Hi Guys! Glenn, Neale, Bob. Many thanks for you help. Without your input it would be impossible to do much at all. I did some validation study of a two element wing for which I had wing MIRA tunnel data. Data was not very "clean" as wing was mounted on a single seater car which was tested with and without wing. So it was actually a good reliable data of how thing wing worked on THIS car. How ever as I didn't have anything better I decided that I'd try anyway. I understand that it's much better to start validating my results on something like Ahmed body – I will do it anyway but it looked much more boring that nice rear wing . I used a mesh consisting of 1800000 elements and results was within 8% for lift and 17% for drag. Used SST model. Flour, side wall and top wall set as free slip. Now I'm trying to model the flow around a (generic but fairly close) sports racer body. I started with flat bottom (no rake) and got positive lift as expected. Than I added healthy front splitter and lift was reduced and center of pressure moved forward (it was far rear) Than I added a rear diffuser only to find that it doesn't really work. At first I had more lift than with flat bottom. After some tweaking of diffuser shape and I managed to reduce lift some more but still it was lift. Now I recreated (fairly close) underbody of 92 group C Toyota sports prototype (a car that produced tons of negative lift. I'm at the closing stages of convergence (2.2e-4) and forces seem to stabilize. Still there's lift…. Not much 155N (still falling but very slowly) for a half car but I expected some down force using a proved design (which was disallowed by tech reg. for creating too much downforce!) Point is I'd like to ask for some good (ball park) guidance for how to model this kind of solution. What is suggested minimum quantity of elements for a roughly 3.5m long , 1.7m wide car body? Fluid domain is 11m long, 2.5m wide and 2.5m tall (half symmetry model). I use around 2000000 elements. If to ask this question from other end what is recommended edge length scale for background and model? I use 0.3m for background with MC of 0.02m for model. I use 5 layers for inflation, Proximity set at 5 for edge (surface not checked). I used free slip for ground plane ( think I have to change it for moving wall with same speed as "free stream" ) I use SST with 1% (low intensity) turbulence option.

So questions are – 1) recommendations for mesh. 2) recommendations for physics settings (with "ground effect" in mind) Machine I'm working on has 2Gb RAM. I had not problems to solve 2350000 elements and it was showing 1.4Gb mem usage. But when I tried to solve a problem with 2550000 elements it said that there's not enough memory…. Strange!

Thank you Ted

1. Mesh

With 2GB of ram you will be limited to ~ 500,000 nodes on a hybrid/unstructured grid (CFX-5 uses about 2000 bytes/node on this kind of grid). This may not be enough to accurately model the flow around you geometry. When you tried the 2550000 element problem (~ 600,000) nodes the flow solver could not allocate enough memory. One other option is to run in parallel and make use of another machine, if you have that capability.

Recommendations for the grid are as we have already said. Make sure you have enough grid in the boundary layer, make sure you resolve separation regions, etc.. etc..

You might do a mesh coarsening study as well. i.e. create a 400,000 and maybe a 200,000 node mesh and see if the lift/drag answers change. How much they are changing will indicate if you are geting towards some sort of mesh independence (or not). You can use richardson extrapolation (do a search on the net for Patrick Roache) to "estimate" values of lift and drag on a more refined mesh if you have numbers for the coarser grids as well.

2. Physics

Yes, use a no-slip moving wall for the ground.

If your side wall is cutting the car in half, use a symmetry plane instead of free slip condition. Should disturb the flow less and you will get proper gradients. You get extrapolated (from the interior) gradients when you use a free-slip condition.

If you can cut the geometry in half, using symmetry, you should do this. You can use two times the number of nodes then.

If you are not getting the expected downforce then you should look closely at why. Is the incoming flow angle all wrong? Is the flow separated? etc... It might be a simple model setup error causing the unexpected result, rather than the mesh.

Neale

Hi Neale, Ted,

I might add that I have also seen some strange behavior on CFX5.6 with Intel/Windows machines with large jobs on single processor which I don't quite understand. My machine is a dual processor 2GB machine, but I cannot run a single processor job larger than about 1.4GB. I don't know why it can't use more of the available memory. The same job in parallel would work fine up to (and even slightly over) my available RAM.

