CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > FLUENT

2D axisymmetric Supersonic flow simulation

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   July 26, 2022, 01:01
Smile 2D axisymmetric Supersonic flow simulation
  #1
New Member
 
ken
Join Date: Jul 2022
Posts: 8
Rep Power: 2
gokenq is on a distinguished road
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.
Attached Images
File Type: gif Capture.GIF (91.5 KB, 22 views)
File Type: gif Capture2.GIF (111.6 KB, 19 views)

Last edited by gokenq; July 27, 2022 at 21:36. Reason: to have a better description.
gokenq is offline   Reply With Quote

Old   July 27, 2022, 07:32
Default
  #2
Senior Member
 
Lorenzo Galieti
Join Date: Mar 2018
Posts: 297
Rep Power: 10
LoGaL is on a distinguished road
I don’t get what is messed up, could you elaborate?
LoGaL is offline   Reply With Quote

Old   July 27, 2022, 09:10
Default
  #3
Member
 
Void_CFD-user
Join Date: Feb 2022
Posts: 67
Rep Power: 2
Indra is on a distinguished road
Quote:
Originally Posted by gokenq View Post
Hi all,

Recently I have been starting a new project testing on supersonic cones at high altitudes in like a 2D simulation.

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.
i think that first of all your domain needs to be bigger for the shock and flow to develop properly. but anyways, what exactly is the problem here?
Indra is offline   Reply With Quote

Old   July 27, 2022, 21:55
Default
  #4
New Member
 
ken
Join Date: Jul 2022
Posts: 8
Rep Power: 2
gokenq is on a distinguished road
Quote:
Originally Posted by Indra View Post
i think that first of all your domain needs to be bigger for the shock and flow to develop properly. but anyways, what exactly is the problem here?
Quote:
Originally Posted by LoGaL View Post
I don’t get what is messed up, could you elaborate?
I try to analyze the front shock of a heat shield (red graph), and it seems to be messed up somewhere since the shock never comes out clear but lots of small waves within the shocks. I tried to make a bigger flow field or small size of the mesh but it did not seem to be working.

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.
gokenq is offline   Reply With Quote

Old   July 28, 2022, 04:12
Default
  #5
Senior Member
 
Lorenzo Galieti
Join Date: Mar 2018
Posts: 297
Rep Power: 10
LoGaL is on a distinguished road
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
LoGaL is offline   Reply With Quote

Old   July 28, 2022, 04:58
Default
  #6
Member
 
Void_CFD-user
Join Date: Feb 2022
Posts: 67
Rep Power: 2
Indra is on a distinguished road
Quote:
Originally Posted by gokenq View Post
I try to analyze the front shock of a heat shield (red graph), and it seems to be messed up somewhere since the shock never comes out clear but lots of small waves within the shocks. I tried to make a bigger flow field or small size of the mesh but it did not seem to be working.

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.
could you show us your solution methods as well as residuals. Also, try putting a structured mesh as your geometry is not that complex(perform a mesh check once in Fluent before running the sim).
Indra is offline   Reply With Quote

Old   July 28, 2022, 21:41
Default
  #7
New Member
 
ken
Join Date: Jul 2022
Posts: 8
Rep Power: 2
gokenq is on a distinguished road
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.
gokenq is offline   Reply With Quote

Old   July 30, 2022, 10:50
Default
  #8
Senior Member
 
Lorenzo Galieti
Join Date: Mar 2018
Posts: 297
Rep Power: 10
LoGaL is on a distinguished road
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
LoGaL is offline   Reply With Quote

Old   August 1, 2022, 01:49
Default
  #9
New Member
 
ken
Join Date: Jul 2022
Posts: 8
Rep Power: 2
gokenq is on a distinguished road
Sorry about that. This is the residuals graph. All other simpler meshes tend to have similar residuals.

thank you!
Attached Images
File Type: gif Capture.GIF (160.7 KB, 6 views)
gokenq is offline   Reply With Quote

