[quarkz]

Hi,

I am now using 2nd order time and space discretization for my NS eqns, using fractional step.

For the boundary conditions, e.g. at the north side, I'm using:

du/dy = 0. v=0.

If I just use a 1st order discretization of the above for my problem, it will be:

u(i,j) = u(i,j-1)

will it affect the overall order of my problem? Will it become overall 1st order?

Thanks

[Rami]

AFAIK, using a 1st order BC in an otherwise 2nd order scheme will pollute the solution and renders it 1st order accurate. Sorry... Try to implement a 2nd order BC as well.

[cfdnewbie]

Yes, I agree with Rami. The overall solution will fall back to the lowest order in your domain, i.e. the boundary contribution. The becomes even more pronounced for high order schemes (>>2), where a low order boundary discretization can totally screw up your solution.

[quarkz]

Ok thanks for the answers. I'll ensure my BC are 2nd order too.

[arjun]

So if I understand this correctly, because BC is 1st order it does not make any difference if everywhere else is Second or higher order. The solution from first order scheme and second order schemes will be same??

I would say 1st order BC may affect that solution but it would NOT make the solution 1st order everywhere.

[Ford Prefect]

I agree with previous poster. It is problem dependent as well. For steady, incompressible, pipe flow the order of the outlet boundary condition should play little role.

1st order: u_b = u_b-1
2nd order: u_b = (4*u_b-1 - u_b-2)/3

If steady and incompressible then u_b-1 = u_b-2 (otherwise continuity is violated), and hence we see that the 2nd order boundary approximation is the same as the 1st order approximation.

For other cases (e.g. lid-driven cavity flow) the order of the boundary conditions is very important.

[cfdnewbie]

Originally Posted by arjun

So if I understand this correctly, because BC is 1st order it does not make any difference if everywhere else is Second or higher order. The solution from first order scheme and second order schemes will be same??

I would say 1st order BC may affect that solution but it would NOT make the solution 1st order everywhere.

The effect at the BC will perpetuate itself into the domain, so while not all cells will become first order accurate, the "bad cells" will drag your overall convergence down. This may or may not be a problem, depending on your requirements, but a single cell of lower order will destroy your theoretical order of convergence - if this matters in your case or not is something for you to decide.

If you are using codes with first or second order accuracy, the effects will not be as harmfull as if you are using high order schemes. Then, high order boundary approximation is crucial, for first and second oder you will get away with a lot more "approximation crimes"!

[cfdnewbie]

Originally Posted by Ford Prefect

I agree with previous poster. It is problem dependent as well. For steady, incompressible, pipe flow the order of the outlet boundary condition should play little role.

1st order: u_b = u_b-1
2nd order: u_b = (4*u_b-1 - u_b-2)/3

If steady and incompressible then u_b-1 = u_b-2 (otherwise continuity is violated), and hence we see that the 2nd order boundary approximation is the same as the 1st order approximation.

I am a little bit confused about your notation here: If your flow goes from left to right (so it leaves the domain at the right face), and b=0 would be the outflow face, then b=-1 and b=-2 would be the interior points...so your bc would be a (supersonic) extrapolation of u, which then would not be a BC in the sense that you are not feeding outer information in the flow (like at a wall), but just letting the flow develop in a natural way. So the argument might not be valid....

Or am i misunderstanding your example?

Cheers,
cfd newbie

[lalupp]

In unstructured mesh How do we implement second order BC du/dn = 0

[Ford Prefect]

Originally Posted by cfdnewbie

I am a little bit confused about your notation here: If your flow goes from left to right (so it leaves the domain at the right face), and b=0 would be the outflow face, then b=-1 and b=-2 would be the interior points...so your bc would be a (supersonic) extrapolation of u, which then would not be a BC in the sense that you are not feeding outer information in the flow (like at a wall), but just letting the flow develop in a natural way. So the argument might not be valid....

Or am i misunderstanding your example?

Cheers,
cfd newbie

I am just assuming zero gradient at the boundary for velocity and use one-sided differences for the derivative approximation.

[cfdnewbie]

Originally Posted by Ford Prefect

I am just assuming zero gradient at the boundary for velocity and use one-sided differences for the derivative approximation.

Allright, so what you are basically doing is an extrapolation form the inside, sth like a supersonic outflow, correct?

in that case, I'm wondering if the discussion about the order of the outflow bc is valid, since outflow bcs (the supersonic type) have no effect on the solution inside the domain, so yes, for such bcd, I guess order is not important.