Any explanations for this? I know a single process is limited to about 2GB due to the 32 bit width, but why is it limited to only about 75% of this?

Glenn

Hi Neale, Glen,

Thank you Neal, I used "free slip" for ground plane... may that caused strange results. I'll try a moving wall now. Never did it before. I set to Cartesian U = 44.72ms^-1 V = 0 W = 0 Didn't find a clear explenation what is it but set is as by err... feeling! Am I wrong here? Also I set Global initialisation (never used it before also) to Cartesian auto with value with same values as above.... They did so in manual for Tutorial5.

Please correct me if you I'm wrong here.

Glen, That's exactly what happens here little over 1.4Gb is maximum (600000+ nodes) 700000 nodes - not enough memory... strange. I'll ask if I can use another PC (ther is one in the same room so to try and run it parallel.

So 5 - 600000 nodes is not enough to resolve (with acceptable results accuracy) a car body?

Thank you Ted

Some more questions regarding mesh "size" What values you suggest for edge lengh sacale? 1) Background 2) Areas of interest

a) underbody or parts of it such as diffuser etc.

b) Wing

c) Other areas?

Currently I'm using 0.3m for background and 0.02m for all car model - didn't spatate it in multiple (different value) mesh controls. Does those values sound like too coarse to hope for reasonably accurate results?

Thank you Ted

Well, I feel that something is wrong with my simulations... I could not get any negative lift using "proven" tricks like diffusers etc. I had +/- 100N of lift at best (half car) I than added a rear wing and suddenly got 1470 N of negative lift (44.72ms^-1, half car) hmmm.... seem a bit too much and most of all the difference is too big... Yes the wing is a well proven two element profile and it does interact with tunnels helping each other... still I'm afraid that something I'm doing wrong…. I'd like to post my out file so I you guys could take a good look at it – may be there's something I'm missing.

Thank you Ted LIBRARY :

MATERIAL : Air Ideal Gas

Option = Pure Substance

Thermodynamic State = Gas

Long Name = Air Ideal Gas (constant Cp)

PROPERTIES :

Option = Ideal Gas

Molar Mass = 28.96 [kg kmol^-1]

Dynamic Viscosity = 1.79e-05 [kg m^-1 s^-1]

Specific Heat Capacity = 1000.0 [J kg^-1 K^-1]

Thermal Conductivity = 0.0252 [W m^-1 K^-1]

Absorption Coefficient = 0.01 [m^-1]

Scattering Coefficient = 0.0 [m^-1]

Refractive Index = 1.0 [m m^-1]

Reference Pressure = 1 [atm]

Reference Temperature = 0 [K]

Reference Specific Enthalpy = 0. [J/kg]

Reference Specific Entropy = 0. [J/kg/K]

END

END END EXECUTION CONTROL :

PARALLEL HOST LIBRARY :

END

PARTITIONER STEP CONTROL :

Runtime Priority = Standard

MEMORY CONTROL :

Memory Allocation Factor = 1

END

PARTITIONING TYPE :

MeTiS Type = k-way

Option = MeTiS

Partition Size Rule = Automatic

END

END

RUN DEFINITION :

Definition File = SP1Gen8.def

Run Mode = Full

END

SOLVER STEP CONTROL :

Runtime Priority = Standard

EXECUTABLE SELECTION :

Double Precision = Off

Use 64 Bit = Off

END

MEMORY CONTROL :

Memory Allocation Factor = 1

END

PARALLEL ENVIRONMENT :

Option = Serial

Parallel Mode = PVM

END

END END FLOW :

SOLUTION UNITS :

Angle Units = [rad]

Length Units = [m]

Mass Units = [kg]

Solid Angle Units = [sr]

Temperature Units = [K]

Time Units = [s]

END

SIMULATION TYPE :

