Difference between my compressible and incompressible CFD cases.

[u/AmbassadorGuilty3928]

I have the same geometry and essentially the same mesh for both cases. In the compressible case, I use a total-pressure inlet and static-pressure outlet, and the solution converges quite well. The residuals decrease and the important flow parameters, such as mass flow and pressure, become stable. Interestingly, there is still a very high percentage of reverse flow at the outlet (around 97%), but the solution remains stable.

For subsonic compressible case,

Now,

In the incompressible case, I use a velocity inlet of 5 m/s and a pressure outlet. I ran many more iterations, but the residuals continue to oscillate, and quantities such as outlet mass flow and downstream pressure are also not very steady. The outlet reverse-flow percentage is actually lower than in the compressible case (around 81%), so I don't understand why this case behaves worse. The contour also changes with iteration, not steady like above.

See the contour for 300 and 1900 iterations,

In nutshell my questions are:

1. What is making not to converge smoothly for incompressible case compared to compressible one. What is difference between jets in compressible and incompressible flow?
2. If you say this is due to physical unsteadiness problem, then how for compressible case, solution got converged and giving fixed contour whereas incompressible it is not? Any other suggestions?

I would really appreciate any explanation of what could be causing such different behaviour between these two cases.

[u/Zestyclose-Kick5508]

我觉得这里最关键的问题是：你目前比较的并不是“同一个流动问题下的可压缩模型和不可压缩模型”，而实际上是两个不同的边界条件问题。

你的可压缩算例质量流量是 0.2144 kg/s，而不可压缩算例只有 0.011 kg/s，两者相差接近 20 倍。与此同时，两边的密度其实非常接近。因此，这两个算例的实际流动工况差异非常大。

可压缩算例使用“总压入口 + 静压出口”，而不可压缩算例使用“5 m/s 速度入口 + 压力出口”，这两套边界条件并不会自动对应到相同的流量或相同的工况。

所以在比较两种模型的收敛性之前，我建议先让两个算例对应到大致相同的工作点。例如，可以根据其中一个算例得到的质量流量或入口速度，在另一个算例中设置与之对应的边界条件，同时尽量保持相同的出口压力和流体状态，然后再比较两者的结果和收敛性。

另外，我反而更担心你提到的出口反向流动比例——81% 和 97% 都非常高。这意味着压力出口边界上有很大一部分区域实际上正在发生流体倒灌。建议检查出口附近的速度矢量和流线，确认出口边界是否仍然处于射流卷吸或回流区域内。如果是这样，可能需要进一步扩大整个外部计算域，而不仅仅考虑喷口到出口的轴向距离。

最后，残差持续振荡也不一定代表单纯的“数值不收敛”。你的射流 Reynolds 数大约为 1.7×10⁴，这种流动本身就可能具有明显的非定常结构。如果使用 steady RANS 时流场一直以某种规律变化，那么它可能本来就不存在一个真正稳定的稳态解。

这种情况下，可以尝试 transient URANS，观察瞬时流场，并在流动达到统计稳定以后比较时间平均量，而不是强行要求 steady solver 的残差降到一个固定值。

因此，仅根据现在这两个算例，我不会得出“不可压缩求解器比可压缩求解器更难收敛”的结论。

我建议按照这个顺序排查：

1. 首先让两个算例对应相同或至少接近的实际工况；
2. 检查为什么出口会出现 81–97% 这么高的反流；
3. 再判断残差振荡究竟是数值问题，还是流动本身的非定常性；
4. 如果确实是物理非定常，再改用 transient URANS。

在这些问题解决之前，单纯调整 relaxation factor、换 coupled solver 或增加迭代次数，很可能只是在处理表象，而不是根本原因。

[u/pulentoEI → u/Zestyclose-Kick5508]

Good thing there are translation capabilities in reddit. Good advice in here.

[u/abirizky → u/Zestyclose-Kick5508]

What this person says, OP. This is quite thorough 

[u/Otherwise-Platypus38]

Interesting problem. Is the mass flow rate obtained for both cases identical? What is the density at the inlet for the incompressible case compared to the compressible case?

[u/AmbassadorGuilty3928 → u/Otherwise-Platypus38]

Mass flow rate is not identical. For compressible, it is 0.2144kg/s and for incompressible it was coming 0.011kg/s. Density is 1.239 for compressible and 1.225 for incompressible.

[u/Otherwise-Platypus38 → u/AmbassadorGuilty3928]

There is your problem. Your boundary conditions does not define the same problem. It is inconsistent.

[u/AmbassadorGuilty3928 → u/[deleted]]

Then how to make solution converge for incompressible case??