I was thinking more about wall / inflow bcs in a flux-based scheme, where it has been shown e.g. by Bassi and Rebay that the effect of a low order bc (with a high order scheme) can be devastating.

Thanks for the nice discussion! Are you from the FD community?

[Ford Prefect]

Originally Posted by cfdnewbie

Allright, so what you are basically doing is an extrapolation form the inside, sth like a supersonic outflow, correct?

in that case, I'm wondering if the discussion about the order of the outflow bc is valid, since outflow bcs (the supersonic type) have no effect on the solution inside the domain, so yes, for such bcd, I guess order is not important.

I was thinking more about wall / inflow bcs in a flux-based scheme, where it has been shown e.g. by Bassi and Rebay that the effect of a low order bc (with a high order scheme) can be devastating.

Thanks for the nice discussion! Are you from the FD community?

Yes I agree, I just wanted to illustrate that order of the boundary condition approximation is not always important. However, I did not think of the boundary as a supersonic boundary. The pressure can be defined at the outlet boundary in a dirichlet way.

As for the original post I think it is best to try both 1st and 2nd order boundaries and then compare the results.

By FD, do you mean Fluid Dynamics? In that case, I would say not really. I do research in Metallurgy, using CFD (well these days it is mostly supervision) and I do some basic FD teaching to third year students. I do dabble in writing cfd codes in my spare time.

[morecfd]

Originally Posted by lalupp

In unstructured mesh How do we implement second order BC du/dn = 0

I have got the same question though I think we must delete the respective derivative terms
am i wrong?

[arjun]

Guys nobody is doubting that the order of scheme on boundary can affect the solution or quality of it.

But my comment was related to these two comments before mine:

Originally Posted by Rami

AFAIK, using a 1st order BC in an otherwise 2nd order scheme will pollute the solution and renders it 1st order accurate. Sorry... Try to implement a 2nd order BC as well.

Originally Posted by cfdnewbie

Yes, I agree with Rami. The overall solution will fall back to the lowest order in your domain, i.e. the boundary contribution. The becomes even more pronounced for high order schemes (>>2), where a low order boundary discretization can totally screw up your solution.

You see, these two things are wrong. While order of BC might affect the solution or might not affect the solution, over all order of solution will NOT fall back to 1st order. Saying categorically that it will fall to 1st order is plainly wrong.

Originally Posted by lalupp

In unstructured mesh How do we implement second order BC du/dn = 0

Usually it is first order. That is phi_bnd = phi_live (cell center for control volume ).

[cfdnewbie]

Originally Posted by arjun

You see, these two things are wrong. While order of BC might affect the solution or might not affect the solution, over all order of solution will NOT fall back to 1st order. Saying categorically that it will fall to 1st order is plainly wrong.

Hey Arjun,
let's debate this

The concept of an "order of a scheme" comes from the Taylor series expansion and is ONLY valid for h -> 0, i.e. in the limit of grid spacing going to zero. So even the most established scheme will only reach its design order of accuracy for "small" h, where h depends on the smoothness of the problem itself (and on the question whether the solution is indeed smooth or not!).

so let's agree that the term "order" only makes sense for h->0, right?

let's take a look at a flow field, where the solution is well-behaved and your second order scheme can treat it in a well-resolved manner, so let's assume the errors goes as h squared to zero. Let's further assume that you have ONE bad cell, where your order reduces to one, so your error goes as h (no squared here).
What's going to happen as h->0 ? Your one bad cell will dominate, and your order will gradually fall back to 1. ( This can be proven with mathematical consideration of convergence rates and series, but I think my example is sufficient. )

One great example of this is that at a shockwave (which can be interpreted as a first order phenomenon), all schemes either add an insane amount of viscosity or fall back to first order, no matter what.

Another example everbody who has ever done convergence testing can relate to is to prescribe an priori solution to the flow by the manufactured solution method (call it an elaborate convergence test if you will). One single "bad" cell in your domain will screw up your convergence rate, and you will NOT reach your design order of convergence.

And lastly, even if your "bad" cell might not drastically alter your computations visually, it might as well ruin things like cd / cl / cw, when you are not looking closely.

I encourage you to read Bassi and Rebays paper, which demonstrates the necessity of high order boundary discretizations quite dramatically!

http://web.mit.edu/ehliu/Public/Proj...M_2D_Euler.pdf

So, I'm looking forward to a lively discussion! Let's keep it coming!

