i should select k epsilon model but which near wall treatment (standard, scalable or enhanced wall treatment) should i choose ? ( i am new to ansys fluent)
i am dealing with the diameters ranging from (3mm to maximum 8 mm). flow rates ranging from (50 mlper min to 500 ml per minute).
I would be glad if someone could give some suggestions.

 

[bigfooted]

The elbow does not make the pipe flow turbulent. You do not need to consider a turbulence model for pipe flow for these low Reynolds numbers. Usually you have to start worrying about turbulence in pipes at Re>2000. Since you do not have a boundary layer, you do not need a fine mesh near the wall, just some cells that are small enough to capture the velocity gradient correctly.

'Some suggestion' : pay attention to the quality of the mesh (use sweeped meshes for instance and check the mesh quality on bad cells).

 

[boneh3ad]

The elbow could make the flow turbulent, but the low Reynolds number should mean all those disturbances are stable and will be damped out and return to laminar flow.

'Some suggestion' : pay attention to the quality of the mesh (use sweeped meshes for instance and check the mesh quality on bad cells).

I am no CFD expert and I certainly don't know all the knobs in ANSYS. What I do know is that, when using a code, two things are of paramount importance. One is knowing what "wall treatment" and "turbulence model" actually mean and the implications of each option. The other is that having a good grid is of paramount importance to getting a good answer.

 

[prashanth]

The elbow does not make the pipe flow turbulent. You do not need to consider a turbulence model for pipe flow for these low Reynolds numbers. Usually you have to start worrying about turbulence in pipes at Re>2000. Since you do not have a boundary layer, you do not need a fine mesh near the wall, just some cells that are small enough to capture the velocity gradient correctly.

'Some suggestion' : pay attention to the quality of the mesh (use sweeped meshes for instance and check the mesh quality on bad cells).

Thanks for your reply... I have started working on it. so i don't need to use inflation for my mesh i guess.

 

[prashanth]

The elbow could make the flow turbulent, but the low Reynolds number should mean all those disturbances are stable and will be damped out and return to laminar flow.



I am no CFD expert and I certainly don't know all the knobs in ANSYS. What I do know is that, when using a code, two things are of paramount importance. One is knowing what "wall treatment" and "turbulence model" actually mean and the implications of each option. The other is that having a good grid is of paramount importance to getting a good answer.

yeah i am not using turbulence model because of low reynolds number. Thanks foe your reply bro.

 

[essenmein]

How do you know what the reynolds number is or are you assuming you have a low reynolds number? To me the reynolds number is kind of the result of a certain combination of things, flow velocity, viscosity, density etc.

I think you can make some generalizations about flow in a pipe of a certain fluid however once you introduce bends, etc you very well may create local areas where there is significant shear stress causing turbulence.

I'd run with turbulence "ON" at least at first to confirm that you don't have turbulence, rather than assuming there is no turbulence.

 

[boneh3ad]

yeah i am not using turbulence model because of low reynolds number. Thanks foe your reply bro.

If your Reynolds number truly is that small, it likely won't matter anyway. The Reynolds stress terms will be tiny and the effects of the turbulence model would be pretty negligible.

How do you know what the reynolds number is or are you assuming you have a low reynolds number? To me the reynolds number is kind of the result of a certain combination of things, flow velocity, viscosity, density etc.

I think you can make some generalizations about flow in a pipe of a certain fluid however once you introduce bends, etc you very well may create local areas where there is significant shear stress causing turbulence.

I'd run with turbulence "ON" at least at first to confirm that you don't have turbulence, rather than assuming there is no turbulence.

The Reynolds number in a pipe is a pretty easy definition:
$$Re_D = \dfrac{\rho V D}{\mu}.$$
For this, the only one of those things that is a variable is $V$, and that corresponds to the mean velocity across the cross-section of the pipe. If a flow enters and leaves a bend with the same area, then $V$ isn't changing, so as long as you have a reasonable estimate for $V$, then you have a reasonable estimate for $Re_D$ even before doing the calculations and can make some pretty strong assumptions based on it. It's not like being off on your velocity, even by a factor of 2 or even 10, is going to change the Reynolds number by the two orders of magnitude required in order for turbulence to be an important consideration here.

In a bend, you certainly may get some interesting physics. The most important off the top of my head is likely to be the potential for flow separation, which can introduce some localized turbulence and losses in the pipe. If the incoming flow is laminar, though, you don't need a turbulence model to predict separation, and if it shows up in the results, you can adjust accordingly.

 

[essenmein]

If your Reynolds number truly is that small, it likely won't matter anyway. The Reynolds stress terms will be tiny and the effects of the turbulence model would be pretty negligible.



