Pressure drop does not match theory

[Omish]

I've modeled a U-Pipe with laminar flow. The pressure drop from Fluent is about 3 kpa , but by theory it should be about 6 kpa (checked several times and I'm sure)
My mesh is very fine and boundary conditions are vel-inlet and pre-outlet and wall. Would you please help me with the problem?

 

[boneh3ad]

Based on which theory?

 

[Omish]

Based on which theory?

Darcy. The formula :
Delta P = f * (L/D) * (V^2/2) * rho

 

[boneh3ad]

That likely suggests that your estimate for $f$ is incorrect, since the other values are pretty straightforward.

 

[Omish]

That likely suggests that your estimate for $f$ is incorrect, since the other values are pretty straightforward.

Since in laminar flow f = 64/Re and Re=rho*V*D/dynamic viscosity ,f is also easy to calculate. And I'm sure about my theoretical answer.I think there must be some kind of special setting or algorithm & method change in Fluent I should take care of.

 

[boneh3ad]

The most obvious culprit with Fluent is that it is allowing the flow to be turbulent while your model assumes laminar flow. However, this would produce an error in the opposite direction. You'd expect a higher pressure drop in the turbulent case. In other words, if Fluent was modeling the flow as turbulent, you should see a higher calculated pressure drop, and your answer would tend to be higher than theory (if the theory is correct).

On the other hand, it is possible that, for a U-bend in the pipe, there would be additional losses associated with the bend that aren't accounted for in the Darcy-Weisbach equation. However, this again would tend to mean that your predictions get worse than they already are, not better. In other words, if all of your parameters in the Darcy-Weisbach equation were correct and the problem was leaving out losses associated with the bend, then you would expect that theory again is predicting less than Fluent (assuming your Fluent is correct).

The next best bet is that your friction factor is not estimated properly for the geometry that you put into Fluent or that something was wrong with your Fluent simulation. I don't know what to tell you there. Maybe your estimated your Reynolds number incorrectly or turned the wrong bells and whistles in Fluent.

 

[Chestermiller]

What do you get if you run Fluent for a straight pipe of the same length?

 

[Omish]

The most obvious culprit with Fluent is that it is allowing the flow to be turbulent while your model assumes laminar flow. However, this would produce an error in the opposite direction. You'd expect a higher pressure drop in the turbulent case. In other words, if Fluent was modeling the flow as turbulent, you should see a higher calculated pressure drop, and your answer would tend to be higher than theory (if the theory is correct).

On the other hand, it is possible that, for a U-bend in the pipe, there would be additional losses associated with the bend that aren't accounted for in the Darcy-Weisbach equation. However, this again would tend to mean that your predictions get worse than they already are, not better. In other words, if all of your parameters in the Darcy-Weisbach equation were correct and the problem was leaving out losses associated with the bend, then you would expect that theory again is predicting less than Fluent (assuming your Fluent is correct).

The next best bet is that your friction factor is not estimated properly for the geometry that you put into Fluent or that something was wrong with your Fluent simulation. I don't know what to tell you there. Maybe your estimated your Reynolds number incorrectly or turned the wrong bells and whistles in Fluent.

Thank you for you answer dear friend. The velocity is 0.585 m/s and D=0.01905 m, density= 992.3 kg/m^3, Dyn. viscosity=0.058 Pa.s . So Re number is about 190 and certainly it is laminar flow.
About loss for bend. Yes you are right and I have also considered and calculated them. They are very small compared with the main loss though since it's low Re problem. So makes not much difference. And as you said it makes the problem even worse.

 

[Omish]

What do you get if you run Fluent for a straight pipe of the same length?

I also tried this way. The same results come out. Still the fluent pressure drop is half the theoric amount.
I even tried CFX to model it. Again the same results were achieved.

 

[Chestermiller]

I also tried this way. The same results come out. Still the fluent pressure drop is half the theoric amount.
I even tried CFX to model it. Again the same results were achieved.