Cheers!

[duri]

Second order BC is required for better accuracy at boundaries with gradients (eg. wall). With zero gradient second order and first order works alike. Practically, first order BC is sufficient enough for Euler solver but not for NS.

Originally Posted by cfdnewbie

The concept of an "order of a scheme" comes from the Taylor series expansion and is ONLY valid for h -> 0, i.e. in the limit of grid spacing going to zero. So even the most established scheme will only reach its design order of accuracy for "small" h, where h depends on the smoothness of the problem itself (and on the question whether the solution is indeed smooth or not!).

so let's agree that the term "order" only makes sense for h->0, right?

This is conflicting with h-methods and p-methods of FEM. In Taylor series h->0 means series gives exactly same value as continuous function on LHS. I wonder how order of accuracy is related to h->0.

Accuracy of an solution can be improved by two ways one increase the mesh size (h-method) (there is a limitation due to round off error, resource...) and next is to increase the order of equation (p -method). This is well proven, you can experiment yourself.
Solve a problem with second order accuracy with a coarse mesh and then solve same problem with first order accuracy with (atleast) 3-4 times refined mesh you may end up with same solution.

Order of scheme is from the truncation of Taylor's series and not on the h->0 assumption. What ever may be the value of h, if you only take the constant term it became first order and by including linear term it becomes second order.

Originally Posted by cfdnewbie

let's take a look at a flow field, where the solution is well-behaved and your second order scheme can treat it in a well-resolved manner, so let's assume the errors goes as h squared to zero. Let's further assume that you have ONE bad cell, where your order reduces to one, so your error goes as h (no squared here).
What's going to happen as h->0 ? Your one bad cell will dominate, and your order will gradually fall back to 1. ( This can be proven with mathematical consideration of convergence rates and series, but I think my example is sufficient. )

When there is a bad cell (eg. highly skewed) it will screw up the solution and will not fall back to first order. Even first order may get screwed up.

Originally Posted by cfdnewbie

One great example of this is that at a shockwave (which can be interpreted as a first order phenomenon), all schemes either add an insane amount of viscosity or fall back to first order, no matter what.

To my knowledge shockwave is not handle by any of the schemes (even Roe scheme). Shocks are handled only at the interface and within a cell, shock cannot be captured. This is because of weak solution approximation.
Whatever you said is an excellent example to prove first order in few cells will not make the entire domain first order. TVD schemes works this way, whenever it encounters shocks it locally makes the scheme to be first order to avoid spurious oscillations around the shock. Any scheme as such will not fall back to first order at discontinuities but limiter makes it to behave that way.

[cfdnewbie]

Originally Posted by duri

Order of scheme is from the truncation of Taylor's series and not on the h->0 assumption. .

The Taylor series expansion is only valid for h->0, that's in the definition of Taylor's expansion, is it not?

[cfdnewbie]

Originally Posted by duri

Practically, first order BC is sufficient enough for Euler solver but not for NS.

.

I beg to differ. A first order cylinder BC will produce spurious entropy at each kink, thereby generating a entropy wake behind the object, and destroy e.g. symmetry. NS on the other hand usually dampens this effect, and is it less pronounced.

This is conflicting with h-methods and p-methods of FEM. In Taylor series h->0 means series gives exactly same value as continuous function on LHS. I wonder how order of accuracy is related to h->0.

Order of accuracy is a mathematical concept, derived from a Taylor series, which is only valid for h->0. If you have a code at hand, try doing a convergence test, starting from a coarse grid. You will see that for a large h, you won't get any order of convergence at all.

Accuracy of an solution can be improved by two ways one increase the mesh size (h-method) (there is a limitation due to round off error, resource...) and next is to increase the order of equation (p -method). This is well proven, you can experiment yourself.

I'm not doubting that, in fact I agree with you. But "order of convergence" is a different concept than accuracy.

Solve a problem with second order accuracy with a coarse mesh and then solve same problem with first order accuracy with (atleast) 3-4 times refined mesh you may end up with same solution.

I agree. Try 16th order, and you will be done with one cell

Order of scheme is from the truncation of Taylor's series and not on the h->0 assumption. What ever may be the value of h, if you only take the constant term it became first order and by including linear term it becomes second order.

I disagree, please see my post above, as Taylor series is only valid for h->0.

When there is a bad cell (eg. highly skewed) it will screw up the solution and will not fall back to first order. Even first order may get screwed up.

