[krihamm]

Hello,

I want to perform supersonic simulations on a rocket for velocities ranging from subsonic to Mach 10. The rocket in question is approximately 15 m high. The body consists of an ogive nose and cylindrical sections with different diameters. The largest cylindrical section has a diameter of approximately 1 m. Four fins are attached to the bottom of the rocket. An enclosure has been added around the geometry.

I have created the geometry and built a - in my opinion - satisfactory mesh. I am, however, unsure about what setup settings I should use. I have run a few simulations with the following setup:

Default domain
Fluid material: ideal gas
Reference pressure: 1 [atm]
Heat transfer: total energy
Turbulence: SST
Wall function: scaleable, High speed (compressible) wall heat transfer model

Inlet
Flow regime option: supersonic
Mass and momentum option: normal speed and pressure
Rel. static pressure: 0
Normal speed: [equivalent to the Mach number I want to simulate]
Turbulence option: medium
Heat transfer: static temperature, 25 C

Outlet
Flow regime option: subsonic
Mass and momentum pressure: average static pressure
Relative pressure: 0
Pres. profile blend: 0.05

Solver control
Advection scheme: high resolution
Turbulence numerics: first order
Interpolation scheme: velocity interpolation type, trilinear (advanced options)
Compressibility control, High speed numerics (advanced options)

Does this seem like a good setup for such simulations? Is there something I have missed or should change? I am relatively new to CFX, so any input is much appreciated!

//krihamm

[ghorrocks]

The rule of thumb is that above Mach 5 the gas starts to dissociate and you get plasma becoming significant. CFX cannot model plasma. So I suspect you will not be able to accurately model up to Mach 10.

The setup of the simulation will depend on what you are trying to learn from the simulation. So what is the reason you are doing this simulation?

[krihamm]

I want to obtain the drag coefficient and the lift coefficient of the rocket.

Would Fluent be a better solver for higher speeds, or is Fluent also limited to Mach 5?

Originally Posted by ghorrocks

The rule of thumb is that above Mach 5 the gas starts to dissociate and you get plasma becoming significant. CFX cannot model plasma. So I suspect you will not be able to accurately model up to Mach 10.

The setup of the simulation will depend on what you are trying to learn from the simulation. So what is the reason you are doing this simulation?

[Gert-Jan]

This is rocket sience. Go to the library, grab a good book and start reading about the basics.

CFX might work up to Mach 3. I am quite sure Fluent's pressure based solver will even be worse. But you could try their density based solver. Ask this in the other forum. Alternatively, contact to ANSYS. They might know.

[ASCT]

Hi,

can I know if fluent solved the supersonic and hypersonic flows?

[ghorrocks]

I don't know of any CFD solver which can handle hypersonic flows. But I have not looked either, so feel free to look for yourself.

[ASCT]

Hi,

I was searching online and found this cfd solver named cfd++ which claims to be accurate for almost all flows including hypersonic flows. but there is no information about how to get it. you can give a shot


http://www.metacomptech.com/index.php/features/icfd

[ghorrocks]

They have a validation case on their website which shows good agreement to a Ma=6 flow. This is on the borderline of Navier Stokes supersonic flows to Hypersonics so CFX might be OK here. I have not checked the detail of what physics CFD++ has to enable hypersonic flow. Caviat Emptor.

How do you get it? Clicking on "Request Info" on there website seems like a good guess....

[Jiricbeng]

Hi there,


my experience is that Fluent is much more convinient than CFX for high speed external aerodynamics (subsonic to supersonic/hypersonic). I recommend performing these simulations in Fluent - you can use far-field boundary, you can use density based solver if desired and in addition Fluent was initially developed for external flows.



Moreover Fluent is capable to even manage one transient analysis with one setup, whereas CFX must be stopped and solver setup must be switched, especially if you want to create a transient run from subsonic to supersonic regime.



I spent some time trying to analyse supersonic flows in CFX but it was clear quite soon that compared to Fluent the CFX has got several disadvantages.

[ghorrocks]

Agreed, the density based solver in Fluent is far superior than CFX's pressure based solver for supersonic flows. Not sure how it goes in hypersonics, however - but it will be better than a pressure based solver.

I don't understand your comment about Fluent managing "one transient analysis with one setup", or why CFX is different to Fluent for this point.

[ASCT]

Hi, I have used both fluent and cfx extensively. In my personal experience and opinion.
shock formations in flow results to discontinuous Partial derivative equations and initially Ausm(adjective upstream segregation method) was specially developed to solve these type of equations.
more over in density based solver, the energy equation is solved along with conservation of mass and momentum equations. I don't know why but most of cfd engineers prefer solving energy equation along with conservation of mass and momentum equations when energy equation is involved. note: note that unlike density based solver, segregate solver and pressure based solver solves energy equation separately.

[Jiricbeng]

Originally Posted by ghorrocks

I don't understand your comment about Fluent managing "one transient analysis with one setup", or why CFX is different to Fluent for this point.

I mean in Fluent you apply Mach number, temperature and pressure on far-field and thats all. In CFX you must apply sub/supersonic regime. Fluent does not care. Therefore Fluent is capable to analyse a simulation including transient acceleration of the rocket (transient boundary conditions applied on far-field), e.g.

t=0s, Ma=0.2
t=20s, Ma=0.5
t=40s, Ma=1.2
t=60s, Ma=2.7
etc. In one transient run, without any interuption.




Note: Surprisingly, in Fluent I have better experience with Pressure based solver pressure-velocity coupled than with Density based solver even for supersonic cases.

[ghorrocks]

I suspect the accelerating rocket use case has a quite limited user base. I don't think that will be a limitation for many users