The Reynolds number in a pipe is a pretty easy definition:
$$Re_D = \dfrac{\rho V D}{\mu}.$$
For this, the only one of those things that is a variable is $V$, and that corresponds to the mean velocity across the cross-section of the pipe. If a flow enters and leaves a bend with the same area, then $V$ isn't changing, so as long as you have a reasonable estimate for $V$, then you have a reasonable estimate for $Re_D$ even before doing the calculations and can make some pretty strong assumptions based on it. It's not like being off on your velocity, even by a factor of 2 or even 10, is going to change the Reynolds number by the two orders of magnitude required in order for turbulence to be an important consideration here.

In a bend, you certainly may get some interesting physics. The most important off the top of my head is likely to be the potential for flow separation, which can introduce some localized turbulence and losses in the pipe. If the incoming flow is laminar, though, you don't need a turbulence model to predict separation, and if it shows up in the results, you can adjust accordingly.

Begs the question then, if not expecting turbulence or some other effect, why bother with the CFD at all when you can get the answer needed with some napkin math or excel?

 

[boneh3ad]

Begs the question then, if not expecting turbulence or some other effect, why bother with the CFD at all when you can get the answer needed with some napkin math or excel?

Depending on exactly what output @prashanth is looking to use, I'd say that yes, that's a very good question. Using Bernoulli with corrections for losses like Darcy-Weisbach would be simple and reasonably effective for most cases, and it even works for turbulent flow. Simulation would primarily be useful for trying to simulate the bends and loss-causing devices individually if you want to look into what is causing the losses, how big they are, and how to tweak the design to reduce them. Otherwise, I'd argue doing it the easy way that doesn't require a cluster is better.

 

[prashanth]

Depending on exactly what output @prashanth is looking to use, I'd say that yes, that's a very good question. Using Bernoulli with corrections for losses like Darcy-Weisbach would be simple and reasonably effective for most cases, and it even works for turbulent flow. Simulation would primarily be useful for trying to simulate the bends and loss-causing devices individually if you want to look into what is causing the losses, how big they are, and how to tweak the design to reduce them. Otherwise, I'd argue doing it the easy way that doesn't require a cluster is better.

Hello,
I am working on different diameter elbow for example 5mm inlet and 3 mm outlet. I can't use bernoulli equation because there will be two unknown variables, Pressure difference and Loss coefficient 'K'. I am using ansys to get the pressure difference values for different inlet velocities or flowrates and from those values i am trying to find the relationship between 'K' and 'Re'. As the 'K' value changes with Reynolds number. @bigfooted @boneh3ad @essenmein If you guys know any information on how to deal with this kind of problem let me know guys(about finding the relationship between K and Re). I would be glad to know. @essenmein And coming to the reynolds number when we have different diameters i am choosing inlet diameter as reference. i can choose outlet diameter too its not a problem, it depends on what i want to use in bernoulli equation either inlet or outlet.

 

[prashanth]

How do you know what the reynolds number is or are you assuming you have a low reynolds number? To me the reynolds number is kind of the result of a certain combination of things, flow velocity, viscosity, density etc.

I think you can make some generalizations about flow in a pipe of a certain fluid however once you introduce bends, etc you very well may create local areas where there is significant shear stress causing turbulence.

I'd run with turbulence "ON" at least at first to confirm that you don't have turbulence, rather than assuming there is no turbulence.

i am confused with the ansys actually because i am new to this software. so you are saying I have to use turbulence model like k epsilon and check for the turbulence regions and if it doesn't show any in velocity vector field i can continue with laminar option. For the low reynolds number i don't need to worry about separation region and secondary flow but for high reynolds number to detect these effects i have to use k-epsilon model right.

 

[essenmein]

i am confused with the ansys actually because i am new to this software. so you are saying I have to use turbulence model like k epsilon and check for the turbulence regions and if it doesn't show any in velocity vector field i can continue with laminar option. For the low reynolds number i don't need to worry about separation region and secondary flow but for high reynolds number to detect these effects i have to use k-epsilon model right.

Ok so I'm also not a CFD expert, just an EE lumped with optimizing air cooled heatsink, we don't have Fluent, we have CFX, but I'm mostly using autodesk CFD (because I know it and to get a lic for CFX usually means begging someone else to release it).

My understanding of NOT running with turbulence is to simply reduce computational effort, esp in larger models, to me if doing something simple like a single 90 elbow, it shouldn't take long to run so leaving turbulence on should not cause an issue and still give you the right result.

 

[boneh3ad]

My understanding of NOT running with turbulence is to simply reduce computational effort, esp in larger models, to me if doing something simple like a single 90 elbow, it shouldn't take long to run so leaving turbulence on should not cause an issue and still give you the right a good result.

I fixed it for you.

"All models are wrong, but some are useful."
- George P. Box

 

[essenmein]

I fixed it for you.

