[wassli]

Can some body please tell me average y+ requirements for Two layer all Y+ wall treatment for Realizible K epsilon two layer Turbulence Model
Waiting for reply....


Thanks in Advance

[wassli]

i am also wandering that is enhanced y+ wall treatment in Fluent and Two layer y+ wall treatment in Star are same or these are different..???

[fluid23]

It varies depending on who you ask, but in general the two layer all wall y+ model likes 1<y+<5 and 30<y+120. In between 5 and 30 the solver is interpreting between the low wall and high wall model so accuracy is reduced compared to what you get in the 'sweet spots'. For some applications, 120 may be too aggressive and an upper limit of 60 may be more appropriate.

[wassli]

Originally Posted by MBdonCFD

It varies depending on who you ask, but in general the two layer all wall y+ model likes 1<y+<5 and 30<y+120. In between 5 and 30 the solver is interpreting between the low wall and high wall model so accuracy is reduced compared to what you get in the 'sweet spots'. For some applications, 120 may be too aggressive and an upper limit of 60 may be more appropriate.

Thank you for the reply... i am keeping y+ in 1<5 but the solution is not getting converged at higher heat flux... If i apply lower heat flux then energy converges but at higher heat flux the energy residuals are rising and not getting converged...

If i am able to get the results conveged then after mesh independence i can get results at lower heat flux....
i don't know how to converge the energy.... i am worried and not know where i am making mistake....

[fluid23]

Are you modeling solid bodies or is the heat flux a boundary condition?

[wassli]

Originally Posted by MBdonCFD

Are you modeling solid bodies or is the heat flux a boundary condition?

no sir , i am just taking the fluid region and appling heat flux at wall. before this i incorporated solid body at wall and did conjugate heat transfer at lower heat flux,then i got the same results at outlet as were obtained but taking only fluid region..
after that, i just need heat transfer coefficient at wall so only took fluid region and applying higher heat fluxes but unable to converge the energy..
i also remind you that if i do conjugate heat transfer and apply higher heat flux at outer wall then also could not get the energy converged.
you can see the mesh y+ at wall and residuals

[fluid23]

I would typically advise against using a surface average to monitor y+, but in a straight pipe you can probably get away with it. Are you running a coupled or segregated analysis?

[wassli]

Originally Posted by MBdonCFD

I would typically advise against using a surface average to monitor y+, but in a straight pipe you can probably get away with it. Are you running a coupled or segregated analysis?

I am using segergated solver because the velocity is very small i.e .583 m/sec and Re No is close to 40,000. if i have not to get the surface average to wall y+ then should i draw line at wall and plot y+ graph and apply that criteria or do something else ?

[fluid23]

The XY plot is an option for the y+ in this application, but for anything more complex it is not sufficient. I typically create a scalar scene with all wall boundaries shown and select wall y+ as the scalar field. Then you just inspect visually and maybe play around with the max/min values to isolate areas which are high/low if necessary.

I think a coupled solver may still work for you. You may also consider adjusting relaxation factors or ramping the solution (start with a low flux and then increase it gradually).

[fluid23]

How are you initializing the flow?

[wassli]

Let me give you more details about the problem that i am modelling supercritical freon r134a and using its polynomial functions for thermophysical properties..
Mesing with Directed Mesher... Boundary condition are Mass flux inlet =600kg/m2.sec inlet Temp=71 c inlet and outlet pressure =4.3MPa absolute. Heat flux is 39KW/M2.
Turbulent prantle number appears when i activate Segregated Flow solver..
its default value is 0.9 , i do not know what does it mean
you can se the polynomial functions...
1.png

2.png

3.png

4.png

[wassli]

Originally Posted by MBdonCFD

How are you initializing the flow?

i give initial conditions in the physical initial conditions node... then after boundary conditons i simply click on initialize button... is there some other way to do that ??

if it is then i really don't know, please tell me if there is some other way...

Thanks

[wassli]

You can see the Y+ by scalar Function. there it green region at the inlet i have given 33mm enterence length so that the flo should be fully developed when it enter the heated length.

i think y+ is in viscous sublayer so turbulent model should show its full strength
1.png

[wassli]

Any Suggestions or recommendations are highly appreciated because i am student and given this task it should get completed...
I have given all my time to complete and due to this my other subjects are getting affected...

Waiting for reply....

[fluid23]

The turbulent prandtl number is just the ratio momentum eddy diffusivity to heat flux eddy diffusivity. A value of 0.9 is commonly applied for a lot of gasses, but I am not sure about R134a. I don't really work with these types of fluids so you may need to research that a bit.

I don't think your issue lies in your equations of state.

As for initializing, that would be how I would approach it. The coupled solver has something called expert initialization, but its probably overkill for this scale of problem. If you are sticking with segregated solver, maybe try initializing the flow to zero and let it converge from there.

As for the mass flux inlet, why did you choose this? I don't encounter that very often. I am not saying it is wrong necessarily, but I am curious to know why. Often times, trouble with residual convergence can indicate improper boundary conditions. If I were to do a pipe flow problem I would probably apply a mass flow inlet (with negative value) and a stagnation inlet at zero pressure. Not sure that it would be appropriate for this, but that's where I would start... granted that too may not always be appropriate.

