[fluid23]

That depends on the wall treatment you are using, the level of accuracy you want and many other factors. The ranges I gave are very broad and loose. If you want to be as accurate as possible use the near wall model and keep your y+ values as close to 1 as you can. Obviously, in most cases it would require cell by cell modification of the mesh to acheive that which you cannot do in star-ccm+. However, you should be able to keep it fairly constrained in a straight pipe like this.

I suggest you read up on the wall treatment methods to understand the specifics. The help docs have good discussions of each one.

[ktytagong]

Thank you very much

[ktytagong]

I got a problem again.
According to the field function, I did follow what you said.
Apparently, I got 'Turbulent intensity field function: Floating point exception [divide by zero]Turbulent intensity field function: Floating point exception [divide by zero]'

Then I could not add the function of turbulent intensity

[fluid23]

The function is added, but it is blowing up because of the zero velocity in the boundary layer. That was an oversight on my part. For now you can just make it:

sqrt(2/3*${TurbulentKineticEnergy})/mag($${Velocity}+0.0001)

I am looking to see if I can make it a conditional statemtent to set Intensity to zero if velocity is zero. The equation above should be accurate enough though. You will get high TI anywhere you have zero velocity like the BL, but should be fine in the core flow. That 0.0001 will not impact anything out there.

[fluid23]

Use this:

mag($$Velocity)==0 ? 0:sqrt(2/3*${TurbulentKineticEnergy})/mag($${Velocity})

[ktytagong]

I will try and update again tomorrow

Thank you very much

[sarvesh34]

Hello

Can anybody help how to define the code for

(Outlettemperature-Liquidtemperature)/(InletTemperature-LiquidTemperature)

For field Function named Temperature Distribution.

I am New here..

Thanks in advance

[fluid23]

First, I am assuming you want this to be calculated for every cell not averaged for the whole fluid. If that is wrong let me know...

Create 2 Reports:
1. Mass Flow Averaged Temperature at Inlet (boundary only), call it InletT
2. Mass Flow Averaged Temperature at Outlet (boundary only), call it OutletT

Create a Field Function:
1. Right-click tools > field functions and select new > scalar.
2. Rename the field function and the function name in the properties window to 'Temperature Distribution'.
3. Leave dimensions as 'dimensionless' since you have T/T.
4. Set the definition to ($OutletReport - $Temperature)/($InletTReport-$Temperature)

It should then appear anywhere you can select scalr field functions (scenes, reports, monitors, etc...). You can treat it just like any other variable.

[sarvesh34]

Thank You very much

I will try it and post if there are any problems

[Bin]

I have a question. I understand that we need to check the y+ value based on the selected wall treatment. Use low y+ wall treatment as example, the desire y+ should be 1 to 5. y+>5 is definitely not recommended, but how about y+<1?

[hwsv07]

Originally Posted by Bin

I have a question. I understand that we need to check the y+ value based on the selected wall treatment. Use low y+ wall treatment as example, the desire y+ should be 1 to 5. y+>5 is definitely not recommended, but how about y+<1?

for the cells right next to the wall, y+ should be less than 5 in order for the viscous sublayer to be sufficiently resolved.

of course you can have very small y+, less what you suggested i.e. <1. however, this would mean excessive computation time.

[Bin]

Originally Posted by hwsv07

for the cells right next to the wall, y+ should be less than 5 in order for the viscous sublayer to be sufficiently resolved.

of course you can have very small y+, less what you suggested i.e. <1. however, this would mean excessive computation time.

This means it won't cause anything bad even the y+ is out of the recommended range (i.e. 1 to 5), just the computation time will be increased?

[hwsv07]

Originally Posted by Bin

This means it won't cause anything bad even the y+ is out of the recommended range (i.e. 1 to 5), just the computation time will be increased?

yes.

consider an unsteady simulation. of course, you can have a timestep size that is infinitely small. but what for? you probably can still can get the same result in a reasonable amount of time at a sufficiently large timestep.

[Bin]

Originally Posted by hwsv07

yes.

consider an unsteady simulation. of course, you can have a timestep size that is infinitely small. but what for? you probably can still can get the same result in a reasonable amount of time at a sufficiently large timestep.

I see. Thank for the explanations.

[Bin]

Originally Posted by MBdonCFD

Use this:

mag($$Velocity)==0 ? 0:sqrt(2/3*${TurbulentKineticEnergy})/mag($${Velocity})

Apart of writing this field function, how about monitoring the variance of velocity [i,j,k]? As far as I know, variance is the second moment of the flow field, means it is (u`)^2; (v`)^2; (w`)^2, which can represent the fluctuaing component. Am I right?