[IronLyon]

Hello,

now I have been working with a simulation about the cooling process, the high temperature liquid state metal using the forced convection helium gas to cool down. I want to get the result of the cooling process in a transient process.

Firstly, what I did is to use the solid - fluid, so the fluid - fluid pair will not involved (for the metall I choose the solid model but using the parameters of liquid state, like heat capacity, heat transfer conductivity, density, except for the viscocity.) But I'm not so satisfied with the results, so I just want to do it in the fluid-fluid way.

For the fluid-fluid model , the most important parameters to control the heat transfer process I think is belows:
1. under the domain- Fluid Pair Models: Heat transfer coefficient
2. mass flow rate for forced convection gas
3. around the high-temperature metal, there is a water coil to make the heat flows out, so I set the heat transfer coefficient & outside temperature
4. wall: Heat transfer coefficient to eliminate the influence from the heat produced by compressible gas (because the in the chamber there is no outlet for the gas)

Now there is the error for the running, and I found the temperature monitor is also not correct, it should be start from 1773k of the metal-temperature, but it showed just like the initial temperature of the gas (about 300 K).

There are the error informations:
ERROR #001100279 has occurred in subroutine ErrAction.
Message:
c_fpx_handler: Floating point exception: Overflow


Parallel run: Received message from slave

Slave partition : 23
Slave routine : ErrAction
Master location : Message Handler
Message label : 001100279
Message follows below - :

ERROR #001100279 has occurred in subroutine ErrAction.
Message:
Stopped in routine FPX: c_fpx_handler


ERROR #001100279 has occurred in subroutine MESG_RETRIEVE.
Message:
Stopping the run due to error(s) reported above



An error has occurred in cfx5solve:
The ANSYS CFX solver exited with return code 1. No results file has been created.

End of solution stage.

Someone has the ideas? Thanks!

[evcelica]

You may need to give some more information, a picture, and the .out or .ccl file file for us to help.

Have you enabled the beta features to run two separate fluids?

[IronLyon]

(delete the repeated reply.)

[IronLyon]

Originally Posted by evcelica

You may need to give some more information, a picture, and the .out or .ccl file file for us to help.

Have you enabled the beta features to run two separate fluids?

There are some pictures about the mesh, in picture 2 the red vector means the inlet flow of the gas, inlet gas and the gas in the chamber are the same helium gas. And for the .out document.
Maybe you will advice me to improve the mesh quality...

1.PNG

2.jpg

3.PNG

Fluid Flow CFX_001.zip

[ghorrocks]

Your geometry is quite complex and large, I would do debugging on this model on a simplified model with a coarse mesh.

You should read the FAQ on overflow error: https://www.cfd-online.com/Wiki/Ansy...do_about_it.3F

Where has your 0.001s time step come from? A very common error on the forum is people simply use to large a time step. I would recommend using adaptive time stepping, homing in on 3-5 coeff loops per iteration. Make sure the starting time step is small enough that the first time step definitely converges, maybe 1e-8[s], and let it increase to whatever it wants from there.

[IronLyon]

Originally Posted by ghorrocks

Your geometry is quite complex and large, I would do debugging on this model on a simplified model with a coarse mesh.

You should read the FAQ on overflow error: https://www.cfd-online.com/Wiki/Ansy...do_about_it.3F

Where has your 0.001s time step come from? A very common error on the forum is people simply use to large a time step. I would recommend using adaptive time stepping, homing in on 3-5 coeff loops per iteration. Make sure the starting time step is small enough that the first time step definitely converges, maybe 1e-8[s], and let it increase to whatever it wants from there.

Thank you! I have tried to cut the model into pieces, so that other not so important teils can be hex. But for these coil parts (with yellow highlight), it seems to be difficult to make them finite.
4.PNG

5.jpg
Until now the solver doesn't work, I 'm not sure if there are some unsuited setting for the fluid-fluid pair.

[ghorrocks]

That is not what I meant when I said simplify the model. I mean do a simple model of a square box or something like that. A really simple model which will run quickly and allow you to debug easily.

And don't forget there is also the issue of your time step size and all the other points on the FAQ I linked to.

[IronLyon]

Originally Posted by ghorrocks

That is not what I meant when I said simplify the model. I mean do a simple model of a square box or something like that. A really simple model which will run quickly and allow you to debug easily.