Yes, it will fall back to a lower order, the question was not whether that was first order or order 1.5 or something, just a lower order.

To my knowledge shockwave is not handle by any of the schemes (even Roe scheme). Shocks are handled only at the interface and within a cell, shock cannot be captured. This is because of weak solution approximation.

Shocks can indeed by captured in a cell, given that the subcell resolution is high enough. I can e.g. capture a shock in a Burger's equation in 1 pseudospectral cell!

Whatever you said is an excellent example to prove first order in few cells will not make the entire domain first order.

Maybe I didn't make this point clear enough. Of course, the cells away from the shock will keep their second order quality, but the WHOLE solution will be less than second order. Do a convergence test with a shock in it, the shock itself is not sufficiently smooth, thus all codes will lose their order of convergence and fall back down to first order.

All I'm saying is that the overall behavior of your solution is governed by the lowest-order phenomenon - it doesn't matter if that comes from physics or numerics.

TVD schemes works this way, whenever it encounters shocks it locally makes the scheme to be first order to avoid spurious oscillations around the shock. Any scheme as such will not fall back to first order at discontinuities but limiter makes it to behave that way.

Allright, so your overall order will suffer because at the shock you are introducing an error of size O(1). That's what I'm trying to say all the time

(BTW, the reason some schemes have to resort to first order is because they wouldn't be stable otherwise. They just dump viscosity on the shock, until it can be resolved by low order methods)

Thanks for your input!

Cheers!

[arjun]

Originally Posted by cfdnewbie

Hey Arjun,
let's debate this

Whats there to debate. I already pointed out that saying that over all solution will fall back to lowest order is wrong. It should be obvious to anybody.

Originally Posted by cfdnewbie

let's take a look at a flow field, where the solution is well-behaved and your second order scheme can treat it in a well-resolved manner, so let's assume the errors goes as h squared to zero. Let's further assume that you have ONE bad cell, where your order reduces to one, so your error goes as h (no squared here).
What's going to happen as h->0 ? Your one bad cell will dominate, and your order will gradually fall back to 1. ( This can be proven with mathematical consideration of convergence rates and series, but I think my example is sufficient. )

Again the same thing. Now what happens that if this bad cell is the boundary cell and there is no change of flow. Further flow field does not mean that everything shall be happening only around that bad cell. In flow field flow has local nature which dominates. For example, if there are small eddies generated and if you are able to capture them correctly by *locally second order* schemes than it does not matter if your some cell in inlet boundary was bad and scheme there was first order.

To tell you the truth, in unstructured grid solvers like starccm+ and fluent schemes at BC are almost always first order. Now search for their presentations where they have investigated the flow comparison between first order and second order schemes. Why do you think their results differ?? May be the order BC did not play as important role as you making it to be.

I am not the only one to tell you this, there are others also who are saying the exact same thing to you in this thread.

Originally Posted by cfdnewbie

One great example of this is that at a shockwave (which can be interpreted as a first order phenomenon), all schemes either add an insane amount of viscosity or fall back to first order, no matter what.

Shockwave is poor example. Second viscosity is NOT added, but flow field due to error behaves as if the viscosity was little bit higher because of use of first order scheme there. Why not use second order scheme?? That is because in shockwave region gradients are very high and it would make solver unstable.

Further, the example with shockwave proves that just because locally first order scheme was used solution over all solution does not become first order. Rest of the place it would be second or higher order accurate.

Originally Posted by cfdnewbie

Another example everbody who has ever done convergence testing can relate to is to prescribe an priori solution to the flow by the manufactured solution method (call it an elaborate convergence test if you will). One single "bad" cell in your domain will screw up your convergence rate, and you will NOT reach your design order of convergence.

One poor cell can disturb the convergence but it is not due to the reason that that ONE CELL was first order accurate. In fact, first order scheme in full region will be 10 times more stable than 2nd order in full domain.

One poor cell can disturb convergence because it can screw up the condition number of matrix. In starCCM+ you can switch off such cell and still run simulation with 2nd order schemes in flow region.

Originally Posted by cfdnewbie

I encourage you to read Bassi and Rebays paper, which demonstrates the necessity of high order boundary discretizations quite dramatically!

http://web.mit.edu/ehliu/Public/Proj...M_2D_Euler.pdf

So, I'm looking forward to a lively discussion! Let's keep it coming!

Cheers!

