Temperature mixing up in wrong velocity field

Gert-Jan · October 19, 2022, 12:04

Hi All,

I have a steady state setup with translation. Several objects move with a conveyor belt in a moving frame of reference, through multiple chambers that are in a stationary frame. In one chamber, the air is heated.

My problem is that I have two veloctity fields: a velocity relative to stationary frame and just velocity. This is the relative velocity, relative to either stationary or moving frame.

Now I expect my temperature to mix up in the velocity in stationary frame, meaning that in the moving frame, the hot air is moving with the obtsacles. But this is not the case. It is moving in opposite direction.

So, the temperature is mixed in the wrong velocity field. Does anyone know a magic button to get realistic results? To let Fluent perform mixing in Velocity in Stationary Frame?

I know the answer is transient. But a steady state, i.e. photo, should also be possible, not? Moreover, it would be a very good method to obtain an intiial guess for a transient anaylsis. If I would take my curent end-result as initial guess for a transient anaylsis, I would be far off.

And for your information: in CFX, I notice the same problem.
And forgive me the coarse mesh etc. It is just a simple test to find the correct settings.

Regs, Gert-Jan

Gert-Jan · October 20, 2022, 02:59

I added three picture fom a topview, making the problem of the phenomena clearer.

LoGaL · October 20, 2022, 15:43

I really do not get the problem, it's a bit hard from your description.

I presume the things are moving towards left? If yes, it makes sense that in a refrerence of frame attached to the things, you see moving air towards the right. Also, what do you mean by temperature mixing in the relative frame of reference?!

Just keep in mind you most likely spent some time in your project, so for you things seem very clear, but for somebody trying to understand you, it's nigh impossible

Gert-Jan · October 20, 2022, 18:28

(That is not so nice. Let me simplify the description and acts as if I have little experience in CFD.)

I have a simulation with obstacles on a conveyor belt that is moving through different chambers. The obstacles and belt are placed in a moving domain and move to te left. The chambers are in a stationary domain.

Since the belt and the obstacles move to the left, I expect the air to move to the left. This is what I see in my picture with the Velocity in Stn Frame. This is correct.

Now I turn on a heater in one of the chambers. I expect the hot air to be dragged with the obstacles to the left. But it moves to the right. Why?

LoGaL · October 21, 2022, 02:53

Ah now I see. Yes I agree with you, there is that sort of hot air slipping to the right.

Is this simulation converged by any means? I would be surprised if it was so, it should be unsteady by nature. If it is not converged at all, which is what I expect, you shouldn’t worry about that hot flare. Actually, if you were to run it a bit more, again supposing it didn’t converge, maybe it would be slipping less, or more, or from the other side

Can i see the residuals? As I said, if it SO unsteady like your case, there’s no trick to do with the steady solver

Gert-Jan · October 21, 2022, 05:33

Certainly it is converged. In residuals and in mass and energy imbalance. Moreover, I monitor values at serval points to see how they develop.

The problem is that I perform a steady state calculation. There we see that scalars and temperature mix up in the vector variable "Velocity". In steady state, this variable is equal to

Velocity i = Velocity in Stn Frame i - Frame Speed i

In the Frame with chambers, the Frame Speed i = 0 since the chambers are standing still. So

Velocity i = Velocity in Stn Frame i - 0 = Velocity in Stn Frame i

In my moving part, I have a constant Frame Speed to the left. Since this is larger than the local Velocity in Stn Frame, the local Variable Velocity component becomes negative, i.e. to the right. Therefore my hot air is going to the right. Same happens in CFX. This is standard procedure when working with rotating or moving frames. You end up with Velocity in Stn Frame and Velocities in Relative Frames. The latter is called Velocity.

The main problem is that I perform a steady state calculation. If I would do a transient analysis, then the moving frame is going to the left, bringing the hot air to the left, step by step. But I do not want to go to transient. My conveyor belt is huge. I would calculate for months. Also because there is no good initial guess. Normally this would be a steady state calculation, i.e. my result above. But then my hot air is in the wrong location, i.e. the worst initial guess I can imagine.

