[waseeqsiddiqui]

I have simulated an internal flow in a diverging nozzle. The inlet condition is pressure inlet while outlet is mass flow inlet. The simulation smoothly converges in 400 to 600 iterations in a Pressure Velocity Coupled Setup.
As observed, the total guage pressure specified in the inlet becomes area weighted static pressure while the total temperature at inlet and outlet almost remains the same specified magnitude.
Why does the outlet total pressure calculated is higher than that of inlet?

[waseeqsiddiqui]

Anyone. ?

[RaiderDoctor]

Not saying I know what your solution is, but can you give us more info on your problem? You talk about how the pressure at the inlet becomes the area-weighted static pressure, and then you discuss temperatures at the inlet and the outlet. However, your question has to do with the total pressure calculated at the outlet is greater than that of the inlet? What does that have to do with anything you just described to us?


On a more basic note, have you considered that the reason the pressure is greater at the outlet is due to Bernoulli's?

If your pipe is diverging, it would makes sense if the pressure was greater at the outlet. To check this, look at your velocity and ensure that it is greater at the inlet, rather than the outlet.

[waseeqsiddiqui]

Thankyou for your response RaiderDr!

I had tried different lengths of diverging nozzles and simulated them in ANSYS FLUENT. My problem setup is to calculate the velocity, temperatures and the pressures at the outlet given the total pressure, mass flow rate and total temperature at the inlet in a compressible pipe flow problem.

Case 1: Whenever I use the conditions Pressure Inlet and Mass Flow Rate Inlet, I get myself a slightly higher total pressure at the outlet but lower velocity. ALSO the specified total pressure at inlet becomes static pressure at inlet for some reason. It converges really fast.
Case 2: If I simulate the same mesh using pressure inlet and mass flow outlet, my output total pressure is calculated less than inlet. Convergence is way difficult to achieve.

It is interesting for Bernoulli phenomena to occur. Thanks for mentioning. I'll research about it. But why does the 2nd case shows lower total pressure given the same conditions?

Sorry for late reply.

[LuckyTran]

Originally Posted by waseeqsiddiqui

Case 1: Whenever I use the conditions Pressure Inlet and Mass Flow Rate Inlet, I get myself a slightly higher total pressure at the outlet but lower velocity. ALSO the specified total pressure at inlet becomes static pressure at inlet for some reason. It converges really fast.
Case 2: If I simulate the same mesh using pressure inlet and mass flow outlet, my output total pressure is calculated less than inlet. Convergence is way difficult to achieve.

Case1. You can't have a pressure inlet and a mass flow rate inlet. It's one or the other. So you are lying about something... And what is your outlet BC? Pressure outlet? For pressure inlet you specify the inlet total pressure and it should not become the static pressure unless you misinterpret something. As a sanity check, initialize the case, do not run any iterations and check the inlet total pressure to confirm it matches the boundary condition. What do you mean becomes? If you use a massflow rate inlet then you don't specify anything about the total pressure and it's free to be whatever it needs to be.
Case 2. Lower outlet total pressure makes sense if you run any viscous model. Convergence will be a bit harder here compared to fixed boundary conditions because it is a pressure outlet with the pressure adjusted every few iterations to achieve your desired mass flow rate.


Also, you can just plot the entire total pressure field and quickly determine the areas where it is increasing or decreasing to find any errors.

[RaiderDoctor]

Okay waseeqsiddiqui, let's break this down a little bit.
Thank you very much for the bit of background information on your setup, but you need to go deeper. At the very least, post a pic of your mesh, diagrams, etc. Is it transient, steady-state, what models are you using? You don't have to describe this all to us, but it would be beneficial for you to at least post a pic of your setup. Simply giving us one sentence describing your setup is not sufficient. So you have a diverging nozzle: what is the inlet pressure? Outlet pressure? What do you expect to happen?