Option = Steady State

END

DOMAIN : SP1Gen8 3D

Coord Frame = Coord 0

Domain Type = Fluid

Fluids List = Air Ideal Gas

Location = SP1Gen8 3D

DOMAIN MODELS :

BUOYANCY MODEL :

Option = Non Buoyant

END

DOMAIN MOTION :

Option = Stationary

END

REFERENCE PRESSURE :

Reference Pressure = 100000 [Pa]

END

END

FLUID MODELS :

COMBUSTION MODEL :

Option = None

END

HEAT TRANSFER MODEL :

Fluid Temperature = 288 [K]

Option = Isothermal

END

THERMAL RADIATION MODEL :

Option = None

END

TURBULENCE MODEL :

Option = SST

END

TURBULENT WALL FUNCTIONS :

Option = Automatic

END

END

BOUNDARY : Inlet

Boundary Type = INLET

Location = Inlet

BOUNDARY CONDITIONS :

FLOW REGIME :

Option = Subsonic

END

MASS AND MOMENTUM :

Normal Speed = 44.72 [m s^-1]

Option = Normal Speed

END

TURBULENCE :

Option = Low Intensity and Eddy Viscosity Ratio

END

END

END

BOUNDARY : Outlet

Boundary Type = OUTLET

Location = Outlet

BOUNDARY CONDITIONS :

FLOW REGIME :

Option = Subsonic

END

MASS AND MOMENTUM :

Option = Average Static Pressure

Relative Pressure = 0 [Pa]

END

END

END

BOUNDARY : FreeWalls

Boundary Type = WALL

Location = FreeWalls

BOUNDARY CONDITIONS :

WALL INFLUENCE ON FLOW :

Option = Free Slip

END

END

END

BOUNDARY : Ground

Boundary Type = WALL

Location = Ground

BOUNDARY CONDITIONS :

WALL INFLUENCE ON FLOW :

Option = No Slip

WALL VELOCITY :

Option = Cartesian Components

Wall U = 44.72 [m s^-1]

Wall V = 0 [m s^-1]

Wall W = 0 [m s^-1]

END

END

END

END

BOUNDARY : SymP

Boundary Type = SYMMETRY

Location = SymP

END

BOUNDARY : SP1Gen8

Boundary Type = WALL

Location = SP1Gen8

BOUNDARY CONDITIONS :

WALL INFLUENCE ON FLOW :

Option = No Slip

END

END

END

END

INITIALISATION :

Option = Automatic

INITIAL CONDITIONS :

Velocity Type = Cartesian

CARTESIAN VELOCITY COMPONENTS :

Option = Automatic with Value

U = 44.72 [m s^-1]

V = 0 [m s^-1]

W = 0 [m s^-1]

END

EPSILON :

Option = Automatic

END

K :

Option = Automatic

END

STATIC PRESSURE :

Option = Automatic

END

END

END

SOLVER CONTROL :

ADVECTION SCHEME :

Option = High Resolution

END

CONVERGENCE CONTROL :

Maximum Number of Iterations = 100

Physical Timescale = 0.1 [s]

Timescale Control = Physical Timescale

END

CONVERGENCE CRITERIA :

Residual Target = 1.E-4

Residual Type = RMS

END

DYNAMIC MODEL CONTROL :

Global Dynamic Model Control = Yes

END

END END COMMAND FILE :

Version = 5.6

Results Version = 5.6 END

+--------------------------------------------------------------------+ | | | Solver | | | +--------------------------------------------------------------------+

+--------------------------------------------------------------------+ | | | CFX-5 Solver 5.6 | | | | Version 2003.04.29-23.00 Tue Apr 29 23:41:39 2003 | | | | Executable Attributes | | | | single-32bit-optimised-supfort-noprof-nospag | | | | Copyright 1996-2003 CFX Limited. | +--------------------------------------------------------------------+

+--------------------------------------------------------------------+ | Job Information | +--------------------------------------------------------------------+

Run mode: serial run

Host computer: USER-R7TZKA1AGL Job started: Tue Mar 23 13:32:50 2004

+--------------------------------------------------------------------+ | Memory Allocated for Run (Actual usage may be less) | +--------------------------------------------------------------------+