Therefore I want to go a steady state. But then I need to find a trick to tell Fluent (or CFX) to mix my temperature (and scalars) in Variable "Velocity in Stn Frame" instead of default "Velocity".

LoGaL · October 21, 2022, 05:54

Forgive me, but I do not see how a case like this admits a steady solution if the obstacles are moving inside the chambers. It is not physically possible. It is periodic, so with steady statistics, but not steady flow.

I highly doubt fluent found a steady solution and, if it did, it's wrong. I can also tell that it didn't converge because the domain is symmetric, and your (RANS?) Temperature contour is not. This is again unphysical. There's no magic trick, if the physics is unsteady by nature, you need to go transient. Also to get the steady statistics, you need to run transient and do the average.

On the other side, I would be surprised if it had to calculate for months...Depends a bit on the computational resources you have. You may even try to reduce the problem to 2D symmetric( so computationally cheaper) and run transient. In this way you neglect the obstacles height and assume them infinitely tall, but it is way more reasonable than trying to get a steady solution in 3D and flogging a dead horse.

Gert-Jan · October 21, 2022, 06:32

I am looking for a transient averaged solution. I.e. a photo shot of a conveyor belt in motion. In principle this could be a steady state CFD-solution, if the temperature and scalars would mix up in the Stationay velocity field.

I fully agree that a steady state CFD-solution is unrealistic. The interaction between obstacles and walls between the chambers certianly have a transient nature. But with a conveyor belt with 100 obstacles and 20 chambers, a steady state solution as a start would be wonderfull. Even as a rough estimation, it would be very welcome. Now I have nothing, other than run fully transient with a miserable initial guess.

Without a few tricks from a magic box, it looks quite hopeless to be honest.
While looking for some help on this forum, I am also waiting for ANSYS to come up with a decent answer.
Fingers crossed.

Gert-Jan · October 21, 2022, 06:50

The reason I am looking for a photo of a certain flow situation is that I'm interested in the time averaged condition in each chamber/the machine as a whole. I'm not really interested in the obstacles. They vary from day to day anyway.

LoGaL · October 21, 2022, 08:05

I see your point, but

1) it won't get any better than this, there are no tricks. You can't get the average picture with this setup. If you still want to try a steady simulation, perhaps have a look at mixing planes. This might be what you are looking for, but i am not sure. They are used in turbomachinery
2) The initial guess is not that bad, it won't take months
3) I firmly believe you should work to simplify your problem in a physically sound way. First step is to simulate half the domain and impose a symmetry boundary condition. Then you can also consider 2D, unless you really care about the effect of the obstacle height

Gert-Jan · October 21, 2022, 11:39

1) I can get a better initial guess if Fluent or CFX allows me to mix the scalars and temperature in the Velocity in Stn Frame.
2) If the hot air has accumlated at the right hand side of my steady state, and then has to travel to the left hand side of my equipment in a transient analysis, I will need several resisdence times, espcially if I the mixing in every chamber is included. That is very inefficient.
3) Probably you are right. I will consider this.

LoGaL · October 21, 2022, 11:48

Look at mixing planes. They might be what you are looking for. They are alrdy implemented in Fluent.

Gert-Jan · October 27, 2022, 03:33

I tried mixing planes in CFX on a geometry look-a-like. You can find the results here:

Hot air is moving in the wrong direction

Mixing plane is averaging the results over the whole interface, leading to high temperature on both left and right hand side. In fact, it assumes the whole interface is connected from left to right, as if it is a periodic part of a cilinder.

LoGaL · October 27, 2022, 05:45

As i suspected, it is not what you are looking for :/. They do exactly what you are asking, but for turbines (cylinders)

Maybe smebody else has an idea for your problem. In the meantime, I would really simplify to a symmetric domain. And try to also do it 2D. I think it may be fast enough.