Let's see your hand calculation.

 

[Omish]

Let's see your hand calculation.

 

[boneh3ad]

What is your source for estimating viscosity? To me it looks like you are off by several orders of magnitude there.

 

[Chestermiller]

I confirm your hand calculation of the pressure drop. So the error must be in the implementation of the Fluent calculation. It sounds like you did not use the correct tube length. Is that possible? Did you only use half the U?

 

[Omish]

What is your source for estimating viscosity? To me it looks like you are off by several orders of magnitude there.

They are reported in a project of experimental work. I also tried with another case and material which had the viscosity of 0.108 Pa.s
The results were in the same manner. If you mean my viscosity amount is not normal what should be the range of normal viscosity?

 

[boneh3ad]

I confirm your hand calculation of the pressure drop. So the error must be in the implementation of the Fluent calculation. It sounds like you did not use the correct tube length. Is that possible? Did you only use half the U?

Did you check his value for viscosity? Assuming the working fluid is water (based on the density value he used), then his viscosity should be in the ballpark of 0.65×10^-3 Pa⋅s, quite a bit lower than what he has used.

They are reported in a project of experimental work. I also tried with another case and material which had the viscosity of 0.108 Pa.s
The results were in the same manner. If you mean my viscosity amount is not normal what should be the range of normal viscosity?

What is your working fluid here?

 

[Omish]

I confirm your hand calculation of the pressure drop. So the error must be in the implementation of the Fluent calculation. It sounds like you did not use the correct tube length. Is that possible? Did you only use half the U?

No I checked it several times. The lengths are all correct and the U-piep is modeled completely.

 

[Chestermiller]

It's hard to imagine that Fluent would get such a calculation incorrect. This would have been their first validation check. Is the fluid non-Newtonian, with shear rate dependence? Is the difference exactly a factor of 2?

 

[Omish]

Did you check his value for viscosity? Assuming the working fluid is water (based on the density value he used), then his viscosity should be in the ballpark of 0.65×10^-3 Pa⋅s, quite a bit lower than what he has used.
What is your working fluid here?

I also tried the same geometry by water. The results were not correct. There was fault by almost 40 percent. My material here is a nanofluid of SN 500/CuO which is being modeled as a one-phase fluid, just like in experimental project.

 

[Omish]

It's hard to imagine that Fluent would get such a calculation incorrect. This would have been their first validation check. Is the fluid non-Newtonian, with shear rate dependence? Is the difference exactly a factor of 2?

No it is Newtonian. But If it is more comfortable and confident let's go on with water. I think if the results with water become correct, the problem would be solved for my fluid too.

 

[Omish]

It's hard to imagine that Fluent would get such a calculation incorrect. This would have been their first validation check. Is the fluid non-Newtonian, with shear rate dependence? Is the difference exactly a factor of 2?

Did you check his value for viscosity? Assuming the working fluid is water (based on the density value he used), then his viscosity should be in the ballpark of 0.65×10^-3 Pa⋅s, quite a bit lower than what he has used.
What is your working fluid here?

Let me solve the model with water one more time and tell you the exact theoric and Fluent answers. So we won't have to worry about the material anymore.

 

[Chestermiller]

Let's keep our eye on the ball. The value of the viscosity is irrelevant to the comparison we are trying to make.

 

[boneh3ad]

Have you checked that you didn't accidentally mix up radius and diameter in your Fluent simulation?

 

[Omish]

Have you checked that you didn't accidentally mix up radius and diameter in your Fluent simulation?

Yes. I'm sure about this.

 

[Omish]

I found s.th about water test I had m

Let's keep our eye on the ball. The value of the viscosity is irrelevant to the comparison we are trying to make.

Have you checked that you didn't accidentally mix up radius and diameter in your Fluent simulation?

