[arjun]

Originally Posted by sbaffini

I am looking, right now, at the Prof. J.Y. Murthy ME608 Notes at Purdue, which has a nice 1D example with Rhie-Chow interpolation at the beginning of chapter 7 and, honestly, I still don't see how RC could produce such solution...

This is because the Rhie and Chow term is something like (pf1 - pf0) * df . Where pf1 and pf0 are interpolated pressure at face from right and left cells. When the solution is smooth the pf1 matches pf0 and this term vanishes. If it does not vanish it becomes part of the flux.

The convergence then only depends on finding some pressure profile that even though produces non zero rhie and chow term , satisfies Sum(fluxes) = 0. Pressure gradient is then just another source term to momentum equation.

In theory rhie and chow term should converge to zero. This in practice does not happen specially in unstructured meshes.

[FMDenaro]

Originally Posted by sbaffini

I am looking, right now, at the Prof. J.Y. Murthy ME608 Notes at Purdue, which has a nice 1D example with Rhie-Chow interpolation at the beginning of chapter 7 and, honestly, I still don't see how RC could produce such solution...

EDIT: Let me say it better and more clearly. Fluent is giving converged residuals and mass imbalance distribution at 1e-17, yet the corresponding solution has div(u) = -1, which is in contrast, to the best of my understanding, to the RC alteration of the continuity equation, which should be order dx^3 (around 1e-7 here) times the 4th order derivative of the pressure (which should be 0 for the solution I'm getting). This is, for Fluent, a fully legit solution of the test problem I've setup but, again, I don't see how this could be possible. I'm maybe wrong, but I see this as very confusing

Actually, the RC term should result like O(dt*h^2), isn't that?


However, I agree, the meaning of a "convergent" solution with a mass imbalance has only added confusion.

[FMDenaro]

Originally Posted by arjun

This is because the Rhie and Chow term is something like (pf1 - pf0) * df . Where pf1 and pf0 are interpolated pressure at face from right and left cells. When the solution is smooth the pf1 matches pf0 and this term vanishes. If it does not vanish it becomes part of the flux.

The convergence then only depends on finding some pressure profile that even though produces non zero rhie and chow term , satisfies Sum(fluxes) = 0. Pressure gradient is then just another source term to momentum equation.

In theory rhie and chow term should converge to zero. This in practice does not happen specially in unstructured meshes.

That does not answer to the fact that an increasing in div V must be balanced to an increasing (opposite sign) of the RC term. The two terms should indefinitely increase in time ...

[sbaffini]

Another update after another small test.

Took the base converged case and switched the inlet bc to mass flow inlet using the value reported from the monitors as value for the bc.

Residuals suddenly jumped to a constant value slightly below 1e-3 with no further evolution in anything else. The solution stayed exactly the same.

Then, I repeated the test starting from scratch and using mass flow inlet as inlet bc.

Now, everything correctly blows up.

Sounds like a bug in velocity inlet bc to me

If now OP could, at least, tell us what Fluent version he is using...

[FMDenaro]

Originally Posted by sbaffini

Another update after another small test.

Took the base converged case and switched the inlet bc to mass flow inlet using the value reported from the monitors as value for the bc.

Residuals suddenly jumped to a constant value slightly below 1e-3 with no further evolution in anything else. The solution stayed exactly the same.

Then, I repeated the test starting from scratch and using mass flow inlet as inlet bc.

Now, everything correctly blows up.

Sounds like a bug in velocity inlet bc to me

Just to simplify anything, are you considering a simple 2d channel with a closed wall?
Is the grid cartesian and structured ?

[sbaffini]

Originally Posted by FMDenaro

Just to simplify anything, are you considering a simple 2d channel with a closed wall?
Is the grid cartesian and structured ?

It's 1D, 128x1x1, inviscid. Honestly, I don't want to make another mesh for this

[sbaffini]

Another small update. SIMPLEC and PISO blow up, but the COUPLED pressure solver doesn't and has the same behavior and solution with both the BCs.

[arjun]

Originally Posted by FMDenaro

That does not answer to the fact that an increasing in div V must be balanced to an increasing (opposite sign) of the RC term. The two terms should indefinitely increase in time ...

Well no. Pressure correct equation corrects the pressure until sum(fluxes) = 0 is achieved. Once a balance is found it will stop correcting.

If there is an increase in velocity then it would be corrected by pressure correction to minimise sum of fluxes.

[arjun]

Originally Posted by sbaffini

Another small update. SIMPLEC and PISO blow up, but the COUPLED pressure solver doesn't and has the same behavior and solution with both the BCs.

Simplec might again converge with smaller urfs.

[CFDParty]

Originally Posted by sbaffini

Another update after another small test.

Took the base converged case and switched the inlet bc to mass flow inlet using the value reported from the monitors as value for the bc.

Residuals suddenly jumped to a constant value slightly below 1e-3 with no further evolution in anything else. The solution stayed exactly the same.

Then, I repeated the test starting from scratch and using mass flow inlet as inlet bc.

