CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   Main CFD Forum (http://www.cfd-online.com/Forums/main/)
-   -   Supersonic flow past a sphere (http://www.cfd-online.com/Forums/main/99316-supersonic-flow-past-sphere.html)

Zeppo March 31, 2012 09:24

Supersonic flow past a sphere
 
2 Attachment(s)
Here is the scheme of cfd problem. A sphere (0.17m diameter) is streamlined by air.
Attachment 12258
The outer boundary is a freestream with params: mach number = 9.52; static pressure = 101325 Pa; temperature = 288K.
The inner boundary is a no-slip wall.
I'd like to obtain a pressure distribution over the sphere surface (pressure vs angle). Is it possible to estimate aerodynamic heating of the sphere surface?
Attachment 12257
If there were any analytic formulas it would suit me fine.

I've tried to simulate it in cfd program without any success. I didn't manage to make it converged.

SergeAS April 2, 2012 10:17

2 Attachment(s)
Quote:

Originally Posted by Zeppo (Post 352420)
Here is the scheme of cfd problem. A sphere (0.17m diameter) is streamlined by air.
Attachment 12258
The outer boundary is a freestream with params: mach number = 9.52; static pressure = 101325 Pa; temperature = 288K.
The inner boundary is a no-slip wall.
I'd like to obtain a pressure distribution over the sphere surface (pressure vs angle). Is it possible to estimate aerodynamic heating of the sphere surface?
Attachment 12257
If there were any analytic formulas it would suit me fine.

I've tried to simulate it in cfd program without any success. I didn't manage to make it converged.

This problem is widely studied since the early 60s of last century and you can easily find a large number of publications on this topic. In addition modern advanced CFD codes for compressible flows should not be any significant problems.
For example, my in-house density based CFD solver is easily coped with it. (see attachments with 2D-axisymmetric p and T fields)
http://www.cfd-online.com/Forums/att...1&d=1333375000
http://www.cfd-online.com/Forums/att...1&d=1333375051

I think that your problem is in the wrong boundary conditions.
Instead of setting the conditions for the freestream flow around the outer edge you need to specify the conditions of the freestream flow at the inlet and zero gradient for outlet

PS: Which CFD code you are used for simulation ?

PPS: As for the air temperature behind the shock wave in the given conditions by you exceeds 4000K, I would recommend to use the model for the properties of air, which takes into account the dependence of the thermodynamic properties on temperature and the dissociation

praveen April 2, 2012 10:32

Quote:

Originally Posted by SergeAS (Post 352697)
This problem is widely studied since the early 60s of last century and you can easily find a large number of publications on this topic. In addition modern advanced CFD codes for compressible flows should not be any significant problems.
For example, my in-house density based CFD solver is easily coped with it. (see attachments with 2D-axisymmetric p and T fields)
http://www.cfd-online.com/Forums/att...1&d=1333375000
http://www.cfd-online.com/Forums/att...1&d=1333375051

I think that your problem is in the wrong boundary conditions.
Instead of setting the conditions for the freestream flow around the outer edge you need to specify the conditions of the freestream flow at the inlet and zero gradient for outlet

PS: Which CFD code you are used for simulation ?

PPS: As for the air temperature behind the shock wave in the given conditions by you exceeds 4000K, I would recommend to use the model for the properties of air, which takes into account the dependence of the thermodynamic properties on temperature and the dissociation

Is this first order or second order scheme ? What is the numerical flux function used ?

SergeAS April 2, 2012 10:41

Quote:

Originally Posted by praveen (Post 352702)
Is this first order or second order scheme ? What is the numerical flux function used ?

You want know all my secrets ? :)

It is blended (CD-LxF) scheme with locally adapted blending factor

Zeppo April 6, 2012 15:09

Thank you Sergey.
Quote:

Originally Posted by SergeAS (Post 352697)
Instead of setting the conditions for the freestream flow around the outer edge you need to specify the conditions of the freestream flow at the inlet and zero gradient for outlet

OK, I'll try doing it like this
Quote:

Originally Posted by SergeAS (Post 352697)
For example, my in-house density based CFD solver is easily coped with it. (see attachments with 2D-axisymmetric p and T fields)

Are these pictures correspond with my boundary conditions (sphere diameter, mach number)? What's the plotting scale? Could you supply me with pressure and temperature distribution over the sphere surface in numeric representation?

