[Syed Wajeeh]

Hello all.
I am simulating a supersonic bell nozzle spinning about its axis. The analysis is transient and I am having a confusion about selecting the right value of time step. I have read the courrant no. should be 1 or less than 1 and it requires maximum velocity and minimum mesh size to get the value of time step but I do not have the max velocity as it comes after the simulation gets completed and also I am confused whether I should use adaptive time stepping or not. Can anyone please guide me in this regard that how to go for the solution as it takes a lot of time for one simulation and divergence is highly un-desired with a given deadline. Thanks in advance to all.

[LuckyTran]

Run it with some initial guesses, you should be able to guess it within an order of magnitude. You've already stated that it is supersonic, which gives a Mach number > 1 so guess something reasonable. Run it and check your Courant number that you achieve and then adjust the time-step accordingly. Then rerun it with nice settings and get nice results.


If you must ask, then the answer is no: don't use adaptive time stepping. Adaptive time-stepping is not an excuse for you to turn your brain off and let the CFD run autonomously. Adaptive time stepping is for shaving computational cost after you've understood the problem. If you're still in the learning phase and wondering what your time-step size needs to be, then I don't recommend its use at all. Use robust methods. Adaptive time stepping is the surest way to miss your deadline.

[Syed Wajeeh]

Thanks a ton Lucky. It was really helpful. Stay Blessed <3

[sbaffini]

Out of curiosity, where the unsteadiness comes from?

[FMDenaro]

Originally Posted by Syed Wajeeh

Hello all.
I am simulating a supersonic bell nozzle spinning about its axis. The analysis is transient and I am having a confusion about selecting the right value of time step. I have read the courrant no. should be 1 or less than 1 and it requires maximum velocity and minimum mesh size to get the value of time step but I do not have the max velocity as it comes after the simulation gets completed and also I am confused whether I should use adaptive time stepping or not. Can anyone please guide me in this regard that how to go for the solution as it takes a lot of time for one simulation and divergence is highly un-desired with a given deadline. Thanks in advance to all.

Be also aware of the fact that the CFL condition is often defined in compressible flows by taking into account also the sound velocity, not only the convective velocity.

[Syed Wajeeh]

sbaffini, actually I was also a bit confused about this in the start when my supervisor told me. The only reason I can decipher up till now is that with wall rotation or frame motion, the flow does not rotate as the nozzle spins about its axis but with the mesh motion, the flow shows the rotation and mesh motion becomes enable only in the case of transient analysis. If you can guide me further in this regard, I will be very thankful to you :-)

[Syed Wajeeh]

FM, Can you please elaborate a bit further on what you have suggested ? I will be very thankful to you

[FMDenaro]

Originally Posted by Syed Wajeeh

FM, Can you please elaborate a bit further on what you have suggested ? I will be very thankful to you

It depends on the eigenvalues u+/-a for the pressure waves. For an example, have a look to page 457 in the Anderson textbook

[sbaffini]

Originally Posted by Syed Wajeeh

sbaffini, actually I was also a bit confused about this in the start when my supervisor told me. The only reason I can decipher up till now is that with wall rotation or frame motion, the flow does not rotate as the nozzle spins about its axis but with the mesh motion, the flow shows the rotation and mesh motion becomes enable only in the case of transient analysis. If you can guide me further in this regard, I will be very thankful to you :-)

It is difficult without further details. Do you plan using URANS or LES/DNS?

What software are you using?

Is your domain axisymmetric?

You mention 3 different things: frame motion, mesh motion and wall motion, which one are you going to use? If you will use mesh motion, it is correct that it only makes sense for unsteady cases, but the other 2 options also make sense in a steady framework, so the question is if the end result can be achieved only with mesh motion or not.

In general, an unsteady case is needed for at least one of two reasons: the boundary conditions (including the geometry as well) change in time or the system under study is such that unsteadiness emerges spontaneously (e.g., like vortex shedding). I would include LES/DNS studies under the latter case as well.

Now, I can't say anything about the second option for your case (because I don't know it), but if you plan using URANS you should ask: is there a reference frame where all my bc (including geometry) are steady? If it does exist, and you certainly aren't in the second option, you could indeed avoid the unsteady computation. You could even opt for a steady axisymmetric one.

