# rocket internal flow simulation

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

 May 3, 2001, 11:31 rocket internal flow simulation #1 Andres Peratta Guest   Posts: n/a I'm trying to solve the problem of an homogeneous propellant burning into a rocket motor ( 2D ). The formulation is based on the conservation equations of mass, momentum, energy and species concentration, with consideration of finite-rate chemical reactions. I'm using ALE (Lagrangian-Eulerian) finite volume formulation on a structured (finite difference) mesh with ICE (Implicit Continuous-Fluid Eulerian) method. Mesh rezoning is implemented in order to resolve the high gradients in the flame zone and solid degradation layer. (Solid cells may be converted into gas cells during the calculation.) Here are my problems. When dealing with very different time scales and Mach numbers ranging from 0.001 to almost 1, I found a lot of problems with convergence and stability of the ICE-ALE algorithm. In adition, the geometry involves large aspect ratio cells (1:1000). I always like finite volumes because physics is clear for each term in the equations, but I'm afraid that they are not very efficient in order to perform all mach number calculation or even to deal with large aspect ratio cells. Is that true? shoul I migrate to another method? Can anybody give me a hint ?. Thanks in advance Andres Here is a brief description of my adapted ALE - ICE algorithm: 1) Initialize thermodynamics, transport and chemical kinetics data. 2) Load initial mesh, boundary and initial conditions. 3) Determine time step. 4) Integrate chemical reaction terms to update e and Y. 5) Integrate the heat diffusion term (ADI) to update e. 6) Integrate mechanical diffusion equation to update Y and e (Fick's law is used). 7) If neccesary, add artificial pressure 8) Advance (u,v) explicitly with momentum equation ( this would be the initial guess for step 10). Apply boundary conditions. 9) Evaluate relaxation factor on each cell (derivative of the function f = p - EOS, respect to p) 10) Obtain time advanced pressure implicitly (in a Lagrangian way) with a Newton-Raphson like solver applied to the momentum, energy and equation of state equations. (Maybe this step should require further explanation.) 11) Iterate step 9) sweeping through the whole mesh until no relevevant pressure corrections is found. 12) Obtain new (u,v) with the latest pressure field using the momentum equation, then apply boundary conditions again. 13) Complete the Lagrangian step updating the internal energy with the field pressure, and then move the mesh vertices with the fluid. 14) Mesh Rezoning : Vertices are moved with arbitrary velocities in order to: i) prevent the mesh from undergoing large distortions, ii) be able to resolve the different length scales involved int the integration domain, (donor cell scheme used) iii) and to change boundary conditions if any solid cell converts into gas cell (due to combustion). 15) Update thermodynamics, transport and chemical kinetics. 16) Swap vectors and repeat time marching ( steps 3 to 15 ) until solution is completed, that is when the propellant finishes. where: (u,v) = vertex velocity p = cell pressure e = cell internal energy E.O.S. = equation of state

 May 4, 2001, 14:20 Re: rocket internal flow simulation #2 Dean Guest   Posts: n/a There are two things in your problem that are challenging. First, the low Mach number requires setting very tight limits on the pressure iteration. A good rule of thumb is that the relative error in the pressure field, abs(dP/P), must be less than the square of the Mach number. So for Mach 1.e-3, the pressure must be iterated to one part in a million. A safety factor of 0.1 is not a bad idea, just to make sure. Note that this requires that you run with 8 bytes in a floating point number (double precision on most computers) since 4 bytes gives you only about 6 significant figures. Also, ICE can have convergence problems for CFL numbers greater than about 10 for the SOR implementation. Second, the 1:1000 aspect ratio could be causing a lot of your trouble. I have experienced this, but I don't have a fix for it other than to use a less extreme grid. You might want to run some numerical experiments with ratios down around 10 or less to see if that helps. Hope this helps.

 May 4, 2001, 16:44 Re: ICE & rocket internal flow simulation #3 Andres Peratta Guest   Posts: n/a Thanks a lot for your response. The rule [abs(dp/p)< M**2] was of great help for me. Respect to the CFL number, you were absolutely rigth: I could reach a CFL number of around 10, and when I try to use greater CFL values then convergence begins to fail. I'll follow your advice, and run numerical experiments with lower cell's aspect ratio. best regards, Andres

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post andrenonaka CFX 14 December 7, 2015 01:42 SimonH. OpenFOAM 0 October 27, 2009 05:39 Kishore FLUENT 1 July 10, 2007 11:42 Kishore FLUENT 8 June 6, 2007 12:17 Axel Rohde Main CFD Forum 1 November 19, 2001 13:19

All times are GMT -4. The time now is 10:00.