I tried again with water. But I changed the velocity to make it laminar flow. Something new I noticed. First I set Re to about 2300 (a bit less) and the fault was 16 percent (theoric=18.92 , Fluent=22.02 both pa). I thought the problem is solved ! BUT then again I set Re to about 190, and the fault became 57 percent ! So much difference.
So I think there's s.th wrong about low Re modeling. Can you help me with settings to make it right? What should I consider for LOW Re models?

 

[bigfooted]

So I think there's s.th wrong about low Re modeling. Can you help me with settings to make it right? What should I consider for LOW Re models?

Make sure the turbulence model is switched off. In the 'Viscous Model' tab, choose 'Laminar'.

Also note that the Darcy-Weisbach equation is valid for developed flow, so at the start of the bend you should have Poiseuille flow. You should have a sufficiently long piece of straight pipe before and after the bend in your simulation. Do you have this?

 

[Omish]

Make sure the turbulence model is switched off. In the 'Viscous Model' tab, choose 'Laminar'.

Also note that the Darcy-Weisbach equation is valid for developed flow, so at the start of the bend you should have Poiseuille flow. You should have a sufficiently long piece of straight pipe before and after the bend in your simulation. Do you have this?

Viscos-Laminar model has been chosen all the time.
And I think it is long enough in start and end. L_e=0.06*Re*D=0.06*190*0.01905=0.218 m
My pipe geometry is exactly like this: 1 meter straight pipe, a 90 degree bend, 11 cm straight pipe, one more 90 degree bend, and 1 meter straight pipe again (almost U-shaped). So there's one meter in start which is 5 times greater than L_e and enough for being fully developed.

 

[Omish]

Let's keep our eye on the ball. The value of the viscosity is irrelevant to the comparison we are trying to make.

Have you checked that you didn't accidentally mix up radius and diameter in your Fluent simulation?

Make sure the turbulence model is switched off. In the 'Viscous Model' tab, choose 'Laminar'.

Also note that the Darcy-Weisbach equation is valid for developed flow, so at the start of the bend you should have Poiseuille flow. You should have a sufficiently long piece of straight pipe before and after the bend in your simulation. Do you have this?

I finally found the problem ! So weird. for straight pipes the answer is wrong also UNLESS you model them as AXISYMMETRIC ! for my geometry (U-shaped pipe) is it possible to model it axisymmetric? if not what can I do now?

 

[256bits]

I finally found the problem ! So weird. for straight pipes the answer is wrong also UNLESS you model them as AXISYMMETRIC ! for my geometry (U-shaped pipe) is it possible to model it axisymmetric? if not what can I do now?

I was just going to ask if you poked on 2D or axisymmetric.

I would think the following should apply:
2d would be a calculation for a depth of 1 m on the z-axis. ie z-axis into the page, x-axis left to right, y -axis top to bottom.

Axisymmetric would be around an x-axis of radius D/2, for say a round tube.
Your x-axis for your u-shape tube would be the radial centerline from end to finish.
Ansys should allow you to set up your grid for complicated shapes.

 

[Omish]

I was just going to ask if you poked on 2D or axisymmetric.

I would think the following should apply:
2d would be a calculation for a depth of 1 m on the z-axis. ie z-axis into the page, x-axis left to right, y -axis top to bottom.

Axisymmetric would be around an x-axis of radius D/2, for say a round tube.
Your x-axis for your u-shape tube would be the radial centerline from end to finish.
Ansys should allow you to set up your grid for complicated shapes.

yes. I tried to use the centerline as my axis BC but Fluent gives errors and doesn't even run for 1 Iteration. The error is about diverging, but I'm pretty sure it's irrelevant; The cause I guess is that the axis is not straight but twisted because of U-shape.
any other suggestions?

 

[akbarff5]

can help me how to show pressure drop value in ansys fluent

 

[Chestermiller]

can help me how to show pressure drop value in ansys fluent

Please read the Rules and Guidelines for Physics Forums. If you want you questions answered on a subject different from that in a particular thread, merely start a new thread. Make sure you choose a descriptive title to attract members' attention, and clearly explain in detail what your problem is. Thank you.