We are not discussing whether second order schemes are needed or not. We are discussing this:

Originally Posted by cfdnewbie

Yes, I agree with Rami. The overall solution will fall back to the lowest order in your domain, i.e. the boundary contribution. The becomes even more pronounced for high order schemes (>>2), where a low order boundary discretization can totally screw up your solution.

[cfdnewbie]

Originally Posted by arjun

Whats there to debate. I already pointed out that saying that over all solution will fall back to lowest order is wrong. It should be obvious to anybody.

Well, you might have pointed that out, but I differ in my opinion. Maybe you didn't read my post carefully, friend. I AM agreeing with you that one cell will not affect each other cell in your domain, but a single bad cell with dominate the error convergence measured as an integral over the whole domain. The way you determine convergence for a scheme is usually NOT done by looking at single cells, but by integrating a suitable error norm (L2 usually) over the whole domain. So again, if you have 100000 smooth cells and one cell with an error of order lower than the rest, it will drag you down. simple as that.

Again the same thing. Now what happens that if this bad cell is the boundary cell and there is no change of flow.

again, this has been discussed in this thread already. Let's consider not the simplest of BCs (and by the way, if you have ever done direct acoustics, you will be aware that outflow bcs can be a great pain in the neck due to reflection), but the more instructive case of wall bcs!

Further flow field does not mean that everything shall be happening only around that bad cell. In flow field flow has local nature which dominates. For example, if there are small eddies generated and if you are able to capture them correctly by *locally second order* schemes than it does not matter if your some cell in inlet boundary was bad and scheme there was first order.

When you bring turbulence into play, it gets very dangerous. You should know that eddy generation and transport is highly sensitive to dispersion and dissipation errors, and thus almost all the basic turbulence is research is done with spectral codes.... think about why that is, and you will see how important sufficient order is for turbulence simulations.
And regarding your example:
If you are introducing an error of O(1) at your inflow bc, you will be sure to see the result in your eddies, unless you are doing some purely supersonic simulations.

To tell you the truth, in unstructured grid solvers like starccm+ and fluent schemes at BC are almost always first order. Now search for their presentations where they have investigated the flow comparison between first order and second order schemes. Why do you think their results differ?? May be the order BC did not play as important role as you making it to be.

Well, I would be happy if you could point me to these presentations, because I find those companies always very reluctant to show these types of comparisons.
Why don't you send me the presentations, I will take a look and you will read up the paper I proposed, and we talk some more? I must admit I tend to trust papers in peer-reviewed journal a tiny bit more than colorful marketing brochures...don't you as well

I am not the only one to tell you this, there are others also who are saying the exact same thing to you in this thread.

so we have a lively discussion going, from which we can all learn. That's great, that's what is missing in this forum way too often! Let's start educating each other...btw, you haven't replied to my remark about h->0!

Shockwave is poor example. Second viscosity is NOT added, but flow field due to error behaves as if the viscosity was little bit higher because of use of first order scheme there. Why not use second order scheme?? That is because in shockwave region gradients are very high and it would make solver unstable.

Viscosity is added for any type of shock capturing like TVD. And btw, you have two ways of doing SC: Add manually enough viscosity to keep your scheme (2nd, 4th, 16th) order stable by smoothing the gradient or use the most dissipative scheme (FOU) to do that for you. Amounts to the same thing.

But you didn't understand my example. A shock wave is a natural "first order BC", because the solution loses its smoothness there, and you will see the same behavior in the convergence as for a faulty first order bc. Sorry to confuse you, I shouldn't have brought it up!

Further, the example with shockwave proves that just because locally first order scheme was used solution over all solution does not become first order. Rest of the place it would be second or higher order accurate.

Yes, again, nobody is doubting that. But do the math, calculate the L2 norm, refine your mesh, compute your EOC, and you will come up with sth LESS THAN 2.

One poor cell can disturb the convergence but it is not due to the reason that that ONE CELL was first order accurate.

Oh yes, it is. Please think carefully again about what I said!

In fact, first order scheme in full region will be 10 times more stable than 2nd order in full domain.

Maybe true, but what does stability have to do with order of convergence?????

One poor cell can disturb convergence because it can screw up the condition number of matrix. In starCCM+ you can switch off such cell and still run simulation with 2nd order schemes in flow region.

I'm very very very confused now. Are you talking about the convergence of your matrix inverter for implicit time stepping??

If that's the case, that would explain a lot of the confusion going on here, friend

Cheers a lot!