CFD Online Discussion Forums - How many boundary conditions do we need for the pressure?

Page 4 of 5

Show 40 post(s) from this thread on one page

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)

- Main CFD Forum (https://www.cfd-online.com/Forums/main/)

- - How many boundary conditions do we need for the pressure? (https://www.cfd-online.com/Forums/main/245524-how-many-boundary-conditions-do-we-need-pressure.html)

FMDenaro

August 31, 2023 03:02

Quote:

Originally Posted by Winston Virtaus (Post 856140)

I was able to get hopefully some better divergence error estimate numbers by monitoring directly the divergence of the mac-like face velocities during runtime. However, I havent yet switched to the APM procedure which would be the more correct choice.

The solver was tried on a 3D channel flow @ Retau = 395 to see if it produced any different behaviour to the backward facing step case.

In the channel flow case the maximum divergence error is around O(1e-7) and its located roughly in the buffer layer region. Usually third cell from the wall.

In the backward facing step case the maximum divergence is now around O(1e-5) and its located far in the downstream where the grid is stretched in the stream-wise direction. Usually second or third cell near the wall.

Any comments on these values now? Is the incompressibility constraint satisfied atleast somewhat acceptably?

Compare these values to the magnitude of your local truncation error.
I suggest also to check if a grid refinement reduces these values.

Winston Virtaus

September 1, 2023 22:47

I'm still working on how the divergence error scales on different grids but I thought I'd ask a quick question about the local truncation error you mentioned.

In the Analysis of the local truncation error in the pressure-free projection method for incompressible flows: a new accurate expression of the intermediate boundary conditions paper its mentioned that the splitting error of the pressure free method can be estimated as
efs = deltaT*[grad(phi)-grap(p)]-deltaT^2/2Re*div(grad(grad(p)) + O(deltaT^3) (equation 24).

If first order implicit Euler is used for the diffusion term in the v* equation, does this then imply that I'm getting only the first order approximation of p i.e. grad(phi) = grad(p)? And if this is indeed the case, would the equation 24 splitting error reduce to efs = -deltaT^2/2Re*div(grad(grad(phi))). Of which the local truncation error part is LTE = efs/deltaT?

FMDenaro

September 2, 2023 03:47

Quote:

Originally Posted by Winston Virtaus (Post 856255)

Using an implicit scheme for the diffusive term would produce always the presence of the diffusive-like term in the error. You can simply check what happens for the implicit Euler scheme by following the procedure in my paper: in the CN scheme cancel the part at time tn and in the part at tn+1 use 1 instead of (1/2).
The expression you get will be quite similar, the only difference is that since you use a first order accurate method, it makes no sense consider higher order terms in the efs.

Winston Virtaus

September 4, 2023 23:50

Following similar analysis for the Implicit Euler as the Crank-Nicholson show in the paper, this was the result:

efs = deltaT*(grad(phi)-grad(p)) - 1/(2*Re)*deltaT^2*div(grad(grad(p))= 1/(2*Re)*deltaT^2*div(grad(grad(phi))) + O(deltaT^3)

leading to error proportional to O(deltaT^2). Is this correct now?

It seems that the Crank-Nicholson option would exactly cancel this leading term.

I hope the procedure was followed properly now :)

FMDenaro

September 5, 2023 04:31

Quote:

Originally Posted by Winston Virtaus (Post 856343)

To confirm your result I should repeat all the procedure for the implicit Euler, but I see a coefficient 1/(2*Re), why? The implicit Euler should produce only 1/Re.

Winston Virtaus

September 5, 2023 21:02

I think it was due to some calculation error in the higher order terms.

However I could do a lower order approximation to the splitting error as

$\textbf{e}_{fs} = \textbf{v}^{n+1}-(\textbf{v}^{*n+1}-\textbf{v}') = \textbf{v}^{n}+\Delta t\frac{\partial \textbf{v}}{\partial t}|^n - \textbf{v}^{*n}-\Delta t\frac{\partial \textbf{v}^*}{\partial t}|^n+\Delta t \nabla \langle \phi \rangle^{n+1}\hspace{1cm}(1)$

which can be further reduced into

$\textbf{e}_{fs} = \Delta t(\textbf{R}^n+\textbf{P}^n)-\Delta t\textbf{R}^{*n}+\Delta t\nabla \langle \phi \rangle^{n+1}= \Delta t [\nabla \langle \phi \rangle^{n+1}+\textbf{P}^n]$ $= \Delta t[\nabla\langle\phi\rangle^{n+1}-\nabla\langle p\rangle^{n+1}]\hspace{1cm}(2)$

assuming

$\textbf{v}^n = \textbf{v}^{*n}, \textbf{R}^{*n} = \textbf{R}^n\hspace{1cm}(3)$

but I'm not exactly sure if the above assumption is correct.