Case 1: As it's written right now, I have to agree with Lucky. You can't have a pressure and mass inlet at the same time. I'm assuming you meant to say that when you try a pressure inlet and a mass flow inlet, you are getting similar results. Again, what velocity/pressures are you expecting to get? Where do these values come from (calculation or empirical?). Can you trust them? You also keep talking about the total pressure becoming static pressure. For your reference, total pressure (as defined by the Fluent manual) for a compressible fluid is:

where:

= total pressure
= static pressure
= Mach number
= ratio of specific heats ()

Keep in mind that this is with respect to the operating pressure.

You are saying that the convergence behavior of case 1 is better than case 2. Honestly, it really doesn't matter which converges faster at this point. If the simulation isn't right, it can have the best convergence behavior in history, but it's still a wrong simulation.

I'm a little confused as to how you are performing case 2. You began by saying you are trying to find the velocity at the outlet. If you are trying to find this value, then how are you able to input a mass flow outlet? If it's having difficulty converging, it might be due to the fact that continuity can't be conserved under the conditions you've set (read what Lucky wrote, then read it again). Again, though, this is just speculation, as I don't know your setup.

I gotta tell you, dude, it's a little concerning to me that you're working with fluids but you didn't consider the Bernoulli effect. If I were you, I would run a hand-calculation before I even touched a computer to get a rough idea of what's going on in my fluid domain. Then, after I've got some values, I'd run the simulation to get better quantities. Remember, Fluent is an extremely powerful tool, but it's not just a cure-all. If you plug-in inappropriate values, you will get garbage results.

I agree with Lucky, you need to plot the overall contour for pressure for you fluid domain to determine if it makes sense. To add to that, consider going through this tutorial (https://confluence.cornell.edu/displ...ow+in+a+Nozzle) which is freely available.

[waseeqsiddiqui]

Thank you for you responses. I will now elaborate my situation. It is a pressure based coupled steady state solver using kw SST and y plus less than 1. The values used for total, static pressure inlet, total temperature, mass flow rate were all taken from a wing body at a certain altitude and mach number using compressible flow calculations and Raymer Charts.
In both cases I have viscosity set to Sutherland. My density is ideal gas. It is a simple pipe with a single entry and exit. Operating Pressure is set to Zero and walls are at no slip condition.

In Case 1;
I have used pressure inlet in inlet while outlet is specified as mass flow inlet. The pressure inlet specified has entries for total pressure, supersonic gauge and total temperature. I have specified the static pressure at the supersonic gauge pressure field while total pressure and total temperature in there respective fields. The exit is specified mass flow inlet and has the fields for supersonic gauge pressure, mass flow rate and total temperature. Here I have specified the same total Temperature as inlet and the mass flow rate for the pipe flow. I have left supersonic gauge pressure field empty.

Observation Case 1: At initialization, the Area-weighted intlet total pressure is as was specified in the inlet. Static Pressure at inlet is the one specified in supersonic gauge pressure The simulation converges real fast by 400 iterations and the residuals go down sharply. Only the warning message of ''reverse flow occurs in # faces'' repeatedly occurs in every iteration.
The resultant mach inlet is much higher than exit. For example, if I have 180 m/s in entry, exit is around 50 m/s. Outlet total pressure is a bit higher, like 30K Pa while inlet is 27K Pa. Static Pressure is less at Inlet as it should be. But its value is the one I specified for total pressure at inlet. Why is that?

In Case 2;
Pressure Inlet is specified at inlet. Mass Flow rate Outlet is specified at exit.

Observation Case 2: Convergence is very hard to achieve. But when achieved, all seems right as expected from theoretical calculations. Total pressure should decrease a bit due to flow seperation phenomena.
Is there a better way to find outlet pressures and velocities?

I will check the pressure distribution see what goes wrong. Nice Idea.
Also I have not ignored bernoulli and whatever I expect I get it right except the total pressure which it cant predict.

