[flippy]

Hello guys!

I'm a final year student trying to complete a project using Ansys FLUENT. One step of which is to try to simulate a 3D pipe flow, then compare the simulation results to Poiseuille's law.

Now, the problem is, the pressure gradients I got from the 3D simulation is nowhere near the one calculated with Poiseuille's equation. What could possibly have gone wrong with my settings?
- I created and meshed a cylinder - with inlet, wall, outlet as boundaries
- Laminar flow
- No-slip wall
- Outlet = outflow, inlet = velocity-inlet (with a known velocity at inlet)
- Solution method: SIMPLE
- The pipe is long enough for the flow to be fully developed before it reaches the outlet

I've read through a few tutorials on pipe flows and such, and managed to follow through the steps, but the problem still persists. So now I'm kinda at a loss.

Any suggestions?

[victoryv]

You need to have fine mesh at the boundaries to resolve the boundary layers. Change the residuals accuracy to 10^-6 and monitor other parameters as well along with the residuals.

[Far]

Outlet = outflow

Make it pressure outlet

[flippy]

Originally Posted by victoryv

You need to have fine mesh at the boundaries to resolve the boundary layers. Change the residuals accuracy to 10^-6 and monitor other parameters as well along with the residuals.

Thanks. I'll try this tomorrow and see how it goes.

Originally Posted by Far

Make it pressure outlet

Isn't this only used when the outlet pressure is a known value? That isn't my case, actually; I'm just trying to find the pressure drop between the inlet an outlet. Please do clarify this for me if you don't mind?

[Far]

hmmmmm

I am talking about static pressure at outlet

[Jabba]

Hello,

I believe that you are simulating an incompressible flow, so I will proceed from that hypothesis.. you should verify if your mesh has an adequate resolution as someone said before

regarding the numerical schemes that you applied, they seem adequate.. which interpolation methods are you using for pressure and other variables?

if your domain is long enough so you really have a developed flow at the outlet, pressure outlet and outflow should give the same results

you need to specify a pressure reference (Pref) and a static pressure (P) at somewhere, preferable at the outlet since you are using a velocity inlet boundary condition.. in this way, the static pressure at the intlet will be resolved

since the flow is incompressible, SIMPLE and the others methods, such as PISO, will resolve the flow for a determined pressure P+Pref, so I guess it really doesn't matter which Pref you input, you will get the same pressure drop between inlet and outlet (again, reminding that the flow is incompressible)

[flippy]

Hello Jabba,

Yes it is incompressible flow. I guess my mesh should be at a reasonable resolution, because I set it as close to the limit as possible (the version I'm using is academic version so it has a limit of 512000 cells, mine is pretty close to that).

Regarding the P-ref I've tried:
- setting a value at the inlet
- not touching it
Both give approx. same result which is about 30% off from Poiseuille's equation result.

I've tried doing the same model, but in 2D, and the result is pretty close to Poiseuille's, so I'm guessing there's not much else I can do is there?

[flotus1]

Poiseuille flow can be simulated up to the limits of computational accuracy of the system.
So the 30% deviation you still have clearly indicate that there is something wrong with your simulation setup.
And even in 3D, you dont need 512k cells to achieve accurate solutions.

[flippy]

Originally Posted by Jabba

which interpolation methods are you using for pressure and other variables?

I leave them as they are. Pressure was Standard I believe, can't seem to remember what the others are, though.

Originally Posted by flotus1

Poiseuille flow can be simulated up to the limits of computational accuracy of the system.
So the 30% deviation you still have clearly indicate that there is something wrong with your simulation setup.
And even in 3D, you dont need 512k cells to achieve accurate solutions.

That's what I fear...

Well I can't be the only one with these problems can I, so any suggestions to what I should look at for mistakes?