Now, everything correctly blows up.

Sounds like a bug in velocity inlet bc to me

If now OP could, at least, tell us what Fluent version he is using...

First of all, I want to apologize for replying this late to this tread, I was on travel over the long weekend. I see that I've started some frustrations here, so again very sorry for this.

These are the specifics to my case:
1. Fluent 2022 R2
2. The fluid density and viscosity is set to be constant
3. I'm using a pressure-based solver, SIMPLE sheme with Rhie-Chow distance based flux type, first order implicit transient formulation, Least squared cell for gradient, second order for pressure, and second order upwind for momentum.
4. I performed 40 time steps with dt=5e-5, with 100 iterations per time step.
5. The residuals for continuity, x-velocity and y-velocity are all set to default (0.001)

[FMDenaro]

Originally Posted by arjun

Well no. Pressure correct equation corrects the pressure until sum(fluxes) = 0 is achieved. Once a balance is found it will stop correcting.

If there is an increase in velocity then it would be corrected by pressure correction to minimise sum of fluxes.

But with a velocity inlet and no outlet, it must be an increasing in velocity gradient, not in the velocity...
That is, we know that, div V must increase, therefore the correction is always in.

[arjun]

Originally Posted by FMDenaro

But with a velocity inlet and no outlet, it must be an increasing in velocity gradient, not in the velocity...
That is, we know that, div V must increase, therefore the correction is always in.

Balanced by pressure ie rhie and chow. Thats only way there is stable solution.

[FMDenaro]

Originally Posted by arjun

Balanced by pressure ie rhie and chow. Thats only way there is stable solution.

Ok, let us assume such a mechanism is working. During the time integration each term will increase to ensure to balance the residual. This happens while having a mass imbalance.

But I expect that these terms will become so large in magnitude that at a certain point the run crashes ...

[sbaffini]

Originally Posted by CFDParty

I see that I've started some frustrations here

Hahahha... guilty as charged. Apologies as well from me for showing frustration

However, my suggestion is to try the mass flow inlet bc and see if you have similar results. My guess is that you won't. Also, in my opinion, this is a clear bug of the velocity inlet bc. I haven't tried every other combination of solver settings but, most of your options haven't shown any significant effect on the results of my base case.

[sbaffini]

Originally Posted by arjun

Simplec might again converge with smaller urfs.

For obvious reasons, I kept default values for all the tests, so I dind't attempt any change of method settings, only switched across methods.

[CFDParty]

Originally Posted by sbaffini

Hahahha... guilty as charged. Apologies as well from me for showing frustration

No worries, I really appreciate all the effort!

Originally Posted by sbaffini

However, my suggestion is to try the mass flow inlet bc and see if you have similar results. My guess is that you won't. Also, in my opinion, this is a clear bug of the velocity inlet bc. I haven't tried every other combination of solver settings but, most of your options haven't shown any significant effect on the results of my base case.

In the mean time I set the absolute criteria for continuity to 1e-05. Which has no trouble converging, also reported the mass flow rate at the inlet which is constant, no reversed flow is detected at the inlet.

Now just tried to change the inlet to mass flow inlet, where the solution again convergences without trouble

[sbaffini]

Originally Posted by CFDParty

No worries, I really appreciate all the effort!



In the mean time I set the absolute criteria for continuity to 1e-05. Which has no trouble converging, also reported the mass flow rate at the inlet which is constant, no reversed flow is detected at the inlet.

Now just tried to change the inlet to mass flow inlet, where the solution again convergences without trouble

Just for a check, I tried with SIMPLE and second order for pressure but I confirm the different behavior of the two inlet bcs. Velocity inlet gives a solution (and actually the pressure seems now to be exactly the Bernoulli solution with no error, except near the inlet), but mass flow inlet doesn't.

I don't know what else to say... just don't do that

[FMDenaro]

My final opinion: any kind of numerical solution that does not crash for such problem is rubbish.

In no way a CFD developer should accept that from his code.

[LuckyTran]

I didn't doubt that someone managed to run a Fluent case that "converged" without blowing up in finite time. But it should eventually blow up. And in my personal opinion this isn't a fault of poorly coded Fluent as I'm fairly confident you could repeat it in many other software as well. I don't think any CFD developer expects anyone to use their code to simulation a problem with no solution (known a priori).

In general, just don't do simulations like this. Benchmark against things that actually make sense. And if you must do it anyway, be prepared that it requires a more-than-surface-level understanding to interpret the results. The benefit of discussing it here in this particular user group is that we've experienced and encountered so many crazy things that it isn't crazy talk.

[arjun]

Originally Posted by LuckyTran

IBenchmark against things that actually make sense. And if you must do it anyway, be prepared that it requires a more-than-surface-level understanding to interpret the results.

This is very true.

As a person who writes CFD solvers, my aim is to provide a robust and stable solver but accuracy takes first place. That means stability NOT at the cost of accuracy.

Having said this, user shall be careful and should have good understanding of what he is solving and what is expected solution. He should know how to judge the solution.