Your wall y+ looks good. I did a little digging and found this FAQ on Steve Portal that may shed some light for you:

https://steve.cd-adapco.com/articles/en_US/FAQ/RD-6-667

[wassli]

Originally Posted by MBdonCFD

The turbulent prandtl number is just the ratio momentum eddy diffusivity to heat flux eddy diffusivity. A value of 0.9 is commonly applied for a lot of gasses, but I am not sure about R134a. I don't really work with these types of fluids so you may need to research that a bit.

I don't think your issue lies in your equations of state.

As for initializing, that would be how I would approach it. The coupled solver has something called expert initialization, but its probably overkill for this scale of problem. If you are sticking with segregated solver, maybe try initializing the flow to zero and let it converge from there.

As for the mass flux inlet, why did you choose this? I don't encounter that very often. I am not saying it is wrong necessarily, but I am curious to know why. Often times, trouble with residual convergence can indicate improper boundary conditions. If I were to do a pipe flow problem I would probably apply a mass flow inlet (with negative value) and a stagnation inlet at zero pressure. Not sure that it would be appropriate for this, but that's where I would start... granted that too may not always be appropriate.

Your wall y+ looks good. I did a little digging and found this FAQ on Steve Portal that may shed some light for you:

https://steve.cd-adapco.com/articles/en_US/FAQ/RD-6-667

Thank you for the reply because after a long time, i have got some body who is listening to my problem..
Before using segregated solver i tried coupled solver but it never get converged then i read blogs and it was clearly mentioned that when you try to capture shock waves then try coupled solver and necessarily when you mac number is greater than or equal to 0.3 or you are solving natural convection problem...
After that i left this solver.... If i am to use it again then what should i take to value to CFL...
i have not tried mass flow inlet before so now i am trying it... and take the velocity initial condition equal to zero and se its effects..

i also don't know the expert properties terms so tha's why i avoid plying with them.... could you please explain some of them and suggest their range so that i may try it....

Thanks

[wassli]

Sorr sir, i really didn't understood why to give the mass flow magnitude with -ve value...
I have applied boundary normal mass flow inlet with +ve value.... is it right or i have to give the negative value.

[fluid23]

Take anything in a blog with a grain of salt. I am not saying that they are wrong perse but I have never heard those conditions before. Star-CCM+ offers the following guidance on selecting coupled vs segregated solvers:

The Segregated Flow model solves the flow equations (one for each component of velocity and one for pressure) in a segregated or uncoupled manner. The linkage between the momentum and continuity equations is achieved with a predictor-corrector approach. This model has its roots in constant density flows. Although it is capable of handling compressible flows and low Rayleigh number natural convection, it is not suitable for capturing shock-waves, high Mach number flows, and high Rayleigh number applications.
The Coupled Flow model solves the conservation equations for mass and momentum simultaneously using a time- (pseudo-time-) marching approach. The preconditioned form of the governing equations used by the Coupled Flow model makes it suitable for solving incompressible and isothermal flows. One advantage of this formulation is its robustness for solving flows with dominant source terms, such as rotation. Another advantage of the coupled flow solver is that CPU time scales linearly with cell count; in other words, the convergence rate does not deteriorate as the mesh is refined.
To guide the choice between the Segregated Flow model and the Coupled Flow model, it is necessary to first consider the relative strengths and weaknesses of each:

• The segregated algorithm uses less memory than the coupled algorithm
• The coupled algorithm yields more robust and accurate solutions in compressible flow, particularly in the presence of shocks
• The coupled algorithm is more robust for high Rayleigh number natural convection
• The number of iterations required by the coupled algorithm to solve a given flow problem is independent of mesh size, while the number of iterations required by the segregated algorithm increases with mesh size
• In some situations the coupled algorithm, combined with the implicit solver, will permit very large CFL numbers. This would be analogous to an under-relaxation factor of 1 for all variables in a segregated algorithm. In contrast, the segregated algorithm needs significant under-relaxation for both velocity and pressure and, in compressible flows, energy.

As for CFL/Courant number in a steady simulation. If you are using segregated solver, a CFL between 1 and 3 is good to start with and you can probably ramp that up once things quite down a bit. As for Courant number in coupled solver, a value of 5 (default) is usually where I start. If things are diverging early then I consider a ramp from 0.1 to 5 over the first couple hundred iterations. As with the CFL/segregated approach you can probably ramp it up toward the end once things quite down.

I am not sure what to tell you on the prandtl number. I do not feel qualified to make a recommendation beyond the default value of 0.9. It is a reasonable assumption in the absence of better information. I encourage you to dig a little and see if there is anything online that might suggest a different value.

[fluid23]

If you apply a negative value to a mass flow (or mass flux) inlet it becomes an outlet. I find it is often better to pull air through the domain than to push it through.... if that makes sense.

[haristrawberry]

Pls make sure the mess have good transition from inflation layer to core elements. For CHT, Pls increase the solid time step size in the factor of 100 w.r.t fluid time scale. And getting low y+ plus case convergence bit tedious, I would suggest to give realistic BC as well as better initial conditions.


Sent from my HTC One A9 using CFD Online Forum mobile app