And don't forget there is also the issue of your time step size and all the other points on the FAQ I linked to.

Thank you! I have tried to simplify the model (using the quadrate coil to replace the circle coil, and simplify the geometry of the hold), but the problem still exist.
8.jpg

9.PNG
Then I did some changes to separate the two fluid domains involved from CFX configuration (in CFX Pre, 'Edit' - 'Options' - 'General' - 'Beta Options' - 'Physics Beta Features' deselect the 'Constant Domain Physics' option), and in the interface set the 'Mass And Momentum' as 'No Slip Wall'. Then the problem is solved, even I use the constant timesteps 0.005s. (After this simple model, I have also tested my original model, it also works. I'm not sure why it works. For my case, there are two fluid domain, one is helium gas, the other is liquid cupronickel at 1500K. And the two fluid don't mix up with each other absolutly)

[IronLyon]

Now I'm interested about how to control the heat transfer process between the two fluid, one is gas at room temperature (293 K), the other one is liquid metal with high temperature (1773 K).
After define the material properties, we can choose the heat transfer options for the interface, like for instance thermal contact resistance (TCR) and thin material.
I'd like to know, for the TCR may it is not suitble for the case between fluids, right? Because the surface should be 100% contacted.
How about the thin material, is it suitble? And after we choose this one, what we can do is only to set the thickness like 1 mm. Is it enough to define the heat transfer??

[ghorrocks]

How you model heat transfer depends on what you are modelling and what you want to resolve. Is the liquid metal a coherent pool with gas above, so heat transfer through the free surface? Or gas bubbles? Foam? liquid metal droplets? What flows are there in the liquid metal and gasses?

[IronLyon]

Originally Posted by ghorrocks

How you model heat transfer depends on what you are modelling and what you want to resolve. Is the liquid metal a coherent pool with gas above, so heat transfer through the free surface? Or gas bubbles? Foam? liquid metal droplets? What flows are there in the liquid metal and gasses?

Thank you. For my case, the melt (liquid) metal ball is suspended in the chamber (filled with gas without gravity). And there is no outlet but an inlet with same gas (forced convection) flows towards the bottom of the metal ball to make it cool down (from 1773 K). This forced gas flows out from the gas cylinder, I set the chamber T and the inlet gas T are just the room temperature 293 K. Interface heat transfer is conservative interface flux, and I didn't use the thermal radiation.
The simulation results showed the cooling rate is slower than the real cooling rate (from the experiment). So should I use the thermal radiation of the metal or any other factors I should consider? Based on the current data/parameters (for instance the material parameter which are not so accurate) I could not do any more to affect the heat transfer process.

[ghorrocks]

Why don't you use radiation models? I would have thought at these temperatures it would be very important.

Have you done a back-of-the-envelope calculation to see whether radiation is important or not?

Here it is:
Radiative heat transfer will be of the order of
q = Stefan-Boltzmann * (T^4 - Ta^4) = 5.67E-8*(1773^4-293^4) = 560kW/m2

Convective heat transfer will be of the order of
q = h * (T - Ta) = 30 * (1773-293) = 44kW/m2

It looks like about 10 times more heat transfer will occur by radiation than by convection. I think your decision to ignore radiation was a bad decision

[IronLyon]

Originally Posted by ghorrocks

Why don't you use radiation models? I would have thought at these temperatures it would be very important.

Have you done a back-of-the-envelope calculation to see whether radiation is important or not?

Here it is:
Radiative heat transfer will be of the order of
q = Stefan-Boltzmann * (T^4 - Ta^4) = 5.67E-8*(1773^4-293^4) = 560kW/m2

Convective heat transfer will be of the order of
q = h * (T - Ta) = 30 * (1773-293) = 44kW/m2

It looks like about 10 times more heat transfer will occur by radiation than by convection. I think your decision to ignore radiation was a bad decision

Thank you. When I use the thermal radiation - P1 model of the metal, there is the error:

ERROR #001100279 has occurred in subroutine ErrAction. |
| Message: |
| Equation subsystem: "Wall Scale - 1" has not been found on both s- |
| ides of interface "Default Fluid Fluid Interface". Check that you |
| have set consistent physics across all domains that use this int- |
| erface. |
+--------------------------------------------------------------------+

+--------------------------------------------------------------------+
| ERROR #001100279 has occurred in subroutine ErrAction. |
| Message: |
| Stopped in routine DEF_ALGM_SUBSYS_ZIF |


| An error has occurred in cfx5solve: |
| |
| The ANSYS CFX partitioner exited with return code 1.