[flotus1]

Although the solution is quite straightforward, there are of course many possibilities to make bad decisions for a CFD beginner and even some traps for experienced users (see http://www.cfd-online.com/Forums/flu...ical-pipe.html)

Lets go through the setup:

1. Check your mesh! Especially the actual size of the domain.
2. Use laminar viscous model
3. Check the viscosity of your fluid (dynamic viscosity!)
4. Check if your domain uses the correct fluid
5. for the easiest setup, use pressure inlet/pressure outlet boundary conditions. Check that the pressure difference is actually small enough to ensure laminar flow.
6. Use second order upwind for the convective fluxes
7. under monitors, untick the "check convergence" boxes for all equations
8. Initialize with zero velocity or with the expected bulk velocity
9. Run as many iterations until the residuals level out
10. If still not satisfied with the solution, use a better mesh

[Jabba]

also try to use PRESTO! for pressure interpolation

regards

[flippy]

So today I gave the simulation another try and I'm still not getting anywhere near the theoretical values.

Here's my case if anyone wanna try and see if they can get the desired results:
- Pipe dia: 1.6cm
- Pipe length: 50cm
- Flow speed: 0.6 m/s
- Steel pipe, fluid = water
- Models: Viscous - Laminar
- Scheme: SIMPLE
- Gradient: Least Squares Cell Based
- Pressure: Standard
- Momentum: 2nd order upwind
- Monitoring the area-weighted values of pressure at inlet and outlet
- Residual 10^-5

[Jabba]

for these conditions, isn't the flow turbulent? Re ~ 9500?

[flippy]

Originally Posted by Jabba

for these conditions, isn't the flow turbulent? Re ~ 9500?

Oh dear the dimensions were wrong, they were supposed to be mm, not cm, sorry!
Right I'll run the simulations again tomorrow with correct dimensions!

Just to clear things out: Only the one I ran today was with wrong dimensions, the ones before that I did with correct dimensions for laminar flow.

[flotus1]

Originally Posted by flotus1

Lets go through the setup:

1. Check your mesh! Especially the actual size of the domain.
2. Use laminar viscous model
3. Check the viscosity of your fluid (dynamic viscosity!)
4. Check if your domain uses the correct fluid
5. for the easiest setup, use pressure inlet/pressure outlet boundary conditions. Check that the pressure difference is actually small enough to ensure laminar flow.
6. Use second order upwind for the convective fluxes
7. under monitors, untick the "check convergence" boxes for all equations
8. Initialize with zero velocity or with the expected bulk velocity
9. Run as many iterations until the residuals level out
10. If still not satisfied with the solution, use a better mesh

Why is nobody listening to me...

[Far]

What results you are expecting? What is the viscosity of Fluid?

[flippy]

@Far:
the fluid is water - viscosity 0.001003 kg/m-s = copied from fluent itself.

So I've run the simulation again today (with correct dimensions!!)
- Re is about 960 so it is laminar
- Monitoring: Vertex average of static pressure at outlet - gives a value of about 600 Pa, while the pressure drop from Poiseuille's is about 375 Pa so clearly there's still something wrong, or I'm monitoring the wrong thing (which shouldn't be the case because that's what I did with the 2D model and I was able to get the result as close as 5% to the Poiseuille's value)
- I tried with air as the fluid and the results I get is still slightly different from Poiseuille's (CFD value: about 7 Pa, Poiseuille's: about 6.7 Pa)

One thing I noticed is the volumetric flow rate at the inlet. According to my calculations it should be 1.206e-6 m3/s, while the value used in FLUENT was 1.188e-6 m3/s (monitoring volumetric flow rate at the inlet as well), could this be the reason?

[Far]

I am getting same value of volume flow rate i.e. from Fluent and Analytical. what is operating pressure?

[flippy]

Originally Posted by Far

I am getting same value of volume flow rate i.e. from Fluent and Analytical. what is operating pressure?

~10.1^5 Pa

[Far]

Originally Posted by flippy

~10.1^5 Pa

it is 1.01 ^ 5 or 10.1 ^5 pa?