Inlet velocity boundary conditions and pressure-poisson equation

FMDenaro · April 17, 2018, 13:53

This condition generates a du/dx term that must be balanced by the dv/dy in the continuity. You will see a slight deviation of the streamlines, depending on the Reynolds number. This is typical for a spatially developping boundary layer
But I suggested to prescribe the Poiseuille velocity everywhere to see if it is mantained. In such a case no deviation at the corner must appear

selig5576 · April 17, 2018, 14:41

Just to make sure I understand you. When you say "prescribe the Poiseuille velocity everywhere" you mean as the inlet BC (as opposed to an initial condition.) The profile I'm working with is

$u_{1,j} = (2.0/3.0)*(1.0 - (y_{1,j}/4.0)^{2}),$
4.0 is the width of my channel.

FMDenaro · April 17, 2018, 14:43

Quote:

Originally Posted by selig5576

Just to make sure I understand you. When you say "prescribe the Poiseuille velocity everywhere" you mean as the inlet BC (as opposed to an initial condition.) The profile I'm working with is

$u_{1,j} = (2.0/3.0)*(1.0 - (y_{1,j}/4.0)^{2}),$
4.0 is the width of my channel.

yes a parabolic profile, the constant of the parabola depends on the flow rate...

selig5576 · April 17, 2018, 15:10

After testing my solver with a Poiseuille profile my pressure profile still looks incorrect. To me, this points to an issue at the bottom left corner and top left corner BC for pressure, yet I don't see anything incorrect about the way I'm setting the BC.

$R_{2,ny-1} = \left(\frac{uf^{*}_{2,ny-1} - u_{1,ny-1}^{n+1}}{\Delta x} - \frac{v^{n+1}_{2,ny} - vf^{*}_{2,ny-2}}{\Delta y}\right)$
$P_{2,ny-1} = (1-\omega)P_{2,ny-1} + \frac{\omega}{\frac{1}{dx^{2}} + \frac{1}{dy^{2}}}\left(\frac{1}{dx^{2}} P_{3,ny-1} + \frac{1}{dy^{2}} P_{2,ny-2}\right)$

Code:

!Top left corner
R(2,ny-1) = (rho/dt)*(inv_dx*(ufs(2,ny-1) - un(1,ny-1)) + inv_dy*(vn(2,ny) - vfs(2,ny-2)))
P(2,ny-1) = (1.0-omega)*P(2,ny-1) + omega/(inv_dxx + inv_dyy)*(inv_dxx*P(3,ny-1) + inv_dyy*P(2,ny-2) - R(2,ny-1))

Code:

!Bottom left corner
R(2,2) = (rho/dt)*(inv_dx*(ufs(2,2) - un(1,2)) + inv_dy*(vfs(2,2) - vn(2,1)))
P(2,2) = (1.0-omega)*P(2,2) + omega/(inv_dxx + inv_dyy)*(inv_dxx*P(3,2) + inv_dyy*P(2,3) - R(2,2))

Note: [MATH]uf,vf[/MATH} refer to the cell faces which I use simple arithmetic averaging.

EDIT 1: At step 550 the velocity profile seems to look better.

FMDenaro · April 17, 2018, 15:34

Quote:

Originally Posted by selig5576

After testing my solver with a Poiseuille profile my pressure profile still looks incorrect. To me, this points to an issue at the bottom left corner and top left corner BC for pressure, yet I don't see anything incorrect about the way I'm setting the BC.

$R_{2,ny-1} = \left(\frac{uf^{*}_{2,ny-1} - u_{1,ny-1}^{n+1}}{\Delta x} - \frac{v^{n+1}_{2,ny} - vf^{*}_{2,ny-2}}{\Delta y}\right)$
$P_{2,ny-1} = (1-\omega)P_{2,ny-1} + \frac{\omega}{\frac{1}{dx^{2}} + \frac{1}{dy^{2}}}\left(\frac{1}{dx^{2}} P_{3,ny-1} + \frac{1}{dy^{2}} P_{2,ny-2}\right)$

Code:

!Top left corner
R(2,ny-1) = (rho/dt)*(inv_dx*(ufs(2,ny-1) - un(1,ny-1)) + inv_dy*(vn(2,ny) - vfs(2,ny-2)))
P(2,ny-1) = (1.0-omega)*P(2,ny-1) + omega/(inv_dxx + inv_dyy)*(inv_dxx*P(3,ny-1) + inv_dyy*P(2,ny-2) - R(2,ny-1))

Code:

!Bottom left corner
R(2,2) = (rho/dt)*(inv_dx*(ufs(2,2) - un(1,2)) + inv_dy*(vfs(2,2) - vn(2,1)))
P(2,2) = (1.0-omega)*P(2,2) + omega/(inv_dxx + inv_dyy)*(inv_dxx*P(3,2) + inv_dyy*P(2,3) - R(2,2))

Note: [MATH]uf,vf[/MATH} refer to the cell faces which I use simple arithmetic averaging.

EDIT 1: At step 550 the velocity profile seems to look better.

The solution appears still like the inlet profile you prescribed is not the correct parabolic solution.

selig5576 · April 18, 2018, 15:21

Disregard what the 2/3 I wrote. I am doing $u_{1,j} = \dot{m} (1 - (y/L_{x})^{2}$ . With that said I am still getting the two "dots" for pressure. In terms of plotting the profile I am in fact getting a parabolic profile.One screenshot is after 150 time steps and the second image is after 22k time steps, in which it converged to a steady state.

FMDenaro · April 18, 2018, 15:33

Quote:

Originally Posted by selig5576

Disregard what the 2/3 I wrote. I am doing $u_{1,j} = \dot{m} (1 - (y/L_{x})^{2}$ . With that said I am still getting the two "dots" for pressure. In terms of plotting the profile I am in fact getting a parabolic profile.One screenshot is after 150 time steps and the second image is after 22k time steps, in which it converged to a steady state.

As you see, the inlet parabolic profile is strongly modified in the interior. If you prescribe the exact solution that would not happen, the inlet profile repeats itself along x

selig5576 · April 18, 2018, 15:38

Maybe I am not understanding you, but are you saying I should not be prescribing the profile I gave in the previous post, but rather the analytical solution to the plane Poiseuille problem?

FMDenaro · April 18, 2018, 15:41

Quote:

Originally Posted by selig5576

Maybe I am not understanding you, but are you saying I should not be prescribing the profile I gave in the previous post, but rather the analytical solution to the plane Poiseuille problem?

yes, you have to check if your code accept the exact solution without changing

selig5576 · April 19, 2018, 11:58

So I'm using the analytical solution to plane Poiseuille flow $u_{1,j} = \frac{1}{2 \mu} \frac{dP}{dx} \left(y^{2} - h^2\right)$ , but my solution instantly diverges due to the pressure gradient in x.

FMDenaro · April 19, 2018, 12:08

Quote:

Originally Posted by selig5576

So I'm using the analytical solution to plane Poiseuille flow $u_{1,j} = \frac{1}{2 \mu} \frac{dP}{dx} \left(y^{2} - h^2\right)$ , but my solution instantly diverges due to the pressure gradient in x.

After one time step?? that is not a numerical instability but is due to a bug in the code...

selig5576 · April 19, 2018, 15:18

When determining dp/dx I read I should use the difference between the inflow and outflow pressure, is that correct? Otherwise I do not think there is a bug in my BC routine.

FMDenaro · April 19, 2018, 15:45

The velocity in a channel of height H for y=(-H/2:+H/2) is

u(y) = -(6Q/H^3)*(y^2-H^2/4)

The parameter being Q=u_average*H.

If you are using non-dimensional values you can just make non-dimensional the previous law

selig5576 · April 20, 2018, 12:13

Thank you for bite. It seems like my profile seems to be actually correct. So far, no dots in the vicinity of the inlet appear.

FMDenaro · April 20, 2018, 12:21

The last figure seems a correct solution, what about the first one? Is it at the first time step and you set an inviscid initial condition?

selig5576 · April 20, 2018, 12:23

Sorry I did not caption them

. The first one is only after 150 time steps, so its quite immature in the development of the flow.