October 21, 2022, 06:32		#8
Gert-Jan Senior Member Gert-Jan Join Date: Oct 2012 Location: Europe Posts: 1,835 Rep Power: 27	I am looking for a transient averaged solution. I.e. a photo shot of a conveyor belt in motion. In principle this could be a steady state CFD-solution, if the temperature and scalars would mix up in the Stationay velocity field. I fully agree that a steady state CFD-solution is unrealistic. The interaction between obstacles and walls between the chambers certianly have a transient nature. But with a conveyor belt with 100 obstacles and 20 chambers, a steady state solution as a start would be wonderfull. Even as a rough estimation, it would be very welcome. Now I have nothing, other than run fully transient with a miserable initial guess. Without a few tricks from a magic box, it looks quite hopeless to be honest. While looking for some help on this forum, I am also waiting for ANSYS to come up with a decent answer. Fingers crossed. Last edited by Gert-Jan; October 21, 2022 at 07:43.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Initial pressure field from velocity field (incompressible)	dhein	STAR-CCM+	3	January 18, 2022 08:12
potential flows, helmholtz decomposition and other stuffs	pigna	Main CFD Forum	1	October 26, 2017 08:34
velocity field of MRF, GGI and rotatingWallVelocity	tonky	OpenFOAM Programming & Development	1	October 14, 2016 11:04
how to customize the initial velocity and temperature field?	gdtiaozi	FLOW-3D	1	December 3, 2013 07:13
where is the calculation of the temperature field	Tobi	OpenFOAM	1	July 30, 2012 10:40

October 20, 2022, 15:43		#3
LoGaL Senior Member Lorenzo Galieti Join Date: Mar 2018 Posts: 374 Rep Power: 12	I really do not get the problem, it's a bit hard from your description. I presume the things are moving towards left? If yes, it makes sense that in a refrerence of frame attached to the things, you see moving air towards the right. Also, what do you mean by temperature mixing in the relative frame of reference?! Just keep in mind you most likely spent some time in your project, so for you things seem very clear, but for somebody trying to understand you, it's nigh impossible

October 21, 2022, 02:53		#5
LoGaL Senior Member Lorenzo Galieti Join Date: Mar 2018 Posts: 374 Rep Power: 12	Ah now I see. Yes I agree with you, there is that sort of hot air slipping to the right. Is this simulation converged by any means? I would be surprised if it was so, it should be unsteady by nature. If it is not converged at all, which is what I expect, you shouldn’t worry about that hot flare. Actually, if you were to run it a bit more, again supposing it didn’t converge, maybe it would be slipping less, or more, or from the other side Can i see the residuals? As I said, if it SO unsteady like your case, there’s no trick to do with the steady solver

October 21, 2022, 05:33		#6
Gert-Jan Senior Member Gert-Jan Join Date: Oct 2012 Location: Europe Posts: 1,835 Rep Power: 27	Certainly it is converged. In residuals and in mass and energy imbalance. Moreover, I monitor values at serval points to see how they develop. The problem is that I perform a steady state calculation. There we see that scalars and temperature mix up in the vector variable "Velocity". In steady state, this variable is equal to Velocity i = Velocity in Stn Frame i - Frame Speed i In the Frame with chambers, the Frame Speed i = 0 since the chambers are standing still. So Velocity i = Velocity in Stn Frame i - 0 = Velocity in Stn Frame i In my moving part, I have a constant Frame Speed to the left. Since this is larger than the local Velocity in Stn Frame, the local Variable Velocity component becomes negative, i.e. to the right. Therefore my hot air is going to the right. Same happens in CFX. This is standard procedure when working with rotating or moving frames. You end up with Velocity in Stn Frame and Velocities in Relative Frames. The latter is called Velocity. The main problem is that I perform a steady state calculation. If I would do a transient analysis, then the moving frame is going to the left, bringing the hot air to the left, step by step. But I do not want to go to transient. My conveyor belt is huge. I would calculate for months. Also because there is no good initial guess. Normally this would be a steady state calculation, i.e. my result above. But then my hot air is in the wrong location, i.e. the worst initial guess I can imagine. Therefore I want to go a steady state. But then I need to find a trick to tell Fluent (or CFX) to mix my temperature (and scalars) in Variable "Velocity in Stn Frame" instead of default "Velocity".