But more details are needed to say something more concrete

[Syed Wajeeh]

Originally Posted by sbaffini

It is difficult without further details. Do you plan using URANS or LES/DNS?

What software are you using?

Is your domain axisymmetric?

You mention 3 different things: frame motion, mesh motion and wall motion, which one are you going to use? If you will use mesh motion, it is correct that it only makes sense for unsteady cases, but the other 2 options also make sense in a steady framework, so the question is if the end result can be achieved only with mesh motion or not.

In general, an unsteady case is needed for at least one of two reasons: the boundary conditions (including the geometry as well) change in time or the system under study is such that unsteadiness emerges spontaneously (e.g., like vortex shedding). I would include LES/DNS studies under the latter case as well.

Now, I can't say anything about the second option for your case (because I don't know it), but if you plan using URANS you should ask: is there a reference frame where all my bc (including geometry) are steady? If it does exist, and you certainly aren't in the second option, you could indeed avoid the unsteady computation. You could even opt for a steady axisymmetric one.

But more details are needed to say something more concrete

Thanks sbaffini. I am using turbulence modelling (k-w SST) in ANSYS Fluent. My nozzle is in 3-dimensions and of course symmetric about its axis of rotation. I have no BCs at all that change with time. I have a pressure inlet, pressure outlet, insulated walls and nozzle is spinning abt its axis at a constant angular velocity say 10 rad/s. I have initially tried with wall rotation and frame motion but the flow did not rotate as all the vectors and path lines were straight (instead of being curved). Then, with the mesh motion being used, the flow eventually got rotated and it was validated by the post processing as well. I am not performing LES or DNS in my case also.
Now, I you can guide me how to apply the steady simulation in my case then I would be highly obliged. Thanks in advance and waiting for a prompt reply

[Syed Wajeeh]

Originally Posted by syed wajeeh

thanks sbaffini. I am using turbulence modelling (k-w sst) in ansys fluent. My nozzle is in 3-dimensions and of course symmetric about its axis of rotation. I have no bcs at all that change with time. I have a pressure inlet, pressure outlet, insulated walls and nozzle is spinning abt its axis at a constant angular velocity say 10 rad/s. I have initially tried with wall rotation and frame motion but the flow did not rotate as all the vectors and path lines were straight (instead of being curved). Then, with the mesh motion being used, the flow eventually got rotated and it was validated by the post processing as well. I am not performing les or dns in my case also.
Now, i you can guide me how to apply the steady simulation in my case then i would be highly obliged. Thanks in advance and waiting for a prompt reply

Mesh Motion (1).jpg

Mesh Motion (2).jpg

Mesh Motion (3).jpg

Frame Moiton (1).JPG

Frame Moiton (2).JPG

[sbaffini]

Originally Posted by Syed Wajeeh

Thanks sbaffini. I am using turbulence modelling (k-w SST) in ANSYS Fluent. My nozzle is in 3-dimensions and of course symmetric about its axis of rotation. I have no BCs at all that change with time. I have a pressure inlet, pressure outlet, insulated walls and nozzle is spinning abt its axis at a constant angular velocity say 10 rad/s. I have initially tried with wall rotation and frame motion but the flow did not rotate as all the vectors and path lines were straight (instead of being curved). Then, with the mesh motion being used, the flow eventually got rotated and it was validated by the post processing as well. I am not performing LES or DNS in my case also.
Now, I you can guide me how to apply the steady simulation in my case then I would be highly obliged. Thanks in advance and waiting for a prompt reply

I think we need to separate, for a moment, your practical case with Fluent from the case you want to solve in theory.

I still don't know exactly what you want to achieve but it seems you want to just have the nozzle to rotate. Given the symmetries, the constant in time boundary conditions and the fact that you are using a RANS model, I think you can easily solve the problem as steady, even axysimmetric (which means 2D). What I mean here is that your conditions have this steady axisymmetric solution as the only relevant one.

To solve for the steady 3D case (will get to axisymmetry in a moment) you just need to set up a rotational velocity at the wall, just the one you actually have, nothing special. I would not, instead, set any frame motion because your original frame is already such that no geometry is moving in it (given the axisymmetry and the axis of rotation).