SergeAS April 6, 2012 16:37

2 Attachment(s)
Quote:

Originally Posted by Zeppo (Post 353491)
Thank you Sergey.
OK, I'll try doing it like this
Are these pictures correspond with my boundary conditions (sphere diameter, mach number)?

diameter and mach number - Yes.
BC - No
Inlet and top side - freestream BC
Outlet - zero gradient in X direction
Wall of sphere - no-sleep BC (wall assumed adiabatic)
bottom side - axisymmetric BC (it is 2D-axisymmetric formulation)

Quote:

What's the plotting scale? Could you supply me with pressure and temperature distribution over the sphere surface in numeric representation?
Size on axis in millimeters, but it is just example and on my point view single simulation is not reliable in this case (used coarse mesh without mesh refinement for a boundary layer near the wall) In addition, you will not be able to refer to these results.

Distribution in x direction of P and T on sphere wall attached

http://www.cfd-online.com/Forums/att...1&d=1333804819
http://www.cfd-online.com/Forums/att...1&d=1333804836

Zeppo April 13, 2012 14:43

Quote:

Originally Posted by SergeAS (Post 353516)
diameter and mach number - Yes.
BC - No
Inlet and top side - freestream BC
Outlet - zero gradient in X direction
Wall of sphere - no-sleep BC (wall assumed adiabatic)
bottom side - axisymmetric BC (it is 2D-axisymmetric formulation)

Distribution in x direction of P and T on sphere wall attached

I've tried 2D axisymmetric modeling and partially succeeded in resolving this problem. The pressure I got is very similar to what you showed. But I faild in getting reasonable temperature field :(.
One more question. How long does it take the surface of sphere to get so hot (~4000K)? What's the order of magnitude?

Zeppo April 13, 2012 14:54

Quote:

Originally Posted by SergeAS (Post 353516)
diameter and mach number - Yes.
BC - No
Inlet and top side - freestream BC
Outlet - zero gradient in X direction
Wall of sphere - no-sleep BC (wall assumed adiabatic)
bottom side - axisymmetric BC (it is 2D-axisymmetric formulation)

Distribution in x direction of P and T on sphere wall attached

I've tried 2D axisymmetric modeling and partially succeeded in resolving this problem. The pressure I got is very similar to what you showed. But I faild in getting reasonable temperature field :(.
One more question. How long does it take the surface of sphere to get so hot (~4000K)? What's the order of magnitude?

SergeAS April 13, 2012 18:35

Quote:

Originally Posted by Zeppo (Post 354607)
I've tried 2D axisymmetric modeling and partially succeeded in resolving this problem. The pressure I got is very similar to what you showed. But I faild in getting reasonable temperature field :(.
One more question. How long does it take the surface of sphere to get so hot (~4000K)? What's the order of magnitude?

Quick assessment of temperature behind the shock wave can be obtained from the relation
\cfrac{T_{2}}{T_{1}} \approx\cfrac{2\gamma(\gamma-1)}{(\gamma+1)^{2}}M_{1}^{2} In stagnation point behind bow shock the temperature will be slightly higher but have a similar order of magnitude

Slightly lower temperature in my calculation due to the fact that my code is specialized for hypersonic flows and considers the real properties of air and dissociation at high temperature

When we talk about "How long" you mean computational or physical time ?

Zeppo April 14, 2012 06:41

Quote:

Originally Posted by SergeAS (Post 354640)
When we talk about "How long" you mean computational or physical time ?

I mean physical time. Let's assume that sphere has the temperature of 288K and starts being affected by a high Mach flow in unperturbed state at the initial time. How much time does the adiabatic surface of a sphere need to become warm? Is it possible to perform an unsteady simulation?

SergeAS April 14, 2012 07:30

Quote:

Originally Posted by Zeppo (Post 354673)
I mean physical time. Let's assume that sphere has the temperature of 288K and starts being affected by a high Mach flow in unperturbed state at the initial time. How much time does the adiabatic surface of a sphere need to become warm? Is it possible to perform an unsteady simulation?

This problem does not consider the thermal state of the sphere itself. Temperature on my pics corresponds only to the temperature of boundary layer of gas (air) assuming no heat transfer between the gas and the surface of the sphere (adiabatic wall).
The solution of unsteady heat conduction is a separate task. At first we can approve assumption of having a uniform distribution of heat in the area (an infinitely large thermal conductivity of the sphere) Warm-up time can be estimated on the basis of the scope of information about the specific heat of material and empirical relations for heat transfer coefficient for sphere (Nusselt number). Or directly simulate coupled unsteady task of heat transfer between gas and solid body if your software allow this

Of course, in this case the adiabatic wall condition is not applicable

Zeppo April 14, 2012 08:12

Quote:

Originally Posted by SergeAS (Post 354680)
Or directly simulate coupled unsteady task of heat transfer between gas and solid body if your software allow this

I'm not interested in heat propagation through the interior of a ball. So we can consider thermal conductivity of the material ball made of as an infinite quantity and make any other appropriate assumptions.


All times are GMT -4. The time now is 03:32.