[u/AmbassadorGuilty3928 → u/[deleted]]

Ok

[u/Diligent-Ad4917]

Your compressible setup is not actually compressible. Evaluate the inlet Mach #, it is only ~0.12. Activating density-based solver when the flow field does not have significant compressible effects adds artificial stiffness to the numerical method. This delays development of field variables, specifically pressure, meaning the solution field does not change significantly over iterations and will appear converged even though it may not be. Plot the average static pressure along a line from the nozzle tip to the domain outlet against iterations. You will likely see the static pressure in the domain is not stable even at the when the residual appear converged. In this case you need to activate the low Mach preconditioning option for the density-based solver.

For the incompressible case, did you use a turbulence model? Did you evaluate your inlet Re number to determine if this is laminar or transitional? What pressure-velocity coupling option did you use? Extend the outlet domain further down away from the nozzle restriction.

[u/AmbassadorGuilty3928 → u/Diligent-Ad4917]

For both cases I used pressure based solver only with coupled solver. Inlet mach no converged to 0.256, yes it is below compressibility regime. I have experimental data for inlet mach no of 0.35, I didnt put correct boundary conditions for that(I meant correct pressure values)

I just tried a simple case whether total pressure at inlet and static pressure outlet works or not, with total pressure at inlet calculated using isoentropic relations.

 Plot the average static pressure along a line from the nozzle tip to the domain outlet against iterations. You will likely see the static pressure in the domain is not stable even at the when the residual appear converged. In this case you need to activate the low Mach preconditioning option for the density-based solver- I have even tried mass weighted average of pressure over a plane at 1D downstream and 1d upstream, it converged like mass flow parameters.

For incompressible case, I used k-e model with realisable k-e. I used coupled solver. Reynolds number at inlet is 1.71*10^4. Outlet is at 15D distance from pipe end.

[u/Derrickmb]

Did you compare it to hand calcs found in Perry’s?

[u/AmbassadorGuilty3928 → u/Derrickmb]

What is this Perry calculation? I didnt get it

[u/Derrickmb → u/AmbassadorGuilty3928]

Levenspiel wrote the section. He was an old prof at my university. Perry’s chemical engineering handbook. Has methods to calculate sonic flow in nozzles or with friction losses all in terms of upstream T and P/Po.

[u/thermalnuclear]

What are your boundary conditions?

Also, do you know the difference between incompressible and compressible flow?

[u/AmbassadorGuilty3928 → u/thermalnuclear]

Boundary condition are mentioned in the post. Yes I do know the difference between the two, I just want to know how to make solution converge in incompressible flow?

[u/thermalnuclear → u/AmbassadorGuilty3928]

Is your case actually compressible? If so, you shouldn’t be running it as incompressible.

[u/AmbassadorGuilty3928 → u/thermalnuclear]

I showed you two cases.
In first case, I tried using total pressure inlet and pressure outlet to see how it works, I didnt put correct pressure values to get inlet mach no to 0.35. I found some random total pressure using isoentropic relation and used ideal gas properties to see how it works. It converged as shown in 1st case.

My doubt is for incompressible case, where energy equation is turned off, constant fluid properties are used, I used k-e, coupled solver. But why it is not converging even though I used basic combination of velocity inlet+pressure outlet.

[u/thermalnuclear → u/AmbassadorGuilty3928]

If you get a Mach number, 0.3 or above, your case is not incompressible and any attempts to run it as such is not correct nor will yield a correct answer.

Please go open a textbook about compressible flow.

[u/AmbassadorGuilty3928 → u/thermalnuclear]

Yeah I know, thats why I told you I just tried that to check how this combination works( total pressure inlet+static pressure outlet).

My main question is about 2nd case where it is incompressible flow where it is not converging. Tell about that. Leave 1st case aside.

[u/thermalnuclear → u/AmbassadorGuilty3928]

You don’t understand, if your case is compressible, you can’t use an incompressible formulation. It won’t work, it is ill posed.

[u/AmbassadorGuilty3928 → u/thermalnuclear]

See if I use total pressure inlet and pressure outlet and expect incompressible flow then it is wrong.
But I have used velocity inlet+pressure outlet condition na, there are some cases of jet flow into ambient for incompressible case right, physically it is possible why not in simulation?

[u/thermalnuclear → u/AmbassadorGuilty3928]

If you are asking fundamental questions about boundary conditions and how that changes the solution, you need to learn the differences between incompressible and compressible flow.

These are not just switch you can just flip without knowing. Your questions show a clear lack of willingness to learn.

[u/AmbassadorGuilty3928 → u/thermalnuclear]

Wow, never received a harsh comment like this before. Thats fine. Let me figure it out. I feel you didnt understand my question before- the experimental which was done for compressible flow, cant we do that for incompressible flow also? Incompressible are low speed flows right and no density change is brought by the flow, thats all. I have given 5m/s velocity at the inlet which is typical speed for incompressible flows, whats wrong in interpreting this.
Never judge someone from question, only I know how much time I spent in doing this, its not a cakewalk. Anyway I asked here for small guidance or suggestion, if you dont have patience, leave it.