Now, this should just work in Fluent, and it is difficult to say what can be wrong in your case set-up. You mention using also a moving frame. This should not make any difference, provided the frame and the wall velocity are the same.

In addition to this, the case is equally doable with a 2D axisymmetric approach, which is 2D with some special equations. You just need to check Fluent manual for how to do this.

[LuckyTran]

Any arbitrary mesh motion should not cause the flow to change unless the boundaries are being deformed.

The influence of the moving wall boundary onto the flow is exactly the region we call the boundary layer. A spinning nozzle should not cause the velocity over the entire cross section to rotate, only the boundary layer should see any difference. Unless.... the entire cross section is a boundary layer.

Frame motion also does not cause anything to happen in the stationary lab frame. If I spin in my chair, the universe is not suddenly rotating, it's only my relative view of the universe that is spinning. So I need to be really careful how I interpret the things that I see while I am spinning.

I don't get how these pathlines are "validated" when they show a very non-physical result. Now I clearly see that these pics are from simulations that you simulated, but it certainly raises more doubts and asks more questions than it answers.

[FMDenaro]

But it is the case where "transient" means the initial stage of the rotation until a fully developed flows is reached?
Otherwise I can only think about the physical unsteadiness of the flow that can be captured only by DNS or LES.

[Syed Wajeeh]

Thanks once again sbaffini. I am getting some clear directions now. Will try to do all what you have mentioned.

[Syed Wajeeh]

Originally Posted by LuckyTran

Any arbitrary mesh motion should not cause the flow to change unless the boundaries are being deformed.

The influence of the moving wall boundary onto the flow is exactly the region we call the boundary layer. A spinning nozzle should not cause the velocity over the entire cross section to rotate, only the boundary layer should see any difference. Unless.... the entire cross section is a boundary layer.

Frame motion also does not cause anything to happen in the stationary lab frame. If I spin in my chair, the universe is not suddenly rotating, it's only my relative view of the universe that is spinning. So I need to be really careful how I interpret the things that I see while I am spinning.

I don't get how these pathlines are "validated" when they show a very non-physical result. Now I clearly see that these pics are from simulations that you simulated, but it certainly raises more doubts and asks more questions than it answers.

You are absolutely right Lucky. I am getting it now. So what you all are trying to suggest me is that I should perform steady analysis with wall rotations in ANSYS Fluent ? And only small changes will be in the BL region ?

[Syed Wajeeh]

Originally Posted by FMDenaro

But it is the case where "transient" means the initial stage of the rotation until a fully developed flows is reached?
Otherwise I can only think about the physical unsteadiness of the flow that can be captured only by DNS or LES.

FM Denaro sorry sir but I could not grasp what you are trying to suggest. Can you please elaborate it a bit so that I can get some more clear directions ?? Thanks in advance

[sbaffini]

Originally Posted by Syed Wajeeh

You are absolutely right Lucky. I am getting it now. So what you all are trying to suggest me is that I should perform steady analysis with wall rotations in ANSYS Fluent ? And only small changes will be in the BL region ?

If the flow enters not rotating (which seems to be your case) and Re is high enough (which should be your case, in order to actually use a RANS turbulence model) then, basically, yes.

The extent of the rotating part within the core of the flow wil grow with the axial coordinate (bigger at the outlet) and be a function of the Re, but I expect it to be relatively little, certainly not the whole section.

And yes, there seems to be no case here for anything unsteady in the end.

Let me also stress again that you can then also study this with axisymmetry, further reducing the simulation cost

[Syed Wajeeh]

Originally Posted by sbaffini

If the flow enters not rotating (which seems to be your case) and Re is high enough (which should be your case, in order to actually use a RANS turbulence model) then, basically, yes.

The extent of the rotating part within the core of the flow wil grow with the axial coordinate (bigger at the outlet) and be a function of the Re, but I expect it to be relatively little, certainly not the whole section.

And yes, there seems to be no case here for anything unsteady in the end.

Let me also stress again that you can then also study this with axisymmetry, further reducing the simulation cost

Thanks a lot dear. It was really helpful