Then using

$(I-\frac{\Delta t}{Re}\nabla^2)\nabla\langle\phi\rangle^{n+1}=\nabla\langle p' \rangle ^{n+1}\hspace{1cm}(4)$

the resulting split error would be

$\textbf{e}_{fs} =\frac{\Delta t}{Re}\nabla^2\nabla\langle \phi \rangle^{n+1}\hspace{1cm}(5)$

Any thoughts? :D

FMDenaro

September 6, 2023 04:02

Quote:

Originally Posted by Winston Virtaus (Post 856429)

In my paper I distinguish the case of the continuous formulation from that of the discrete one (but only for the AB/CN scheme). Following the discrete approach, the implicit Euler scheme should introduce the first order error, according to what you get.

Winston Virtaus

September 6, 2023 23:09

Thanks for the confirmation!

The paper is indeed very comprehensive and rigorous. The time-discrete analysis was abit harder to follow due to the inverse operator so thats why I followed the continuous analysis.

Its going to be interesting to see what kind of splitting error numbers I get when the error relation is postprocessed. The relation seems rather cheap to compute, is it customary to keep tracking it during runtime too?

FMDenaro

September 7, 2023 04:08

Quote:

Originally Posted by Winston Virtaus (Post 856482)

You should consider Eq.(26) as general infos for the discrete equations. In case of the implicit Euler equation, I would expect the splitting error in the form dt*O(LTE)= O(dt^2).
But it is not customary to keep a trace of that during a run.
The aim of the paper is to provide the framework and show the congruent accuracy order of the BCs for the intermediate velocity.

Winston Virtaus

September 7, 2023 22:34

Thanks! I'll take a look. :)

Winston Virtaus

September 23, 2023 17:30

3 Attachment(s)

I did some more testing on the boundary conditions in a simpler test case to which a closed form solution is available:

Poisseule flow between infinite parallel plates at Re≈26.6

Peak flow velocity of 1 m/s
Pressure gradient of 1 m/s2
Mesh resolution was 16x16x16.
Timestep roughly 1e-3 seconds.

Boundary conditions

Dirichlet for physical velocity
Taylor series based BCs for intermediate velocity
Neumann conditions for pressure

I decided to calculate the actual error from the analytical solution. The correct APM formula is also used for face velocities.

Is the divergence error now low enough compared to the velocity and pressure gradient errors?

FMDenaro

September 23, 2023 17:41

Quote:

Originally Posted by Winston Virtaus (Post 857390)

I did some more testing on the boundary conditions in a simpler test case to which a closed form solution is available:

Poisseule flow between infinite parallel plates at Re≈26.6

Peak flow velocity of 1 m/s
Pressure gradient of 1 m/s2
Mesh resolution was 16x16x16.
Timestep roughly 1e-3 seconds.

Boundary conditions

Dirichlet for physical velocity
Taylor series based BCs for intermediate velocity
Neumann conditions for pressure

I suppose you have the height of 1m, the magnitude of the error seems quite congruent for a second order scheme. However, I would suggest to check further the BC at the inflow, there (and at the two corners), it appears some peaks. Since you are prescribing Dirichlet conditions both at inflow and outflow, I see a different distribution of the errors.

Winston Virtaus

September 23, 2023 23:08

Quote:

Originally Posted by FMDenaro (Post 857391)

Yes quite close, channel height was 0.2m :)

So ideally i should expect a similar error pattern near both inlet and outlet?

Its very well possible that there are still inconsistencies in the boundary conditions.

Ogbency001

September 24, 2023 22:46

Enquiry: CFD Modeling of Bio-pesticide Sprayer Optimization for Agricultural Applicat

I want to achieve the following objectives and need your guide Develop a simplified CFD model to simulate the bio-pesticide
sprayer application process.

Analyze the spray pattern and droplet behaviour using the CFD
model.

Optimize the sprayer design and operational parameters to
enhance spray coverage and droplet size distribution.