I have deselect 'Constant Domain Physics', is this the problem?

And by the way, as I can image, when the forced gas blows towards the liquid metal ball from the bottom, there will be a shift of the ball. If I want to know how much the displacement could be, if there any way to get the informations from the monitor?
Now I just put the monitor on the interface to get the pressure, I want to use the pressure later to calculate the force and then compare the force with the force with the lorence force (electromagnetic field make the metal ball float and in the right position, besides the environment is no gravity). But I think too much calculation is not so accurate. And I found that I can use the expression like: force_x()@location, but when the monitor set to the interface of metal side, it was always stable for the pressure (for the force it was always 0). Should I put the monitor on the interface but the gas side? And if I can directly get the shift/displacement of the metal ball?

[ghorrocks]

This is looking more and more like the old "let's model everything" adventure. This always ends in wasted time and no useful results. I guarantee it. I have seen it so many times.

What you are doing is extremely complex - radiation, multiphase, heat transfer over high temperature gradients, phase change, multiple materials, and now you are adding FSI/rigid body motion as well. This is a very complicated simulation and you should expect it will take months of work to get working properly.

I strongly recommend you simplify this simulation and look at the key performance parameters in simplified cases. In my experience you learn a lot more about complex systems like this as you can understand what is going on better and see the effect of your simplifying assumptions.

I'll jump off my soap box now and answer your question: You are using the P1 radiation model. This is intended for optically dense mediums, in other words where the radiation does not travel very far, due to heavy particle loading, smoke, opaque fluids etc. Didn't you say the gas is helium? And the metal is a ball in the middle? I would think the helium is going to be optically transparent, and if that is the case then the P1 model is not suitable. You need to consider either Monte Carlo or Direct Transfer models. Note these models are significantly more complex and tricky to use than the P1 model.

[IronLyon]

Originally Posted by ghorrocks

This is looking more and more like the old "let's model everything" adventure. This always ends in wasted time and no useful results. I guarantee it. I have seen it so many times.

What you are doing is extremely complex - radiation, multiphase, heat transfer over high temperature gradients, phase change, multiple materials, and now you are adding FSI/rigid body motion as well. This is a very complicated simulation and you should expect it will take months of work to get working properly.

I strongly recommend you simplify this simulation and look at the key performance parameters in simplified cases. In my experience you learn a lot more about complex systems like this as you can understand what is going on better and see the effect of your simplifying assumptions.

I'll jump off my soap box now and answer your question: You are using the P1 radiation model. This is intended for optically dense mediums, in other words where the radiation does not travel very far, due to heavy particle loading, smoke, opaque fluids etc. Didn't you say the gas is helium? And the metal is a ball in the middle? I would think the helium is going to be optically transparent, and if that is the case then the P1 model is not suitable. You need to consider either Monte Carlo or Direct Transfer models. Note these models are significantly more complex and tricky to use than the P1 model.

Thank you. I know the model is somehow complicated, the simulation results may be not accurate, but I’m trying to complete the functions which I need (one is to simulate the cooling process, and the other is to know the shift under the effect of the blowing gas. And during these few months on learning CFX I have actually learned a lot)
I will trying other model for the thermal radiation, until now the Monte Carlo has the same error, but I will try to adjust other options.
For the monitor, I used the force_y()@location (Interface on the gas side, but the result showed quite small, I’m not sure if it was correct). Like what you have said, did you mean this kind of monitor (or even some way to monitor the displacement) is only suitable for the rigid body, but not for the fluid?
Thank you

[ghorrocks]

If you don't do some validation and verification then all you are doing is generating pretty pictures. Using radiation modelling as an example, start by taking a box with a hot face and a cold face. The analytical heat transfer in this case is easy. Then simulate it and try to get CFX to give an accurate heat transfer value. Basic simulations like this are vital so you understand the models good enough to get them accurate.