CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   FLUENT (https://www.cfd-online.com/Forums/fluent/)
-   -   Comically high residuals, need advice on why (https://www.cfd-online.com/Forums/fluent/226552-comically-high-residuals-need-advice-why.html)

Mattobox April 30, 2020 14:19

Comically high residuals, need advice on why
 
Hi there,

I've finalised my design of an air intake for my dissertation, and all of the geometry should be right. I've also done calculations to verify all boundary conditions, so these should be *at the very least* in the right ball-park figure, if not absolutely correct. I'm using ANSYS Fluent.

However, well, my residuals are... extremely high. Like 10^5 high... And I don't know why.

My mesh isn't the finest thing in the world (for this initial test run), but its not anywhere near bad enough to cause these residuals I wouldn't think.

My boundary conditions should be correct based on what I've calculated. My boundaries are pressure far field, pressure out and walls.

Pressure Far-Field was calculated from altitude data to be 11600Pa, Mach 2 and 218K. From my calculations, the static pressure rise should be approximately 4.93 through the intake. Therefore my outlet pressure is set from this at 57600Pa. I've also calculated temperature at pressure outlet, and I believe this calculation is atleast in the right ball-park at 386K. This is basically all I've input, so I don't see how it can be so wrong.

Reference Value and Initialisation are both set to Farfield, initialisation is standard initialisation.

I've also tried enabling both K-Omega and K-Epsilon turbulence models, which do not reduce residuals.

I'll attach an imgur file going over my mesh and setup, if anyone could give any help you'll be an absolute life saver: https://imgur.com/a/KFvMXrJ

Thanks a lot for any responses

vinerm April 30, 2020 14:46

Setup
 
Though not a bad idea, but you can work with Pressure-based solver as well since Mach number is around 2. Even if it increases a little more downstream, it should be alright. Pressure based solve is much more stable.

In any case, to test the setup, try fmg-initialization after doing standard initialization. If fmg-initialization is successful, then the material and boundary conditions are alright, otherwise, there is something wrong.

Whether the flow behaves like Inviscid or not is determined by Re and not by Mach number. Turbulence will certainly make it more stable. But then you should check Re and then decide if inviscid is more appropriate or not.

You can start simulation with a lower pressure at the outlet and slowly increase it to make the simulation more stable. Density based solver usually requires some steering of the solution. And fmg-initialization is best initial condition to start with.

Reference values have not effect on the solution. Those are only meant for post-processing.

Mattobox April 30, 2020 15:13

Quote:

Originally Posted by vinerm (Post 768102)
Though not a bad idea, but you can work with Pressure-based solver as well since Mach number is around 2. Even if it increases a little more downstream, it should be alright. Pressure based solve is much more stable.

In any case, to test the setup, try fmg-initialization after doing standard initialization. If fmg-initialization is successful, then the material and boundary conditions are alright, otherwise, there is something wrong.

Whether the flow behaves like Inviscid or not is determined by Re and not by Mach number. Turbulence will certainly make it more stable. But then you should check Re and then decide if inviscid is more appropriate or not.

You can start simulation with a lower pressure at the outlet and slowly increase it to make the simulation more stable. Density based solver usually requires some steering of the solution. And fmg-initialization is best initial condition to start with.

Reference values have not effect on the solution. Those are only meant for post-processing.

Thank you for this.

I have done an FMG-Initialization, and got some results, but I'm not sure what they mean.

I'm not entirely sure how to refer to the terms, but I did a 4 layer Initialisation. I did 1500 iterations so I hope that's enough. Layer 4 converged to 0.01. Layer 3 went to 0.179 normalised residuals, layer 2 to 0.0145, and layer 1 to a HUGE 430.

I take it this is not good? What does it mean?

vinerm April 30, 2020 15:21

FMG-Initialization
 
Default is set to three levels of coarseness, so, that is alright. All you need to ensure is that fmg-initialization finishes without error and if you display velocity and pressure contours after that, without running any iteration, those look plausible. If that is not the case, then you have to look at boundary conditions.

duri May 1, 2020 11:25

Quote:

Originally Posted by Mattobox (Post 768094)
Hi there,

I've finalised my design of an air intake for my dissertation, and all of the geometry should be right. I've also done calculations to verify all boundary conditions, so these should be *at the very least* in the right ball-park figure, if not absolutely correct. I'm using ANSYS Fluent.

However, well, my residuals are... extremely high. Like 10^5 high... And I don't know why.

My mesh isn't the finest thing in the world (for this initial test run), but its not anywhere near bad enough to cause these residuals I wouldn't think.

My boundary conditions should be correct based on what I've calculated. My boundaries are pressure far field, pressure out and walls.

Pressure Far-Field was calculated from altitude data to be 11600Pa, Mach 2 and 218K. From my calculations, the static pressure rise should be approximately 4.93 through the intake. Therefore my outlet pressure is set from this at 57600Pa. I've also calculated temperature at pressure outlet, and I believe this calculation is atleast in the right ball-park at 386K. This is basically all I've input, so I don't see how it can be so wrong.

Reference Value and Initialisation are both set to Farfield, initialisation is standard initialisation.

I've also tried enabling both K-Omega and K-Epsilon turbulence models, which do not reduce residuals.

I'll attach an imgur file going over my mesh and setup, if anyone could give any help you'll be an absolute life saver: https://imgur.com/a/KFvMXrJ

Thanks a lot for any responses


Is that your domain size. It will not converge with that small domain. The body is truncated and so all the boundaries on the right end has to be pressure outlet with no reflection.


All times are GMT -4. The time now is 02:12.