Validate the CFD model by comparing the simulated spray
characteristics with available experimental data or previous
studies

Question1: Which solver in OpenFoam is best for this ?
Question 2: I have learn many tutorial and know how to do simulation based on the tutotial but can not find any on pesticide sprayer; what should I do

Winston Virtaus

September 25, 2023 23:27

Quote:

Originally Posted by Ogbency001 (Post 857427)

Most likely an VOF-based solver like interFoam would be the way to go.

These guys had some nice results with that solver: https://www.youtube.com/watch?v=jUOQwt6lWS8

Winston Virtaus

October 8, 2023 13:15

3 Attachment(s)

It seems that the source of the error has something to do with the second derivative of pressure.

This time the inlet and outlet physical velocity boundary conditions are constructed via low order upwinding/downwinding and the normal velocity component is altered to achieve the target flowrate which leads to the situation where both the normal gradient of physical velocity and second derivative of pressure basically vanish. As result, something interesting happens to the errors:

Maximum error of pressure is reduced almost by a factor of 10. Its now also almost uniform throughout the domain.
The velocity divergence is lower and more uniform with symmetric but opposite errors in inlet and outlet region
Velocity error is basically uniform in the streamwise direction and changes in the wall normal direction fairly smoothly.

Currently I'm resetting the velocity at the boundary to its physical value after each time-step, so the 3rd derivative of pressure is not taken into account at the boundary.

I'm thinking the Poisson solver part is working properly, but the intermediate velocity step could need some tweaking to help cancel out the third derivative of pressure at the APM step.

FMDenaro

October 8, 2023 13:51

Now seems working better, as further check you can see if the divergence error depends on a grid refinement as should be for the APM.

Winston Virtaus

October 9, 2023 22:33

2 Attachment(s)

Thanks for the input! :)

Two different tests were performed to see the divergence error scaling:

In the first plot mesh size was fixed to 0.04 m and timestep was changed from roughly Co=1 to Co=0.01

On the second plot timestep was fixed to Co=0.6 and mesh size was instead changed. The mesh size was reduced from about 0.1 m to about 0.01 m by splitting the mesh equally in all directions between runs.

All plots are on a double logarithmic scale.

It looks like there is still some inconsistency in the code.

FMDenaro

October 10, 2023 03:52

Quote:

Originally Posted by Winston Virtaus (Post 858088)

Thanks for the input! :)

Two different tests were performed to see the divergence error scaling:

In the first plot mesh size was fixed to 0.04 m and timestep was changed from roughly Co=1 to Co=0.01

On the second plot timestep was fixed to Co=0.6 and mesh size was instead changed. The mesh size was reduced from about 0.1 m to about 0.01 m by splitting the mesh equally in all directions between runs.

All plots are on a double logarithmic scale.

It looks like there is still some inconsistency in the code.

You should do the test at constant dt/h ratio, that could solve your issue.

hunt_mat

October 10, 2023 09:27

Quote:

Originally Posted by kinematic_presser (Post 837274)

Hello guys,
I am still somewhat new to CFD (just starting my masters degree) so please bear with me if my question is dumb.

I am simulating fluid flow in a channel for an assignment. The aim of the assignment is to simulate 2 dimensional incompressible Poiseulle flow, moving from left to right. It is a very simple simulation. There are no obstacles and it is a simple rectangular domain. For the velocity, I enforce a velocity inlet condition at the inlet and a homogeneous Neumann condition at the outlet. I enforce a homogeneous Dirichlet condition (no-slip) at the top and bottom wall. This all makes sense to me as the INSE are second order in u .

But, when I was looking over some example tutorial cases in OpenFOAM, I noticed that their simulations were enforcing a boundary condition for the pressure on both the inlet AND the outlet, and correspondingly, on both the bottom AND the top wall. They typically used a homogeneous Neumann condition on the top and the bottom wall, a homogeneous Neumann condition on the inlet, and a Dirichlet condition on the outlet.

This does not make sense to me from a mathematical point of view, because the INSE are first order in p in both the x and y coordinate, so specifying boundary conditions at only, for example, the bottom and left wall should already be enough to fully specify the solution.

I know that the INSE are invariant under constant pressure shifts p --> p+p0 which gives the system a little extra freedom. I also know that typically the pressure is simulated using the pressure Poisson equation, which is of course second order. But this is a consequence of the INSE, not a governing equation in its own right.

I would appreciate some elucidation on this topic. Thanks.

It is possible to obtain a Poisson equation for the pressure, so that means you need boundary conditions for all your boundaries.

All times are GMT -4. The time now is 01:53.

Page 4 of 5

« First

Show 40 post(s) from this thread on one page