[diggee]

Hello. I am trying to reproduce an article's results where a DNS simulation of flow in a gradually expanding pipe is done. This (http://imgur.com/wIe5AmD) is the domain. d = 1cm.

After nearly ten days, I have 7 seconds of the solution. But the fluid has yet not completely passed through the entire outlet pipe even once (since it is so long). I know that it doesn't make sense to compute numerical quantities (friction factor, velocity fluctuations etc) if the flow field has not been solved in the entire domain even once. But I have to compare some numerical quantity to validate my simulation. Is there anything at all that I can compare with a partial solution?


If it matters, I am using ANSYS Fluent.

[lcarasik]

Originally Posted by diggee

Hello. I am trying to reproduce an article's results where a DNS simulation of flow in a gradually expanding pipe is done. This (http://imgur.com/wIe5AmD) is the domain. d = 1cm.

After nearly ten days, I have 7 seconds of the solution. But the fluid has yet not completely passed through the entire outlet pipe even once (since it is so long). I know that it doesn't make sense to compute numerical quantities (friction factor, velocity fluctuations etc) if the flow field has not been solved in the entire domain even once. But I have to compare some numerical quantity to validate my simulation. Is there anything at all that I can compare with a partial solution?


If it matters, I am using ANSYS Fluent.

I don't think you will have anything meaningful to compare at this point. How did you initialize it? Did you start from a laminar solution and perpetuate the system?

[FMDenaro]

Originally Posted by diggee

Hello. I am trying to reproduce an article's results where a DNS simulation of flow in a gradually expanding pipe is done. This (http://imgur.com/wIe5AmD) is the domain. d = 1cm.

After nearly ten days, I have 7 seconds of the solution. But the fluid has yet not completely passed through the entire outlet pipe even once (since it is so long). I know that it doesn't make sense to compute numerical quantities (friction factor, velocity fluctuations etc) if the flow field has not been solved in the entire domain even once. But I have to compare some numerical quantity to validate my simulation. Is there anything at all that I can compare with a partial solution?


If it matters, I am using ANSYS Fluent.

No, you can't. Then, even when you get a developed flow you still need to run the solution further to sample the field for the statistics.
I suggest to control the time evolution of the total kinetic energy and wait until it oscillates around an average value.

[flotus1]

If it took 10 days to compute less than 1 flow-through time, there is really no point in continuing with this simulation as is.
You should very carefully examine every aspect of the setup of your simulation to see if you can save computational costs and/or get much more computing power.

[diggee]

Originally Posted by lcarasik

I don't think you will have anything meaningful to compare at this point. How did you initialize it? Did you start from a laminar solution and perpetuate the system?

No, I did not start form a laminar solution. Even if I wanted to, I don't think it is possible in this case as turbulence is triggered in this due to the divergence of the pipe. So residuals would have never converged for a steady laminar case.

I initialized it from the inlet conditions. So pretty much everything in the rest of the domain (where the flow has not reached) is garbage data right now.

[diggee]

Originally Posted by FMDenaro

No, you can't. Then, even when you get a developed flow you still need to run the solution further to sample the field for the statistics.
I suggest to control the time evolution of the total kinetic energy and wait until it oscillates around an average value.

Yes, this is what the author has plotted along with vorticity, along the center line of the entire domain.

If you don't mind, could you please clear a doubt of mine? The author says that local turbulence (seen through vorticity along the center line)first travels downstream, stops for a brief moment, then travels upstream and then stops at a certain axial position and becomes spatially constant. But for me, it is only traveling downstream. It should've started traveling upstream around 4s and reached final position around 6s. So will the behavior, as reported by the author, only happen when the fluid completely passes once or there is something with my solution so far?

[diggee]

Originally Posted by flotus1

If it took 10 days to compute less than 1 flow-through time, there is really no point in continuing with this simulation as is.
You should very carefully examine every aspect of the setup of your simulation to see if you can save computational costs and/or get much more computing power.

Yes, I have stopped simulating it now cos it would take a month for the fluid to pass through just once. Moreover, I would then have to make a DNS worthy mesh throughout the entire domain which is computationally impractical here, given the resources I have at my disposal.

The author reports advection of turbulence in his article which is basically what I wanted to reproduce. But I am not getting his trend/ pattern. I have asked about this to in my reply to FMDenaro. Would you happen to have an idea regarding that?

[FMDenaro]

Originally Posted by diggee

Yes, this is what the author has plotted along with vorticity, along the center line of the entire domain.

If you don't mind, could you please clear a doubt of mine? The author says that local turbulence (seen through vorticity along the center line)first travels downstream, stops for a brief moment, then travels upstream and then stops at a certain axial position and becomes spatially constant. But for me, it is only traveling downstream. It should've started traveling upstream around 4s and reached final position around 6s. So will the behavior, as reported by the author, only happen when the fluid completely passes once or there is something with my solution so far?

I haven't read the paper describing this problem. However, let me say that is not clear to me a "local turbulence" that travels... I can imagine mass, momentum and energy as transported variables that travel along the pipe. You can consider the kinetic energy also. But from what you wrote, I suppose you have a compressible code, right?