EDIT: The pressure profiles seem to be consistent from what we would expect given the type of problem.

FMDenaro · April 20, 2018, 12:24

Quote:

Originally Posted by selig5576

Sorry I did not caption them

. The first one is only after 150 time steps, so its quite immature in the development of the flow.

Have you tried to set the exact profile everywhere as initial condition? The code should not change the initial condition and your pressure solver should converge immediately

selig5576 · April 20, 2018, 12:35

Yes, I have done that and it converges to the fully developed flow within 2-5 iterations.

FMDenaro · April 20, 2018, 12:41

Ok, seems to be ok.

selig5576 · April 24, 2018, 13:28

Returning back to my 3D solver. Here is my situation: If I have no outflow boundary conditions and run a lid driven cavity problem, my code returns the correct solution. As soon as I implement outflow boundary conditions (even a 1 x 1 x sized domain with 32^3 points) my pressure solver diverges. Interesting thing I've noticed is if I remove the advection term, my pressure solver does not diverge. Since I had validated my advection scheme on the LDC, I do not believe my discretization is wrong. I think the criminal is my pressure solver. There are only 5 pressure BCs with outflows conditions. The the outlet in x at the normal and the 4 corner pressure BCs at the outlet.

Example:
$R_{nx-1,2,2} = \frac{\rho}{dt}\left(\frac{vf^{*}_{nx-1,2,2} - v^{n+1}_{nx-1,2,2}}{dx} + \frac{wf^{*}_{nx-1,2,2} - w^{n+1}_{nx-1,2,1}}{dz}\right)$
$P_{nx-1,2,2} = (1-\omega)P_{nx-1,2,2} + \frac{\omega}{1/dy^2 + 1/dz^2}\left(\frac{1}{dy^{2}}P_{nx-1,3,2} + \frac{1}{dz^{2}}P_{nx-1,2,3} - R_{nx-1,2,2}\right)$

I prescribe this at

P(nx-1,ny-1,2),P(nx-1,2,nz-1),P(nx-1,ny-1,nz-1)

as well.

Mathematically, I believe the outlet BC is causing continuity at the faces to be violated, thus causing my PPE to diverge. Though the role of advection in causing this is currently confusing me. This divergence of pressure happens at around 480 SOR iterations. I am also using a plug inlet.

April 17, 2018, 13:53		#21
FMDenaro Senior Member Filippo Maria Denaro Join Date: Jul 2010 Posts: 6,773 Rep Power: 71	This condition generates a du/dx term that must be balanced by the dv/dy in the continuity. You will see a slight deviation of the streamlines, depending on the Reynolds number. This is typical for a spatially developping boundary layer But I suggested to prescribe the Poiseuille velocity everywhere to see if it is mantained. In such a case no deviation at the corner must appear selig5576 likes this. Last edited by FMDenaro; April 17, 2018 at 16:07.

April 17, 2018, 14:41	Poiseuille flow	#22
selig5576 Senior Member Selig Join Date: Jul 2016 Posts: 213 Rep Power: 10	Just to make sure I understand you. When you say "prescribe the Poiseuille velocity everywhere" you mean as the inlet BC (as opposed to an initial condition.) The profile I'm working with is $u_{1,j} = (2.0/3.0)*(1.0 - (y_{1,j}/4.0)^{2}),$ 4.0 is the width of my channel.

April 18, 2018, 15:38	Poiseuille flow	#28
selig5576 Senior Member Selig Join Date: Jul 2016 Posts: 213 Rep Power: 10	Maybe I am not understanding you, but are you saying I should not be prescribing the profile I gave in the previous post, but rather the analytical solution to the plane Poiseuille problem?

April 19, 2018, 11:58	Plane Poiseuille flow	#30
selig5576 Senior Member Selig Join Date: Jul 2016 Posts: 213 Rep Power: 10	So I'm using the analytical solution to plane Poiseuille flow $u_{1,j} = \frac{1}{2 \mu} \frac{dP}{dx} \left(y^{2} - h^2\right)$ , but my solution instantly diverges due to the pressure gradient in x.

