[mxodio]

Hi!

I am trying to include heat transfer on a simulation with a continuous flow and a dispersed fluid, however the simulation crashes due to the fact that the variable of particle temperature is not defined at the inlet.

When I run the case without heat transfer everything works fine, I even get the particle breakup correctly, and the continuous phase shows the correct temperature.

The continuous phase has defined for Heat transfer = Total Energy, and the dispersed phase has Heat transfer = Particle Temperature. In the Fluid Pairs model also Heat Transfer =Ranz Marshall. I insert the particles at the inlet, and I include an overall inlet temperature of 408 K for both phases, which is also the initialization temperature at the Domain definition.

Still, the simulation crashes and the error clearly shows that the inlet temperature for the particles (called drop.Temperature) is not defined at the inlet. I tried a CEL expression: ave(drop.Temperature)@Inlet = 408 [K] but it is not working.

Slave: 3 Error in subroutine GET_TEMP_BELG :
Slave: 3 Variable/locale undefined for BC type
Slave: 3 GETVAR originally called by subroutine INJECT_PART_BCP
Slave: 3 Variable name: drop.Temperature
Slave: 3 Locale name: Inlet
Slave: 3 BC physical type: INLET
Slave: 3 BC type: UNKNOWN
Slave: 3 Mesh Locale: BELG11
Slave: 3 Mesh Entity: CENTRE
Slave: 3 ----------------------------------
Slave: 3 Error in subroutine GET_TEMP_BELG :
Slave: 3 GETVAR originally called by subroutine INJECT_PART_BCP

So, my questions to anyone who can help would be:
- Has anyone had a similar problem?
- Is the syntax of the CEL expression correct?
- Is this the correct way to set up heat transfer in this type of flow?
- Could this be a software problem? Perhaps my version doesn't have heat transfer for particle enabled?

I appreciate any advice and opinions that you can share

[ghorrocks]

You cannot set ave(anything)@anywhere to a value. Rather, ave()@ returns a value. If this is how you set the drop inlet temperature I am surprised it did not report it an as error - but it certainly would not then put anything useful in the drop temperature.

Try setting the drop temperature at the inlet to a constant 408K. Does that work?

[mxodio]

Hi,

Thank you for your help That is what I was trying to do, unsuccessfully, with the CEL expression. How should I write the expression in order to SET the temperature? Do I need a fortran script?

I can't find where to input an inlet temperature exclusively for the droplets. At the inlet boundary condition I set a Total Temperature value, and the continuous phase takes this value with no problem, but the droplets don't seem to recognize it. If I run this without heat transfer, then yes, the droplets use this temperature value.

This is where the inlet temperature is defined, and in no other places can I include temperature for the droplets.

BOUNDARY: Inlet
Boundary Type = INLET
Interface Boundary = Off
Location = Inlet
BOUNDARY CONDITIONS:
FLOW REGIME:
Option = Subsonic
END
HEAT TRANSFER:
Option = Total Temperature
Total Temperature = 408.5 [K]
END

[Opaque]

On BOUNDARY: Inlet, there should be a tab for Fluid Values.

On such tab, you should Define Particle Behavior, and hopefully there will be a heat transfer setting for the Static Temperature.

Definitely, Total Temperature specification is for the continuous fluid.

Hope the above helps,

[mxodio]

That is the problem. Since I can't print-screen the tab, here is the code for the fluid tab information available WITH the heat transfer options described in previous messages.

FLUID: drop
BOUNDARY CONDITIONS:
Define Particle Data = t
MASS AND MOMENTUM:
Option = Cartesian Velocity Components
U = 124.3 [m s^-1]
V = 0 [m s^-1]
W = 0 [m s^-1]
END
PARTICLE DIAMETER DISTRIBUTION:
Diameter = 10 [micron]
Option = Specified Diameter
END
PARTICLE MASS FLOW RATE:
Mass Flow Rate = 2.83e-7 [kg s^-1]
END
PARTICLE POSITION:
Option = Uniform Injection
Particle Locations = Random
NUMBER OF POSITIONS:
Number = 500
Option = Direct Specification
END
END
END
END

As you can see, there is no place to enter a static temperature. That is why I wanted to input the boundary condition with a CEL expression or a Fortran subroutine.

How do I code in the inlet static temperature of the droplets? Due to the fact that the graphic inter phase doesn't allow me to do so.

Thank you for your help!!

[Opaque]

Odd.. What version of ANSYS CFX are you using ?

A suggestion will be to play the CoalCombustion_nonox.pre tutorial, and see if that one works. Look at the CoalInlet boundary.

You do not have to run the simulation, just play the tutorial and review the setup. Then you can compare the settings between your case, and the tutorial.

Good luck

[mxodio]

Thanks! The CFX version is 14.5 and it is owned by the university.

I checked the Coal Combustion tutorial, and the static temperature at the Inlet condition is defined in the Boundary Details Tab (the same place where I defined Total Temperature in my case).

It appears that the static temperature option is only available for solid particles , and is set for everything in this boundary: continuous and dispersed phases present in that boundary.

Isn't there a way for me to create this property? Because my heat transfer simulation runs and only crashes when it needs this inlet value. Can't I "code it in"?

Well, I guess this is a limitation of the software. Maybe in later versions this is improved.

[Opaque]

It seems that is a defect in ANSYS CFX 14.5. I checked in versions 15.0, and 16.0 and the Static Temperature for the particles is set in the Fluid Values tab.

You can try adding the command yourself by
- Right click on the boundary of interest
- Select Edit in Command Editor,
- Add the snippet you need,
- Press Process,
- Ignore the warning from the software,
- Press Close

Here is the snippet you want to add

....

FLUID: drop
BOUNDARY CONDITIONS: 
Define Particle Data = t

HEAT TRANSFER:
Option = Static Temperature
Static Temperature = MYVALUE
END

MASS AND MOMENTUM: 
Option = Cartesian Velocity Components
U = 124.3 [m s^-1]
V = 0 [m s^-1]
W = 0 [m s^-1]
END

....

END
END

Good luck

[mxodio]

It worked!!!! I included temperature, ignored the warnings, and now my simulation has good results

Also, I learned that if I you inject the liquid droplets in the domain tab (not at the inlet boundary condition as I need) then the temperature option does appear. However, this only allows for cone or sphere type injections, and in my case I needed a uniform injection at the inlet. So, it seems it was just a glitch.

Thanks! You have earned good karma points