[LuckyTran]

Just avoid statistics, especially the low frequency stuff. These problems with localized turbulence generally usually have small length scales that decay rapidly so that they're quickly decorrelated. Most of the flow simply gets advected downstream anyway so you don't need to worry about a sort of demon sitting downstream that is firing bad turbulence upstream. Just make sure there is enough flow-time for the inlet to arrive at the location you are interested.

Usually it is pretty easy to tell in 2D plots where the actual usable result is and where the garbage is or if you get a result and also very easy to tell in your spectra. It's even easier if you're reproducing something someone else has done before (i.e. you can compare your result to a known solution).

Long problems are a pain. =( I've also been waiting over a month for a problem.

[lcarasik]

Originally Posted by LuckyTran

Just avoid statistics, especially the low frequency stuff. These problems with localized turbulence generally usually have small length scales that decay rapidly so that they're quickly decorrelated. Most of the flow simply gets advected downstream anyway so you don't need to worry about a sort of demon sitting downstream that is firing bad turbulence upstream. Just make sure there is enough flow-time for the inlet to arrive at the location you are interested.

Usually it is pretty easy to tell in 2D plots where the actual usable result is and where the garbage is or if you get a result and also very easy to tell in your spectra. It's even easier if you're reproducing something someone else has done before (i.e. you can compare your result to a known solution).

Long problems are a pain. =( I've also been waiting over a month for a problem.

If you are doing DNS or LES, you absolutely can not ignore statistics. You need the statistics to create an appropriate time averaging of your quantities (after reaching a well defined turbulent state).

Based off what the topic creator has told us, they have not even reached a fully turbulent state nor checked to see if the simulation is experiencing turbulence. Anything they try and compare at this point is invalid.

[FMDenaro]

yes, I agree, statistics are the only way to assess the quality of the DNS/LES solution...but maybe LuckyTran was considering the fact that during the numerical transient stastistics are not necessary.

However, can we know the number of grid points used for the simulation? and the formulation?

[diggee]

Originally Posted by LuckyTran

Just avoid statistics, especially the low frequency stuff. These problems with localized turbulence generally usually have small length scales that decay rapidly so that they're quickly decorrelated. Most of the flow simply gets advected downstream anyway so you don't need to worry about a sort of demon sitting downstream that is firing bad turbulence upstream. Just make sure there is enough flow-time for the inlet to arrive at the location you are interested.

Usually it is pretty easy to tell in 2D plots where the actual usable result is and where the garbage is or if you get a result and also very easy to tell in your spectra. It's even easier if you're reproducing something someone else has done before (i.e. you can compare your result to a known solution).

Long problems are a pain. =( I've also been waiting over a month for a problem.

This is EXACTLY what my prof said, word for word. He was like since the pipe is so long, the solution way downstream wont matter too much anyway. As long as it passes through the region of interest (the gradual divergence in my case) , you can compare local quantities for that region. Problem is, the author of the article doesn't give much numerical data for comparison concerning only that region but rather the entire outlet (Cf, for example) after the flow field has been solved for the entire domain.

There is just one graph wherein he plots the spatio temporal advection of stream wise vorticity along the pipe. If my simulation is correct, I should be able to get his advection trend (or similar) in the region of interest as long as I solve for that much time (flow to pass through the divergence) at least, right? I am desperately counting on this

[diggee]

Originally Posted by lcarasik

If you are doing DNS or LES, you absolutely can not ignore statistics. You need the statistics to create an appropriate time averaging of your quantities (after reaching a well defined turbulent state).

Based off what the topic creator has told us, they have not even reached a fully turbulent state nor checked to see if the simulation is experiencing turbulence. Anything they try and compare at this point is invalid.

The statistics are not important (I think) if one wants to compare local quantities that have been evaluated for the region of interest. I should have mentioned earlier that I only want to compare a 2D spatio temporal plot of stream wise vorticity along the pipe centerline. For such a thing, statistics don't play a role, I guess.

The flow never reaches a fully turbulent regime. Due to external perturbation+geometry, transitional flow is triggered but it is spatially localized. Further downstream, it is the usual laminar paraboloid flow field. For the time that I have simulated so far, transition has been triggered but not solved so much that the entire domain is solved.

[diggee]

Originally Posted by FMDenaro

yes, I agree, statistics are the only way to assess the quality of the DNS/LES solution...but maybe LuckyTran was considering the fact that during the numerical transient stastistics are not necessary.

However, can we know the number of grid points used for the simulation? and the formulation?

Total mesh volumes is around 11 million. It is so less cos I have made a DNS worthy mesh only in the region wherein the author reports the turbulence patch gets localized. I don't exactly know what you mean by formulation, but I am only solving the usual transient, incompressible, laminar case in Fluent but with a Kolmogorov time step and very fine mesh.

[FMDenaro]

diggee,
I do not agree with you, many of your assumptions are not based on a real assessment...I don't know what paper are you following and I cannot judge that. But for sure, you are going to study onlu a numerical transient, without any physical meaning.
To be more specific, what you would do is the simulation of the physical transient in which the flow starts from the rest and develop as in an experimentla device. To do that you should consider many unknown parameters. Just an example: are you setting a real time-dependent physically correlated inflow velocity?