Old   August 1, 2022, 08:17
Default
  #10
Senior Member
 
Lorenzo Galieti
Join Date: Mar 2018
Posts: 297
Rep Power: 10
LoGaL is on a distinguished road
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?
LoGaL is offline   Reply With Quote

Old   August 1, 2022, 10:03
Default
  #11
New Member
 
ken
Join Date: Jul 2022
Posts: 8
Rep Power: 2
gokenq is on a distinguished road
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)
gokenq is offline   Reply With Quote

Old   August 1, 2022, 10:24
Default
  #12
Member
 
Void_CFD-user
Join Date: Feb 2022
Posts: 67
Rep Power: 2
Indra is on a distinguished road
Quote:
Originally Posted by gokenq View Post
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)

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.
Indra is offline   Reply With Quote

Old   August 1, 2022, 23:37
Default
  #13
New Member
 
ken
Join Date: Jul 2022
Posts: 8
Rep Power: 2
gokenq is on a distinguished road
This is the setting.

I will try using face mashing.

Thank you for helping me out!
Attached Images
File Type: gif Capture2.GIF (61.2 KB, 10 views)
File Type: gif Capture.GIF (104.8 KB, 5 views)
gokenq is offline   Reply With Quote

Old   August 2, 2022, 03:25
Default
  #14
Senior Member
 
Lorenzo Galieti
Join Date: Mar 2018
Posts: 297
Rep Power: 10
LoGaL is on a distinguished road
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)
LoGaL is offline   Reply With Quote

Old   August 2, 2022, 05:06
Default
  #15
New Member
 
ken
Join Date: Jul 2022
Posts: 8
Rep Power: 2
gokenq is on a distinguished road
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.
gokenq is offline   Reply With Quote

Old   August 2, 2022, 08:05
Default
  #16
Senior Member
 
Alexander
Join Date: Apr 2013
Posts: 2,178
Rep Power: 31
AlexanderZ will become famous soon enoughAlexanderZ will become famous soon enough
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
AlexanderZ is offline   Reply With Quote

Old   August 2, 2022, 14:02
Default
  #17
Member
 
Void_CFD-user
Join Date: Feb 2022
Posts: 67
Rep Power: 2
Indra is on a distinguished road
[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.
Indra is offline   Reply With Quote

Old   August 4, 2022, 10:20
Default Suggestions
  #18
New Member
 
Wallace Rosendo
Join Date: Mar 2021
Posts: 4
Rep Power: 3
wrosendoeng is on a distinguished road
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.
wrosendoeng is offline   Reply With Quote

Old   August 5, 2022, 14:33
Default
  #19
Senior Member
 
Lorenzo Galieti
Join Date: Mar 2018
Posts: 297
Rep Power: 10
LoGaL is on a distinguished road
Lol, at that pressure it is definitely laminar.. it is almost rarified
LoGaL is offline   Reply With Quote

Old   August 5, 2022, 14:41
Default
  #20
New Member
 
Wallace Rosendo
Join Date: Mar 2021
Posts: 4
Rep Power: 3
wrosendoeng is on a distinguished road
Quote:
Originally Posted by LoGaL View Post
Lol, at that pressure it is definitely laminar.. it is almost rarified
Yeah, I have to apologize me. I didn't see the pressure in BC. I considered it as a sea-level pressure and, yes, it's quite low and then, laminar condition may be applied.
wrosendoeng is offline   Reply With Quote

Reply

Tags
axisymmetric 2d fluent, boundary condition, high altitude, shock capturing, supersonic flow

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


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 07:40
real gas simulation in ejector for supersonic flow rahul_bhad1 FLUENT 1 March 31, 2015 22:12
mass flow rate issue in supersonic nozzle simulation xkang FLUENT 0 July 31, 2014 17:06
fluid flow fundas ram Main CFD Forum 5 June 17, 2000 22:31


All times are GMT -4. The time now is 13:30.