April 19, 2018, 15:18	Bug	#32
selig5576 Senior Member Selig Join Date: Jul 2016 Posts: 213 Rep Power: 10	When determining dp/dx I read I should use the difference between the inflow and outflow pressure, is that correct? Otherwise I do not think there is a bug in my BC routine.

April 19, 2018, 15:45		#33
FMDenaro Senior Member Filippo Maria Denaro Join Date: Jul 2010 Posts: 6,773 Rep Power: 71	The velocity in a channel of height H for y=(-H/2:+H/2) is u(y) = -(6Q/H^3)(y^2-H^2/4) The parameter being Q=u_averageH. If you are using non-dimensional values you can just make non-dimensional the previous law selig5576 likes this.

April 20, 2018, 12:21		#35
FMDenaro Senior Member Filippo Maria Denaro Join Date: Jul 2010 Posts: 6,773 Rep Power: 71	The last figure seems a correct solution, what about the first one? Is it at the first time step and you set an inviscid initial condition?

April 20, 2018, 12:23	Poiseuille flow	#36
selig5576 Senior Member Selig Join Date: Jul 2016 Posts: 213 Rep Power: 10	Sorry I did not caption them . The first one is only after 150 time steps, so its quite immature in the development of the flow. EDIT: The pressure profiles seem to be consistent from what we would expect given the type of problem.

April 20, 2018, 12:35	Channel	#38
selig5576 Senior Member Selig Join Date: Jul 2016 Posts: 213 Rep Power: 10	Yes, I have done that and it converges to the fully developed flow within 2-5 iterations.

April 20, 2018, 12:41		#39
FMDenaro Senior Member Filippo Maria Denaro Join Date: Jul 2010 Posts: 6,773 Rep Power: 71	Ok, seems to be ok. selig5576 likes this.

April 24, 2018, 13:28	3D Situation	#40
selig5576 Senior Member Selig Join Date: Jul 2016 Posts: 213 Rep Power: 10	Returning back to my 3D solver. Here is my situation: If I have no outflow boundary conditions and run a lid driven cavity problem, my code returns the correct solution. As soon as I implement outflow boundary conditions (even a 1 x 1 x sized domain with 32^3 points) my pressure solver diverges. Interesting thing I've noticed is if I remove the advection term, my pressure solver does not diverge. Since I had validated my advection scheme on the LDC, I do not believe my discretization is wrong. I think the criminal is my pressure solver. There are only 5 pressure BCs with outflows conditions. The the outlet in x at the normal and the 4 corner pressure BCs at the outlet. Example: $R_{nx-1,2,2} = \frac{\rho}{dt}\left(\frac{vf^{}_{nx-1,2,2} - v^{n+1}_{nx-1,2,2}}{dx} + \frac{wf^{}_{nx-1,2,2} - w^{n+1}_{nx-1,2,1}}{dz}\right)$ $P_{nx-1,2,2} = (1-\omega)P_{nx-1,2,2} + \frac{\omega}{1/dy^2 + 1/dz^2}\left(\frac{1}{dy^{2}}P_{nx-1,3,2} + \frac{1}{dz^{2}}P_{nx-1,2,3} - R_{nx-1,2,2}\right)$ I prescribe this at as well. Mathematically, I believe the outlet BC is causing continuity at the faces to be violated, thus causing my PPE to diverge. Though the role of advection in causing this is currently confusing me. This divergence of pressure happens at around 480 SOR iterations. I am also using a plug inlet.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Wind turbine simulation	Saturn	CFX	58	July 3, 2020 01:13
Multiphase flow - incorrect velocity on inlet	Mike_Tom	CFX	6	September 29, 2016 01:27
Wrong flow in ratating domain problem	Sanyo	CFX	17	August 15, 2015 06:20
Question about heat transfer coefficient setting for CFX	Anna Tian	CFX	1	June 16, 2013 06:28
Error finding variable "THERMX"	sunilpatil	CFX	8	April 26, 2013 07:00