[diggee]

Originally Posted by FMDenaro

diggee,
I do not agree with you, many of your assumptions are not based on a real assessment...I don't know what paper are you following and I cannot judge that. But for sure, you are going to study onlu a numerical transient, without any physical meaning.
To be more specific, what you would do is the simulation of the physical transient in which the flow starts from the rest and develop as in an experimentla device. To do that you should consider many unknown parameters. Just an example: are you setting a real time-dependent physically correlated inflow velocity?

Yes, that is what I am simulating. The spatio temporal graph that I want to compare to is for the entire time period (from t = 0) showing the spatio temporal advection of stream wise vorticity. As for the velocity profile, I am using a UDF to give a paraboloid inlet just like the author has done in the article, and just like it would be in an experiment for a long inlet pipe. I am failing to understand why is this an issue?

As for the physical meaning, the spatio temporal variation of stream wise vorticity depicts the location of the localized turbulent patch with time. Could you please tell me what assumptions of mine are you referring to?

[FMDenaro]

Originally Posted by diggee

As for the velocity profile, I am using a UDF to give a paraboloid inlet just like the author has done in the article, and just like it would be in an experiment for a long inlet pipe

Not at all ... the Re_x value for a long pipe says you get a turbulent profile that, in a DNS formulation, means you have to set a 3D unsteady inflow

[lcarasik]

Originally Posted by diggee

The statistics are not important (I think) if one wants to compare local quantities that have been evaluated for the region of interest. I should have mentioned earlier that I only want to compare a 2D spatio temporal plot of stream wise vorticity along the pipe centerline. For such a thing, statistics don't play a role, I guess.

The flow never reaches a fully turbulent regime. Due to external perturbation+geometry, transitional flow is triggered but it is spatially localized. Further downstream, it is the usual laminar paraboloid flow field. For the time that I have simulated so far, transition has been triggered but not solved so much that the entire domain is solved.

1. That's likely not DNS. You have to resolve all of the scales to call it DNS.
2. Anything you use at this point in your simulation is likely numerical junk that isn't physically meaningful. You need to flush out the numerical junk (several flow through times) to have anything meaningful to compare to, even for transition flow.

[LuckyTran]

Guys I think you are not used to the problem.

This isn't like a simulation of a globally turbulent flow where you perturb an initial solution with garbage noise and pray that that it develops into your turbulent flow. You have some inflow, all the "turbulence" is generated in the expansion. It is still DNS because just need to resolve all the scales in the expansion. You might not want to call it turbulence but just flow instabilities. Also because this isn't a fully turbulent flow, the smallest scales tend to be very large.

It is a spatially localized problem. For example a turbulent jet embedded in a huge freestream. Only the flow in the vicinity of the jet is turbulent, it's inviscid everywhere else.

My point is that the flow from the inlet advects downstream and undergoes or experiences the unstable flow in the expansion. Navier-Stokes may be spatially elliptic but it's still dominated by advection (remember the boundary layer equations are parabolic). Hence, you should be able to see reasonable results even though you don't have a complete flow-thru time as long as you can at least march with the flow from the inlet. You can add a little factor of safety and require double this flow-time or triple if you want. If you cannot do this marching, then you definitely need more simulation time.

You can always run the simulation longer. But for looking at an initial result, I think there can be something learned and the most important features of the flow should already be present. You can even learn a lot during this numerical transient.

Originally Posted by diggee

If you don't mind, could you please clear a doubt of mine? The author says that local turbulence (seen through vorticity along the center line)first travels downstream, stops for a brief moment, then travels upstream and then stops at a certain axial position and becomes spatially constant.

Keep watching for this and see if it pops up later. If it never shows up, then you have to wonder about why you do not get the same result. If it shows up later... that gives you a hint that it's cause by elliptic properties (downstream effects propagating upstream) and not purely do to the parabolic effect (i.e. something happens upstream and simple gets washed downstream).

Right now you are able to observe the birth of the phenomena if it exists. Once you get the flow-thru time established, it will be difficult to just stop it. You'll only be able to see this phenomenon as a development on an already existing flow feature. And maybe that is what it is.

When these features show up can tell you a lot of things. Now if they never show up, then you are maybe in trouble. =)

[FMDenaro]

I do not agree....why? Think a similar flow, the backward facing step with a small height. If you set a laminar profile the onset of turbulence from the expansion will be different from that you would have with a real turbulent profile. The stress at the wall is different. The reattachment lenght will be different. And having a laminar profile after a long pipe is not physically reasonable.
Therefore, you are right when you consider the flow trasport properties advected (apart from the elliptic behavior of pressure) downstream but, to simulate accurately the transient, you have to prescribe a correlated profile. The only way to do an accurate representation of this problem is to have an upward pipe sufficiently long to let the laminar profile develop in a turbulent profile before the expansion. This way you can predict the local onset of the turbulence from the expansion. Furthermore, the vorticity field advected from the inflow in the centerline is strongly affected by the assumption of a laminar profile.