Data Type Kwords Words/Node Words/Elem Kbytes Bytes/Node

Real 172635.8 340.11 85.48 674358.7 1360.45 Integer 69909.9 137.73 34.62 273085.4 550.92 Character 1459.5 2.88 0.72 1425.3 2.88 Logical 40.0 0.08 0.02 156.2 0.32 Double 908.0 1.79 0.45 7093.8 14.31

+--------------------------------------------------------------------+ | Total Number of Nodes, Elements, and Faces | +--------------------------------------------------------------------+

Domain Name : SP1Gen8 3D

Total Number of Nodes = 507584

Total Number of Elements = 2019493

Total Number of Tetrahedrons = 1604900

Total Number of Prisms = 409696

Total Number of Pyramids = 4897

Total Number of Faces = 103601

+--------------------------------------------------------------------+ | Average Scale Information | +--------------------------------------------------------------------+

Domain Name : SP1Gen8 3D

Global Length = 4.0620E+00

Maximum Extent = 1.1000E+01

Density = 1.2094E+00

Dynamic Viscosity = 1.7900E-05

Velocity = 4.4720E+01

Advection Time = 9.0833E-02

Reynolds Number = 1.2273E+07

Speed of Sound = 3.4057E+02

Mach Number = 1.3131E-01

================================================== ==================== OUTER LOOP ITERATION = 41 CPU SECONDS = 9.57E+03 ---------------------------------------------------------------------- | Equation | Rate | RMS Res | Max Res | Linear Solution | +----------------------+------+---------+---------+------------------+ | U-Mom | 0.93 | 1.0E-04 | 8.1E-03 | 1.2E-02 OK| | V-Mom | 0.93 | 3.6E-05 | 1.9E-03 | 2.8E-02 OK| | W-Mom | 0.94 | 3.4E-05 | 1.5E-03 | 2.0E-02 OK| | P-Mass | 0.93 | 6.8E-06 | 3.4E-04 | 9.0 2.2E-02 OK| +----------------------+------+---------+---------+------------------+ | K-TurbKE | 0.92 | 1.5E-04 | 1.7E-02 | 5.5 2.3E-02 OK| +----------------------+------+---------+---------+------------------+ | O-TurbFreq | 0.93 | 1.3E-05 | 1.3E-03 | 12.4 1.7E-03 OK| +----------------------+------+---------+---------+------------------+

CFD Solver finished: Tue Mar 23 16:19:02 2004 CFD Solver wall clock seconds: 9.9340E+03

Execution terminating: all RMS residual AND global imbalance are below their target criteria.

================================================== ====================

Boundary Flow and Total Source Term Summary ================================================== ====================

+--------------------------------------------------------------------+ | U-Mom | +--------------------------------------------------------------------+ Boundary : Ground 4.4343E+00 Boundary : Inlet 1.5908E+04 Boundary : Outlet -1.5237E+04 Boundary : SP1Gen8 -6.7562E+02 Boundary : SymP 3.2384E-14

----------- Domain Imbalance : -1.3428E-03

Domain Imbalance, in %: 0.0000 %

+--------------------------------------------------------------------+ | V-Mom | +--------------------------------------------------------------------+ Boundary : FreeWalls 6.6834E+02 Boundary : Ground -2.1417E+03 Boundary : Inlet 4.8196E-02 Boundary : Outlet 1.0273E+02 Boundary : SP1Gen8 1.3707E+03 Boundary : SymP -1.9552E-14

----------- Domain Imbalance : 1.0596E-01

Domain Imbalance, in %: 0.0007 %

+--------------------------------------------------------------------+ | W-Mom | +--------------------------------------------------------------------+ Boundary : FreeWalls 9.7787E+02 Boundary : Ground 2.7671E+00 Boundary : Inlet -7.5328E-05 Boundary : Outlet 8.4205E+01 Boundary : SP1Gen8 -6.8101E+02 Boundary : SymP -3.8448E+02