[RaiderDoctor]

Unfortunately waseeqsiddiqui, this is where pictures would be extremely beneficial. If you can't due to certain restrictions, I understand, but at least tell us this straight away or make up some crude images using PowerPoint. The main reason is before you were explaining to us that you were working with a diverging nozzle, and now you say you are working with a simple pipe. I can assume that it's still technically a nozzle, but this kind of visual information would have been beneficial earlier on.

Saying that your viscosity and density are set to Sutherland and the ideal gas law isn't really saying much. This is describing a behavior, not necessarily how the fluid acts. Imagine if I told you I was working with a liquid, and I have my viscosity set to Newtonian. Based off of this, you have no way of knowing the fluid's resistance to shear, only that its linear. This is neither here nor there, it just might be beneficial for future readers who are working on a similar project but, in this context, I don't think it matters.

So, for case 1 you have two inlets? I cannot stress this enough, you need to check your results for case 1. Observe the velocity vectors, and ensure that they are oriented in the correct direction. I highly doubt it, however, as the warning message you received is consistent when either an inlet or an outlet experiences flow in the opposite direction that it is prescribed (i.e. an inlet has flow leaving the domain and an outlet has flow entering it). In this instance, that would most likely be the pressure inlet, which is the first part of that warning message I'm assuming.

I really don't understand what you mean by your last sentence in observation case 1: how can static pressure be less at the inlet, but the same as the total pressure? I think there might be a typo here.

In observation case 2, it makes sense why convergence would be difficult to achieve. Look what Lucky said in the post above as to why convergence is difficult here. Again, you mention that total pressure decreases, but fail to specify where. And the bit about pressure decreasing due to flow separation? Are you sure about that? Typically, flow separation occurs when an adverse pressure gradient forms due to lower velocity caused by an expanding channel (conservation of mass). I could be wrong, but the pressure typically increases in a diverging channel, not decreases.

As to your last question; maybe, but we don't know how you are finding the outlet pressures and velocities currently.
When you say that you will check pressure distributions and the like, it is a very good practice to check your results qualitatively before checking them quantitatively. That way, you can at least know immediately if there are any unnatural flow conditions that should not be present in your simulation, that may have some effect on your data.

[waseeqsiddiqui]

Something with the forum is not allowing me to upload picture via cfd forum android app. (error; this forum has disabled media sharing) Anyways, I get it I am not a good explainer.

It is a straight pipe with greater cross sectional area on outlet thn inlet. So I call it a diverging nozzle. Sorry for confusing.

So I checked and my outlet has negative mass flow rate which means flow is exiting the domain. (inlet has positive)
Velocity vectors exit thru outlet of the domain aka mass flow inlet.

I did mention above that Static Pressure was found higher than inlet. Which Should happen. Because of Bernoulli Conservation of Energy. But why does the Total Pressure increases?

I have viewed the cornell link you had sent. It is very good. They have used pressure inlet and pressure outlet. In my case, I cannot use pressure outlet as I don't know the outlet static pressure.

[waseeqsiddiqui]

As a summary, I would request answer to this Major Question.

How would you perform CFD simulation of compressible internal flows if you have all these variables (all pressures, temperatures, mach) in inlet But you don't know any of these in exit?

[LuckyTran]

First you said you had a diverging nozzle. Now you say you have a simple pipe? I'm assuming the pipe was a lie and you actually have a diverging nozzle.

I see now that you are using a massflow inlet at an outlet and flipping the massflow around.

At a pressure inlet, there is an input for total pressure and supersonic / initial static pressure. During initialization, if you use compute from and choose this inlet, it takes takes the value you specified in the static pressure here (which is why it is labeled super sonic / initial static pressure). After any calculation is done, if the inlet is not supersonic, the supersonic static pressure is completely ignored and only the total pressure is used (that's why most people never put any number into this box, it doesn't do anything). At 100 m/s, you're probably subsonic.

Case 1 converges very quickly because you've basically forced a velocity at the outlet and superconstrained the flow. You've also constrained the velocity to be uniform and purely normal to the boundary.