October 21, 2022, 05:54		#7
LoGaL Senior Member Lorenzo Galieti Join Date: Mar 2018 Posts: 374 Rep Power: 12	Forgive me, but I do not see how a case like this admits a steady solution if the obstacles are moving inside the chambers. It is not physically possible. It is periodic, so with steady statistics, but not steady flow. I highly doubt fluent found a steady solution and, if it did, it's wrong. I can also tell that it didn't converge because the domain is symmetric, and your (RANS?) Temperature contour is not. This is again unphysical. There's no magic trick, if the physics is unsteady by nature, you need to go transient. Also to get the steady statistics, you need to run transient and do the average. On the other side, I would be surprised if it had to calculate for months...Depends a bit on the computational resources you have. You may even try to reduce the problem to 2D symmetric( so computationally cheaper) and run transient. In this way you neglect the obstacles height and assume them infinitely tall, but it is way more reasonable than trying to get a steady solution in 3D and flogging a dead horse.

October 21, 2022, 06:50		#9
Gert-Jan Senior Member Gert-Jan Join Date: Oct 2012 Location: Europe Posts: 1,835 Rep Power: 27	The reason I am looking for a photo of a certain flow situation is that I'm interested in the time averaged condition in each chamber/the machine as a whole. I'm not really interested in the obstacles. They vary from day to day anyway.

October 21, 2022, 08:05		#10
LoGaL Senior Member Lorenzo Galieti Join Date: Mar 2018 Posts: 374 Rep Power: 12	I see your point, but 1) it won't get any better than this, there are no tricks. You can't get the average picture with this setup. If you still want to try a steady simulation, perhaps have a look at mixing planes. This might be what you are looking for, but i am not sure. They are used in turbomachinery 2) The initial guess is not that bad, it won't take months 3) I firmly believe you should work to simplify your problem in a physically sound way. First step is to simulate half the domain and impose a symmetry boundary condition. Then you can also consider 2D, unless you really care about the effect of the obstacle height

October 21, 2022, 11:39		#11
Gert-Jan Senior Member Gert-Jan Join Date: Oct 2012 Location: Europe Posts: 1,835 Rep Power: 27	1) I can get a better initial guess if Fluent or CFX allows me to mix the scalars and temperature in the Velocity in Stn Frame. 2) If the hot air has accumlated at the right hand side of my steady state, and then has to travel to the left hand side of my equipment in a transient analysis, I will need several resisdence times, espcially if I the mixing in every chamber is included. That is very inefficient. 3) Probably you are right. I will consider this.

October 21, 2022, 11:48		#12
LoGaL Senior Member Lorenzo Galieti Join Date: Mar 2018 Posts: 374 Rep Power: 12	Look at mixing planes. They might be what you are looking for. They are alrdy implemented in Fluent.

October 27, 2022, 03:33		#13
Gert-Jan Senior Member Gert-Jan Join Date: Oct 2012 Location: Europe Posts: 1,835 Rep Power: 27	I tried mixing planes in CFX on a geometry look-a-like. You can find the results here: Hot air is moving in the wrong direction Mixing plane is averaging the results over the whole interface, leading to high temperature on both left and right hand side. In fact, it assumes the whole interface is connected from left to right, as if it is a periodic part of a cilinder.

October 27, 2022, 05:45		#14
LoGaL Senior Member Lorenzo Galieti Join Date: Mar 2018 Posts: 374 Rep Power: 12	As i suspected, it is not what you are looking for :/. They do exactly what you are asking, but for turbines (cylinders) Maybe smebody else has an idea for your problem. In the meantime, I would really simplify to a symmetric domain. And try to also do it 2D. I think it may be fast enough.