----------- Domain Imbalance : -6.4325E-01

Domain Imbalance, in %: -0.0040 %

+--------------------------------------------------------------------+ | P-Mass | +--------------------------------------------------------------------+ Boundary : Inlet 3.3845E+02 Boundary : Outlet -3.3845E+02

----------- Domain Imbalance : -8.2397E-04

Domain Imbalance, in %: -0.0002 %

================================================== ====================

Wall Force and Moment Summary ================================================== ====================

Note: Pressure integrals exclude the reference pressure. To include

it, set the expert parameter 'include pref in forces = t'.

+--------------------------------------------------------------------+ | Pressure Force On Walls | +--------------------------------------------------------------------+

X-Comp. Y-Comp. Z-Comp. FreeWalls 0.0000E+00 -6.6837E+02 -9.7786E+02 Ground 0.0000E+00 2.1417E+03 0.0000E+00 SP1Gen8 6.4576E+02 -1.3732E+03 6.8027E+02

+--------------------------------------------------------------------+ | Viscous Force On Walls | +--------------------------------------------------------------------+

X-Comp. Y-Comp. Z-Comp. FreeWalls 0.0000E+00 3.2591E-02 -7.6426E-03 Ground -4.4343E+00 -2.0795E-04 -2.7671E+00 SP1Gen8 2.9863E+01 2.4558E+00 7.4443E-01

+--------------------------------------------------------------------+ | Pressure Moment On Walls | +--------------------------------------------------------------------+

X-Comp. Y-Comp. Z-Comp. FreeWalls -1.5354E+02 3.0369E+03 -2.7937E+03 Ground -2.0808E+03 0.0000E+00 4.9514E+03 SP1Gen8 7.0814E+02 4.1478E+02 -1.9594E+03

+--------------------------------------------------------------------+ | Viscous Moment On Walls | +--------------------------------------------------------------------+

X-Comp. Y-Comp. Z-Comp. FreeWalls 9.9285E-04 4.2500E-02 1.8558E-01 Ground 1.4069E-01 7.1819E+00 -2.2568E-01 SP1Gen8 -7.0144E-01 1.8395E+01 -1.2665E+01

+--------------------------------------------------------------------+ | Locations of Maximum Residuals | +--------------------------------------------------------------------+ | Equation | Node # | X | Y | Z | +--------------------------------------------------------------------+ | U-Mom | 42991 | 1.625E+00 | 6.055E-01 | 8.500E-01 | | V-Mom | 197012 |-1.188E+00 | 4.554E-01 | 9.023E-01 | | W-Mom | 21040 | 2.302E-01 | 6.401E-01 | 5.685E-02 | | P-Mass | 18801 |-1.164E+00 | 9.913E-02 | 8.710E-01 | | K-TurbKE | 231908 |-2.227E+00 |-7.127E-03 | 1.482E-01 | | O-TurbFreq | 138205 | 1.624E+00 | 6.054E-01 | 8.497E-01 | +--------------------------------------------------------------------+

+--------------------------------------------------------------------+ | Peak Values of Residuals | +--------------------------------------------------------------------+ | Equation | Loop # | Peak Residual | Final Residual | +--------------------------------------------------------------------+ | U-Mom | 3 | 2.55572E-02 | 9.98007E-05 | | V-Mom | 3 | 1.49114E-02 | 3.55704E-05 | | W-Mom | 3 | 3.05907E-03 | 3.36187E-05 | | P-Mass | 1 | 1.82491E-02 | 6.81435E-06 | | K-TurbKE | 1 | 1.61058E-01 | 1.54667E-04 | | O-TurbFreq | 1 | 2.48693E-02 | 1.30758E-05 | +--------------------------------------------------------------------+