Case 2 converges slower because it's taking time (iterations) to figure out what the outlet pressure needs to be to get the mass flow rate that you targeted. Meanwhile the velocity at this boundary is whatever arrives at the boundary, is 3D, points in somewhat arbitrary (and sometimes might even be reversed). There are much more degrees of freedom here compared to case 1.

Originally Posted by waseeqsiddiqui

As a summary, I would request answer to this Major Question.

How would you perform CFD simulation of compressible internal flows if you have all these variables (all pressures, temperatures, mach) in inlet But you don't know any of these in exit?

In general you don't. You need boundary conditions and you're missing these at the outlet. You do not even have a problem definition at this point. It's like saying I want to do CFD of something, but I know not what that something is. The only time you can do CFD without knowing anything at the outlet is when you have a supersonic outlet.

Reality works the same way. Try to fix all the properties at the inlet of a pipe. You don't have any magical devices that creates a bubble universe that supplies flow at exactly a certain pressure and temperature and flow rate.

Mach number is not a boundary condition (there is no Mach number in the Navier-Stokes equation). The boundary conditions you want are going to be total pressure, total temperature, and mass flow rate. If you need to, calculate the mass flow rate using the Mach number using your smartphone or whatever. You can do this calculation because you know what the geometry is! That is, you know the cross-sectional areas of the inlet.

You need a downstream boundary condition (unless the outlet is supersonic). Use a pressure outlet with targeted mass flow rate option if you are subsonic. If you are supersonic you can put anything there.

If your inlet is supersonic. You still don't specify the Mach number directly. You indirectly specify the Mach number by specifying the static pressure and total pressure.

[waseeqsiddiqui]

Originally Posted by LuckyTran

First you said you had a diverging nozzle. Now you say you have a simple pipe? I'm assuming the pipe was a lie and you actually have a diverging nozzle.

I see now that you are using a massflow inlet at an outlet and flipping the massflow around.

At a pressure inlet, there is an input for total pressure and supersonic / initial static pressure. During initialization, if you use compute from and choose this inlet, it takes takes the value you specified in the static pressure here (which is it is labeled super sonic / initial static pressure). After any calculation is done, if the inlet is not supersonic, the supersonic static pressure is completely ignored and only the total pressure is used (that's why most people never put any number into this box, it doesn't do anything). At 100 m/s, you're probably subsonic.

Case 1 converges very quickly because you've basically forced a velocity at the outlet and superconstrained the flow. You've also constrained the velocity to be uniform and purely normal to the boundary.

Case 2 converges slower because it's taking time (iterations) to figure out what the outlet pressure needs to be to get the mass flow rate that you targeted. Meanwhile the velocity at this boundary is whatever arrives at the boundary, is 3D, points in somewhat arbitrary (and sometimes might even be reversed). There are much more degrees of freedom here compared to case 1.



In general you don't. You need boundary conditions and you're missing these at the outlet. You do not even have a problem definition at this point. It's like saying I want to do CFD of something, but I know not what that something is. The only time you can do CFD without knowing anything at the outlet is when you have a supersonic outlet.

Reality works the same way. Try to fix all the properties at the inlet of a pipe. You don't have any magical devices that creates a bubble universe that supplies flow at exactly a certain pressure and temperature and flow rate.

Mach number is not a boundary condition (there is no Mach number in the Navier-Stokes equation). The boundary conditions you want are going to be total pressure, total temperature, and mass flow rate. If you need to, calculate the mass flow rate using the Mach number using your smartphone or whatever. You can do this calculation because you know what the geometry is! That is, you know the cross-sectional areas of the inlet.

You need a downstream boundary condition (unless the outlet is supersonic). Use a pressure outlet with targeted mass flow rate option if you are subsonic. If you are supersonic you can put anything there.

If your inlet is supersonic. You still don't specify the Mach number directly. You indirectly specify the Mach number but specifying the static pressure and total pressure.

Thankyou. Appreciate your response.