|
[Sponsors] |
July 26, 2022, 00:01 |
2D axisymmetric Supersonic flow simulation
|
#1 |
New Member
ken
Join Date: Jul 2022
Posts: 8
Rep Power: 4 |
Hi all,
Recently I have been starting a new project testing supersonic cones at high altitudes in like a 2D simulation. My goal is to try to analyze the front shock of a heat shield which is shown in the Mach graph, ignoring the backflow. But I can't get a clean shock, and I keep getting waves within the shocks. So I took a step back to use an angled hill to test out the flow. But it still won't converge, and appear some reflect waves within the shock in the blue graph. For some reason, my flow keeps messing up even creating multiple different meshes. The following pictures are my setups and simulation results. I hope you guys can help me out. Solver: Density-based (I tried Pressure based, but it also didn't work) Turbulence model: Laminar ( I also tried spalart allamars) Velocity inlet from left to right as the pressure outlet the bottom is the axis, and the top is used as the wall but it is pretty far from the shock. the wall is in the right corner where a hill-shaped bump. (so the bottom be like three lines, axis - wall - wall ) Velocity speed (960 m/s ) initial pressure (52 pa for high altitude ) material: air density: ideal gas viscosity: Sutherland law energy: on (automatic for ideal gas) All these are after 8000 iterations. Last edited by gokenq; July 27, 2022 at 20:36. Reason: to have a better description. |
|
July 27, 2022, 06:32 |
|
#2 |
Senior Member
Lorenzo Galieti
Join Date: Mar 2018
Posts: 375
Rep Power: 12 |
I don’t get what is messed up, could you elaborate?
|
|
July 27, 2022, 08:10 |
|
#3 | |
Member
Void_CFD-user
Join Date: Feb 2022
Posts: 67
Rep Power: 4 |
Quote:
|
||
July 27, 2022, 20:55 |
|
#4 | |
New Member
ken
Join Date: Jul 2022
Posts: 8
Rep Power: 4 |
Quote:
So I took a step back and just do an angled hill and test from there (blue graph) but it also seems to be not working because that happens again even after 30,000 iterations or become invalid due to high residuals. |
||
July 28, 2022, 03:12 |
|
#5 |
Senior Member
Lorenzo Galieti
Join Date: Mar 2018
Posts: 375
Rep Power: 12 |
Ah ye, there's that kind of flow separation after the shock.
First, extend the domain as the other person above suggested. This won't probably change anything, BUT you need to do it anyways, otherwise the CFD is garbage Second, is the solution converged? In my experience, that sort of post-shock flow separation problem is purely numerical, and it is because the steady solver didn't find a steady solution. Can I see the residuals? I bet even after 30k iterations they didn't go down |
|
July 28, 2022, 03:58 |
|
#6 | |
Member
Void_CFD-user
Join Date: Feb 2022
Posts: 67
Rep Power: 4 |
Quote:
|
||
July 28, 2022, 20:41 |
|
#7 |
New Member
ken
Join Date: Jul 2022
Posts: 8
Rep Power: 4 |
This is a quick report of the project. Please take a look at my whole process.https://docs.google.com/document/d/1...f=true&sd=true
My goal is to analyze the front shock structure and find its stable flow setting. Currently not dealing with any after shock or backflow in the afterbody (So the project can be easier) But thank you for your time. |
|
July 30, 2022, 09:50 |
|
#8 |
Senior Member
Lorenzo Galieti
Join Date: Mar 2018
Posts: 375
Rep Power: 12 |
Please provide what was asked: residual plots. I don’t have time to go through your folder
If you ask for help, you must be willing to follow instructions xD |
|
August 1, 2022, 00:49 |
|
#9 |
New Member
ken
Join Date: Jul 2022
Posts: 8
Rep Power: 4 |
Sorry about that. This is the residuals graph. All other simpler meshes tend to have similar residuals.
thank you! |
|
August 1, 2022, 07:17 |
|
#10 |
Senior Member
Lorenzo Galieti
Join Date: Mar 2018
Posts: 375
Rep Power: 12 |
So your simulation is not even converging eh? The residuals are actually exploding…pretty useless to show results if you ask me.. if you let it go longer you will eventually get floating point exception
What settings do you use for the simulation? If you do check mesh in fluent,do you get errors in the console? |
|
August 1, 2022, 09:03 |
|
#11 |
New Member
ken
Join Date: Jul 2022
Posts: 8
Rep Power: 4 |
I don't have any error in mesh from the fluent check quality or check meshes.