+--------------------------------------------------------------------+ | False Transient Information | +--------------------------------------------------------------------+ | Equation | Type | Elapsed Pseudo-Time | +--------------------------------------------------------------------+ | U-Mom | Physical | 4.10000E+00 | | V-Mom | Physical | 4.10000E+00 | | W-Mom | Physical | 4.10000E+00 | | P-Mass | Physical | 4.10000E+00 | | K-TurbKE | Physical | 4.10000E+00 | | O-TurbFreq | Physical | 4.10000E+00 | +--------------------------------------------------------------------+

+--------------------------------------------------------------------+ | Average Scale Information | +--------------------------------------------------------------------+

Domain Name : SP1Gen8 3D

Global Length = 4.0620E+00

Maximum Extent = 1.1000E+01

Density = 1.2038E+00

Dynamic Viscosity = 1.7900E-05

Velocity = 4.3168E+01

Advection Time = 9.4097E-02

Reynolds Number = 1.1793E+07

Speed of Sound = 3.4057E+02

Mach Number = 1.2676E-01

+--------------------------------------------------------------------+ | Variable Range Information | +--------------------------------------------------------------------+

Domain Name : SP1Gen8 3D +--------------------------------------------------------------------+ | Variable Name | min | max | +--------------------------------------------------------------------+ | Velocity u | -4.19E+01 | 8.30E+01 | | Velocity v | -4.97E+01 | 5.25E+01 | | Velocity w | -5.33E+01 | 5.28E+01 | | Pressure | -3.86E+03 | 2.22E+03 | | Dynamic Viscosity | 1.79E-05 | 1.79E-05 | | Specific Heat Capacity at Constant Pressure| 1.00E+03 | 1.00E+03 | | Thermal Conductivity | 2.52E-02 | 2.52E-02 | | Density | 1.16E+00 | 1.24E+00 | | Isothermal Compressibility | 1.21E-05 | 1.21E-05 | | Static Entropy | 2.35E+03 | 2.37E+03 | | Turbulence Kinetic Energy | 9.44E-04 | 1.52E+02 | | Turbulence Eddy Frequency | 5.82E+01 | 1.03E+06 | | Eddy Viscosity | 8.92E-07 | 2.15E-01 | | Temperature | 2.88E+02 | 2.88E+02 | | Wall Scale | -1.28E-03 | 2.86E+00 | | Wall Distance | 1.00E-20 | 2.27E+00 | +--------------------------------------------------------------------+

+--------------------------------------------------------------------+ | CPU Requirements of Numerical Solution | +--------------------------------------------------------------------+

Subsystem Name Discretization Linear Solution

(secs. %total) (secs. %total) ---------------------------------------------------------------------- Wall Scale 1.24E+02 1.5 % 1.67E+02 2.0 % Momentum and Mass 4.41E+03 53.2 % 1.02E+03 12.3 % TurbKE and TurbFreq 1.38E+03 16.7 % 1.18E+03 14.2 %

-------- ------- -------- ------ Summary 5.92E+03 71.4 % 2.37E+03 28.6 %

+--------------------------------------------------------------------+ | Job Information | +--------------------------------------------------------------------+

Host computer: USER-R7TZKA1AGL Job finished: Tue Mar 23 16:19:33 2004 Total CPU time: 9.820E+03 seconds

or: ( 0: 2: 43: 40.219 )

( Days: Hours: Minutes: Seconds )

Total wall clock time: 1.000E+04 seconds

or: ( 0: 2: 46: 43.000 )

( Days: Hours: Minutes: Seconds )

End of solution stage.

+--------------------------------------------------------------------+ | The results from this run of the CFX-5 solver have been written to | | D:\SPP01\SP1Gen_CFD\SP1Gen8\SP1Gen8_002.res | +--------------------------------------------------------------------+

Hi Ted,

In regards to your question about how mant elements to use:

You have to determine that as it is highly problem dependant. I assume from your posts that drag and lift are the values of interest - that means you keep increasing the mesh size until the drag and/or lift does not change with different meshes.

As has been commented on a previous posting, if you are modelling a car body at car speeds, getting good drag prediction is difficult, and you almost certainly will need a simulation big enough that you will need several computers in parallel. Lift should be a bit easier.

