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

waves of values in supersonic flow

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

Like Tree1Likes
  • 1 Post By ghorrocks

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   September 13, 2017, 14:14
Default waves of values in supersonic flow
  #1
Member
 
Andy
Join Date: Jul 2017
Posts: 35
Rep Power: 5
Starcatcher is on a distinguished road
Greetings,


I get very strange results from a supersonic compressible CFX-simulation.
The geometry you can see in the attached picture. The Inlet and outlet are the periodic faces.


There is a shaft with two walls and two symmetry boundaries. The inlet and outlet are connected with an interface. The velocity is generated a subdomain with a momentum source (Domain->Subdomain->Source->Momentunm Source->x Component = 100000 kg/(mēsē)) It is enough impulse to accelerate the flow up to 1,4 Mach.
But from some reason waves in values get produced, see picture 1. They can be observed in the density, temperature and pressure field. When I turn off the compressibility they do not appear, so it has to do with that.

Turbulence model: SST
Advection Scheme: High Resolution
Turbulence Numerics: First order
Wall Heat Transfer: Adiabatic



Of course the calculation gets an overflow and crashes. After quite a lot iterations, but the waves can be observed already after view iterations.



Does anybody have a clue why I get such results and how I fix my setup?

Bild1.jpg


Thanks

Last edited by Starcatcher; September 13, 2017 at 19:08.
Starcatcher is offline   Reply With Quote

Old   September 13, 2017, 15:56
Default density based
  #2
Member
 
Andy
Join Date: Jul 2017
Posts: 35
Rep Power: 5
Starcatcher is on a distinguished road
Is the maybe I shall somehow change the solver to density based. Is it possible in CFX? Is CFX otherwise pressure based?
Starcatcher is offline   Reply With Quote

Old   September 13, 2017, 18:52
Default
  #3
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,400
Rep Power: 127
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
CFX does not have a density based solver. Only Fluent has that.

Are you aware that compressible frictional flow in a duct results in more than just pressure drop along the flow direction - the temperature and density changes as well. https://en.wikipedia.org/wiki/Compressible_duct_flow

As you have not specified any source term to control the thermal field I am not sure whether this flow is actually periodic.
ghorrocks is offline   Reply With Quote

Old   September 13, 2017, 19:07
Default
  #4
Member
 
Andy
Join Date: Jul 2017
Posts: 35
Rep Power: 5
Starcatcher is on a distinguished road
Thank you ghorrocks for the fast response.
Of course I'm aware of the basics of fluid mechanics.
Please note, that the change in the values happen not along the flow direction, but perpendicular to it. The Inlet and outlet are the periodic faces.

A heat source is not planned. I just initialized the calculation with a temperature of 500K. Because the walls are adiabatic no energy gets lost.
The momentum source compensates the pressure lost through friction at the walls.

I already ran this simulation with a smaller source and a low velocity (<0,3Ma) and there were no problems.

They say, that supersonic flows should be simulated with a density based solver. But where is an analogical setting in CFX?
Starcatcher is offline   Reply With Quote

Old   September 13, 2017, 19:13
Default
  #5
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,400
Rep Power: 127
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
There is no analogous solver to Fluent's density based solver. CFX has one solver for all flows.

The reason I pointed to the compressible flow link is because it shows the temperature changes in the flow direction as well. This means the flow is not periodic. So you are modelling the flow using a setup which cannot handle the actual flow, so weird things can happen. So I would not bother about fixing waves in a model which is non-physical in the first place. The non-physical simulation is a more fundamental problem.
ghorrocks is offline   Reply With Quote

Old   September 13, 2017, 19:25
Default
  #6
Member
 
Andy
Join Date: Jul 2017
Posts: 35
Rep Power: 5
Starcatcher is on a distinguished road
A very interesting explenation.
The peridicity is used here in order to observe a fully developed boundary layer without modelling the whole inlet length of the duct. So it shows just a small section of an imaginary pipe.

The case and the approach are given from the professor. I'm not allowed to change it. But I have to solve it.

Sent from my SM-A510F using CFD Online Forum mobile app
Starcatcher is offline   Reply With Quote

Old   September 13, 2017, 19:46
Default
  #7
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,400
Rep Power: 127
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Yes, using periodic boundaries is a standard way of modelling fully developed flow. But compressible flow in a duct is never fully developed (well, not until it gets Mach 1 and then stays there). And that is your fundamental problem. You can't use a method for fully developed flow to model something which is not fully developed.

You can tell your professor that his problem is not solvable
juliom likes this.
ghorrocks is offline   Reply With Quote

Reply

Tags
momentum sources, overflow, subdomain, supersonic, waves

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
CFD by anderson, chp 10.... supersonic flow over flat plate varunjain89 Main CFD Forum 18 May 11, 2018 07:31
Boundary Conditions for Supersonic Flow wididid OpenFOAM Running, Solving & CFD 5 August 17, 2017 01:17
Supersonic flow in a duct ecto STAR-CCM+ 1 July 6, 2017 12:00
problem in initializing the flow for supersonic jon william FLUENT 0 October 30, 2006 08:16
Inviscid Drag at subsonic, subcritical Mach # Axel Rohde Main CFD Forum 1 November 19, 2001 12:19


All times are GMT -4. The time now is 06:43.