setting: Solver: Density-based (I tried Pressure based, but it also didn't work) Turbulence model: Laminar ( I also tried spalart allamars) Velocity inlet from left to right is the pressure outlet the bottom is the axis, and the top is used as the wall but it is pretty far from the shock( I can have a bigger flow field) . Velocity speed (960 m/s ) initial pressure (52 pa for high altitude ) material: air density: ideal gas viscosity: Sutherland law energy: on (automatic for an ideal gas) The simple shape I did is in the right corner where a hill-shaped bump is. (so the bottom be like three lines, axis - wall - wall )( the blue graph) |
|
August 1, 2022, 09:24 |
|
#12 | |
Member
Void_CFD-user
Join Date: Feb 2022
Posts: 67
Rep Power: 4 |
Quote:
What I meant by solver setting in the solution methods that detail all the discretization schemes used, usually we'd advise using a first order scheme to begin with if you have convergence issues. Please share a snapshot of that and also a snap of your mesh. Do perform the mesh check in fluent. Additionally, try using fmg initialisation, it's a better form of initialisation. Also if you mesh is similar to the one in first image, try putting structured grid. |
||
August 1, 2022, 22:37 |
|
#13 |
New Member
ken
Join Date: Jul 2022
Posts: 8
Rep Power: 4 |
This is the setting.
I will try using face mashing. Thank you for helping me out! |
|
August 2, 2022, 02:25 |
|
#14 |
Senior Member
Lorenzo Galieti
Join Date: Mar 2018
Posts: 375
Rep Power: 12 |
To be fair, I think the mesh quality is quite good…and also the setup might be correct. it could just be that you are simulating quite difficult flow conditions.. this 60 pa at 1000 m/s is quite extreme
Did you already try to slowly ramp up the velocity? So say you start the simulation at 100 m/s, converge the simulation, increase to 200, run, increase to 400, run ecc ( at one point , you can also script it, rather than doing it manually) |
|
August 2, 2022, 04:06 |
|
#15 |
New Member
ken
Join Date: Jul 2022
Posts: 8
Rep Power: 4 |
Because of the shape of the heat shield, it is hard for me to do face meshing because I need to assign different regions and it often comes out of that blue stop sign. So I used vertex sizing for different radii around the wall, I used multiple circle zone with decreasing cell size for the meshes to get a better quality of the mesh-like above 0.9 average element quality. For face mesh, I often get a 0.41 average element quality, even if I try different zones' dirstrubtion. What would be a good range for the face mesh quality?
The reason I doing a high velocity and low pressure is that I want to simulate a reentry situation at a higher altitude. I did not try to slowly ramp up the velocity, but I can definitely do that! Thank you! I will let you know what is the result. |
|
August 2, 2022, 07:05 |
|
#16 |
Senior Member
Alexander
Join Date: Apr 2013
Posts: 2,363
Rep Power: 34 |
1. as was suggested you may gradually increase velocity
2. your may increase your domain so the shock wave don't interfer with outflow BC. ACtually you want domain as large as possible
__________________
best regards ****************************** press LIKE if this message was helpful |
|
August 2, 2022, 13:02 |
|
#17 |
Member
Void_CFD-user
Join Date: Feb 2022
Posts: 67
Rep Power: 4 |
[QUOTE=gokenq;832893]This is the setting.
I will try using face mashing. Thank you for helping me out![/QUOTE Alright so there's a few things you can do here. Chnage fradient scheme to least square or node based. First start with first order scheme for flow and when residuals go down, change to second order. Also turn on pseudo time step and use a low time scale factor, i.e reduce from 1 to 0.5 or even lower and let the residuals go down. Furthermore you can use high order term relaxation but that comes later on. Try firstly with the above changes. |
|
August 4, 2022, 09:20 |
Suggestions
|
#18 |
New Member
Wallace Rosendo
Join Date: Mar 2021
Posts: 7
Rep Power: 5 |
First of all, the turbulence model used in this case is wrong. Laminar modelling doesn`t serve due to high Reynolds number presented in this situation.
Three suggestions: 1. Use RANS modelling: Spalart-Allmaras or SST k-omega (2nd option is better, but SA model is cheapier for computational cost and is also good) 2. Check the mesh next from the wall for each RANS modelling (y plus has to be between 0 and 10 for linear region of boundary layer, greater than that the buffer region of boundary layer may be calculated and it's not good due to high possibility of numerical errors.) 3. Include "pressure-far-field" BC on the top region. It's a good option for inviscid supersonic flows that uses ideal gas law, like your case. |
|
August 5, 2022, 13:33 |
|
#19 |
Senior Member
Lorenzo Galieti
Join Date: Mar 2018
Posts: 375
Rep Power: 12 |
Lol, at that pressure it is definitely laminar.. it is almost rarified
|
|
August 5, 2022, 13:41 |
|
#20 |
New Member
Wallace Rosendo
Join Date: Mar 2021
Posts: 7
Rep Power: 5 |
||
Tags |
axisymmetric 2d fluent, boundary condition, high altitude, shock capturing, supersonic flow |
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Issues on the simulation of high-speed compressible flow within turbomachinery | dowlee | OpenFOAM Running, Solving & CFD | 11 | August 6, 2021 06:40 |
real gas simulation in ejector for supersonic flow | rahul_bhad1 | FLUENT | 1 | March 31, 2015 21:12 |
mass flow rate issue in supersonic nozzle simulation | xkang | FLUENT | 0 | July 31, 2014 16:06 |
fluid flow fundas | ram | Main CFD Forum | 5 | June 17, 2000 21:31 |