[wassli]

Thanks for these worthy information's... now i will try coupled solver using these recommendations....
please just clarify me one thing that should i choose outlet and give it to mass flow inlet and take the negative sign with it or do not do this and at the inlet. give the magnitude a negative sign..

[wassli]

Originally Posted by 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

Currently i am solving for fluid domain only and don't need to do CHT because the result at low heat flux with and without CHT are same so that's why i left it.

[fluid23]

I would assign a mass flow inlet to the outlet boundary and give it a negative value equal in magnitude to your target flow rate. The inlet should be a stagnation inlet at zero pressure (unless you have other information which may suggest something else).

[wassli]

Originally Posted by MBdonCFD

I would assign a mass flow inlet to the outlet boundary and give it a negative value equal in magnitude to your target flow rate. The inlet should be a stagnation inlet at zero pressure (unless you have other information which may suggest something else).

Ok thank you so much..

[fluid23]

Good luck. Let me know if any of this ended up helping, unfortunately the science of computational fluid dynamics sometimes involves a level of trial and error to find what works and what doesn't.

[me3840]

Originally Posted by MBdonCFD

I would assign a mass flow inlet to the outlet boundary and give it a negative value equal in magnitude to your target flow rate. The inlet should be a stagnation inlet at zero pressure (unless you have other information which may suggest something else).

I would really advise against using a mass flow condition with a negative value. The reason is this enforces a uniform velocity in a downstream position, which is in almost every case physically impossible.

You should either fix the pressure at the outlet and prescribe a mass flow rate at the inlet, or prescribe the inlet total pressure and outlet static pressure and monitor for mass conservation. The former is generally preferable and yields faster convergence. Both of these are very typical pipe flow problem boundary conditions.

IMO the problem here is clearly the mesh. The first cell aspect ratio is very large and the transition ratio from the last layer to the first core cell is probably more than 10. You need to resize your directed mesh so that the growth away from the wall is smooth through the entire cross section; the last layer should be about the same size as the first core cell.

I would also avoid having the first cell as high as y+=5. Keeping it below 1 guarantees you get at least a couple points in the viscous sublayer.

[fluid23]

That is actually not true. I use this approach all the time and it does not enforce a uniform velocity downstream. Star-CCM+ specifies this approach in their help documentation and I have had several conversations with CD-Adapco employees who say this is a totally valid approach.

There may very well be a mesh issue that needs resolved, but you are dead wrong about the mass flow inlet.

[me3840]

Okay, I misspoke a bit earlier.

The velocity field is specified uniform for a constant-density flow. For a moment I forgot we were dealing with something compressible.

However, this does not mean it's OK to use a mass flow outlet just because we're variable density, which in turn gives a nonuniform mass flow. The reason this is the case is because the density field is not enough information to always reconstruct the proper velocity field at the outlet. The distribution being enforced at the outlet is not based by any upstream momentum quantity.

Look at these images with the boundary conditions:
http://imgur.com/a/xvJl2

The first two images have mass flow inlets. They allow the boundary layer to develop naturally and don't have anything surprising in them.

The second two images are the BC scheme you propose. Because the outlet mass flow is chosen based only on the density, the velocity field is more-or-less uniform. This was computed using ideal-gas. You can clearly see the outlet condition is enforcing a far larger velocity in the boundary layer than what is natural, and the BL is being compressed down at the end because of it.

If the flow is heated at the walls this could change, but merely hoping the density will make up for using this boundary condition is a poor choice relative to just using a better set of BCs. What happens when there's recirculation or an eddy hits the outlet? The BC will have no idea it's really there and will warp the momentum unnaturally.

[wassli]

sorry, i am confused with this conversation... i am trying using Stagation pressure inlet and mass flow outlet as boundary conditon.. solution converges but the profile i need is not obtained there is a large temperature fluctuations at wall which should not happen and ..."segregated slover gives warning i.e. conjugate gradient solver didn''t converged."

if i am to try stagnation pressure inlet and pressure outlet as Bc's then i have same Gauge pressure at inlet and outlet and pressure losses are approx negligible..

In other case i got results with fluent i first activates refprop and then gives mass flux inlet and pressure outlet... in fluent, for SIMPLE solver, the solution coverges within 300 iterations and if i use COUPLE solver with CFL=200 then it converges within 50 iterations and convergence criteria i set is e-6 for all.

the question is why it does not get converged in star...!?
now i am improving mesh and trying results then will update you...

Thanks for giving me information and your time, i am hoping that i will get results with this guidence

[me3840]

Originally Posted by wassli

if i am to try stagnation pressure inlet and pressure outlet as Bc's then i have same Gauge pressure at inlet and outlet and pressure losses are approx negligible..

Yes, this is expected if you set the two pressures to 0. However, that isn't the idea behind these BCs. You want to fix one and adjust the other until you get the mass flow rate you're looking for. Obviously this is less convenient than using mass flow inlet and pressure outlet, which is why I would encourage their use.

I'm not sure what mesh you used with Fluent, but if you use similar boundary conditions in a STAR-CCM+ simulation with the same material properties, the solvers should act very similar to one another. (at least, the two segregated solvers and the two density-based coupled solvers - STAR-CCM+ has no equivalent to Fluent's pressure-based coupled solver).

[anaspauzi]

Originally Posted by 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.

Is there any reference to support the use of y+ between 1 and 5?

I find that y+<1 tends to diverge and around 2 or 3 is more stable for my case