"All models are wrong, but some are useful."
- George P. Box

Hah, in my defense we validate FEA with measurements before trusting models...

 

[bigfooted]

A small remark: Turbulence models only give good predictions when the Reynolds number is sufficiently high and the flow is fully developed. They have big problems determining laminar from locally turbulent regions. If your Reynolds number is low, don't use a turbulence model.
These laminar flow simulations are very fast, I could get the loss coefficient as a function of Reynolds number in one hour on my workstation (using one geometry and changing the inlet velocity to vary the Reynolds number, very easy to setup in ansys workbench). just make sure that you have a long straight pipe before the bend to create a fully developed flow in the pipe. I also noticed that there are some papers about the topic in the micro-fluidics community so there is probably experimental data as well to verify your simulations.

 

[boneh3ad]

Hah, in my defense we validate FEA with measurements before trusting models...

The same thing happens with CFD. It's still a model, whether it is modeling a solid or a fluid.

 

[prashanth]

A small remark: Turbulence models only give good predictions when the Reynolds number is sufficiently high and the flow is fully developed. They have big problems determining laminar from locally turbulent regions. If your Reynolds number is low, don't use a turbulence model.
These laminar flow simulations are very fast, I could get the loss coefficient as a function of Reynolds number in one hour on my workstation (using one geometry and changing the inlet velocity to vary the Reynolds number, very easy to setup in ansys workbench). just make sure that you have a long straight pipe before the bend to create a fully developed flow in the pipe. I also noticed that there are some papers about the topic in the micro-fluidics community so there is probably experimental data as well to verify your simulations.

@bigfooted just curious have you tried giving the Velocity profile using UDF instead of adding long pipe in the front ?...I tried to give it through UDF but i was not getting the laminar velocity profile at the inlet. I found few codes in the interenet and tried but it was a failure. but i am working on the method you suggested though.

 

[bigfooted]

Try something like this, put the udf in the fluent directory and compile there:

#include "udf.h"
#include "mem.h"

/* 
      in fluent this will be available as a udf boundary condition in 
      Boundary Condition -> inlet -> Velocity Magnitude 
      after you compiled the udf using 
      User Defined -> Functions -> Compiled 
*/
DEFINE_PROFILE(bcInlet,thread,index) {
   /* coordinates x=x[0], y=x[1], z=x[2] */
   real x[ND_ND];
   /* pointer to the face */ 
   face_t face;
   /* loop over the cell faces in a thread (a thread is a named selection) */
   begin_f_loop(face,thread){
      /* put the spatial coordinates of the face center in x */
      F_CENTROID(x,face,thread);
      /* assuming x=x[0] is the radial direction of the pipe and the radius is 1*/
      /* put your actual profile here */
      F_PROFILE(face,thread,index) = -(x[0]-1)*(x[0]+1);
   }
end_f_loop(face,thread);
}

There are some examples here:
http://jullio.pe.kr/fluent6.1/help/html/udf/node71.htm

 

[prashanth]

Try something like this, put the udf in the fluent directory and compile there:

#include "udf.h"
#include "mem.h"

/*
      in fluent this will be available as a udf boundary condition in
      Boundary Condition -> inlet -> Velocity Magnitude
      after you compiled the udf using
      User Defined -> Functions -> Compiled
*/
DEFINE_PROFILE(bcInlet,thread,index) {
   /* coordinates x=x[0], y=x[1], z=x[2] */
   real x[ND_ND];
   /* pointer to the face */
   face_t face;
   /* loop over the cell faces in a thread (a thread is a named selection) */
   begin_f_loop(face,thread){
      /* put the spatial coordinates of the face center in x */
      F_CENTROID(x,face,thread);
      /* assuming x=x[0] is the radial direction of the pipe and the radius is 1*/
      /* put your actual profile here */
      F_PROFILE(face,thread,index) = -(x[0]-1)*(x[0]+1);
   }
end_f_loop(face,thread);
}

There are some examples here:
http://jullio.pe.kr/fluent6.1/help/html/udf/node71.htm

Thanks man you have been very helpful...I will look into it...

 

[gmax137]

When doing piping losses "by hand" -- like using Crane 410, I was always told to use the Re dependent friction factor for friction, but to use the turbulent value (fT) for the fittings (for instance, a standard 90 degree elbow use k=30*fT). Maybe that's just how the empirical data was boiled down? Sorry if this is tangential to the thrust of this thread.

 

[prashanth]

When doing piping losses "by hand" -- like using Crane 410, I was always told to use the Re dependent friction factor for friction, but to use the turbulent value (fT) for the fittings (for instance, a standard 90 degree elbow use k=30*fT). Maybe that's just how the empirical data was boiled down? Sorry if this is tangential to the thrust of this thread.

We can't use the crane method to find it in laminar flow right ?