Glenn

Guys,

The answer is pretty easy to the Windows 1.4-1.5 GB limit.

- The OS takes up space: daemons, services, fonts, etc... - Device drivers take up space: video, sound, disk, serial ports, parallel ports, etc...

If you want more space make sure you aren't running anything, delete a bunch of fonts, and then create a hardware profile where you disable everything except the bare bones of what you need, then reboot with that profile.

Neale

Just to add to the windows memory stuff. When you run in serial the flow solver allocates one big chunk. When you run in parallel the flow solver allocates two smaller chunks which "fit" easier into the windows memory space.

This is not a CFX problem. It's windows really. Although you might argue it's a CFX problem because of the architecture they use. i.e. allocate one big chunk of ram at the beginning of the run rather than allocating it on the fly. Then again, allocating on the fly has it's own problems, eg, not freeing memory, overwriting memory, etc...

Neale

Neal, Any ideas how to disbale the non such in windows or linux to free more memory for simulations ?

Hi Neale,

I know there is more to it than that. The OS shuffles non-important things out to the swap file, leaving the core memory for whatever is currently running. Even though the device drivers all take up space, it is space on the swap file not core memory.

The issue is that for a given simulation which requires (say) 1.9GB of RAM, it will not run in serial on a WinXP dual processor machine, but it will run in parallel on the same machine locally. On the parallel run the total memory requirement is in fact marginally greater (maybe 2.0GB total), but the individual processes are about 1GB.

And another thing: 2^32=4E9, so why is it a 2GB limit where 32 bits should give you 4GB?

Glenn

Thanks Glen, Could someone give me an idea for about how much PC power is needed for reasonably accurate Lift and Drag prediction? Best I can get is 3PC's of 2.8 2Gb mem... So question 1) Should I assume that it's impossible to have accurate results with 1.4Gb (available out of total 2Gb if 1PC is used) When I say accurate I mean within 10%. 2) Is there any hope if I use 3PC as mentioned above?

Thank you Ted

Not all device drivers and Windows system files are swapped out. Some permanently remain in memory but not necessarily in contiguous memory space. i.e you could have a memory layout like:

system files:free space1:device driver1:more free space2: device driver2

In a serial run "free space1" and free space2" are not big enough, but in a parallel run both are big enough for individual processes. If you have any device drivers that don't get swapped out (this is possible) then a serial run will not work.

Yes 2^32 is 4GB, but the problem is that on windows a 16 byte (32 bit) memory pointer is "signed" (has a sign bit and 31 numeric bits). This gives a range of -2^31->+2^31 (total is 4GB). So, since memory cannot have negative addresses you only get 2^31 accessable.

This is not just on Windows, it's pretty much on all 32 bit operating systems.

Neale

Tudor, this is so problem dependent that it is pretty much impossible to answer. All that is true is that you can run about 500k nodes unstructured grid on a 2GB PC with CFX-5. It's unstructured so make sure you get the nodes where you need them (i.e. resolving the right flow features).

Also, make sure you do the mesh independence analysis I mentioned earlier and you will know if you are getting to the right answer.

Head over to the NPARC Alliance website. They talk about Paul Roache's richardson extrapolation. If you do this on a few mesh sizes you can determine if you are at least 'asymptotically' approacing the answer that CFX-5 is going to get. What is nice about this stuff is even if you can only run say 200k nodes, 350k nodes, and 550k nodes you can estimate the 1million node answer within a couple of percent as long as the 200k, 350k and 550k node runs were in the asymptotic range (i.e. already smoothly approaching the final answer that CFX-5 would get if you kept further refining the mesh).

Neale

Here are the NPARC links I mentioned:

http://www.grc.nasa.gov/WWW/wind/valid/validation.html

http://www.grc.nasa.gov/WWW/wind/val.../tutorial.html

On the second link, pay particular attention to section 8.

Neale

Hey Tudor, how has the changes to the model gone ? has their been any improvements to the results ? Just curious having followed your posts etc. I should imagine the change on ground boundary condition will have a big effect ??? Bob