Hi, I am making a simulation of a 1m hull form (free surface), at velocity 0.8363m/s which makes Froude number 0.267.

While at simulation the Froude number is different and also changes (1 iteration 0.1718 and then increase/decreases according to wave speed calculated internally).

Is this normal or should the Froude no. remain the same as calculated by me? Since the Froude no. is calculated at such low number then the timestep choosen would also affect the simulation, which it does and end which error message of 'floating point'.

Does anyone have any suggestions?

Thanks in Advance. Joe

Joe

Its worth checking to see what geometric length scale (i.e. hull length) CFX is using to calculate Froude number, as well as the reference location at which the velocity is also taken to compute Froude number. I guess the variation in Froude number during the progression of the simulation is happening as a result of the variation in the velocity at the prescribed reference location for the Froude number calculation (if this happened to be downstream of the vessel, you would expect some variation. If it was at the inlet you would hope it would be fixed!).

The manual does give information on the reference location and geometric length scale's used in its internal calculations.

I hope this helps. James

Hi I checked the dimensions CFX takes for my domain and they differ. My domain has dimensions of x(-2.5,10.5), y(0,1), z(-1,0.5) and CFX co-ordinate frame has [0, 0, 0] so does this mean i have to create a new reference location at [-2.5, 0, 0.5] in order for CFX to calculate correctly the Froude number?

If so, does this happen with the CEL expressions?

Thanks in advance, Joe

I wouldn't worry too much about the CFX calculation of Fn, just set up your own CEL expression using the correct length scale and inlet velocity.

From the output file i get:

Global length 2.3991 Minimum Extent 1 Maximum Extent 13

Domain created is x(-2.5, 10.5)

I need to change the way CFX sees the Domain but does this happen by changing the coordinate frame or what you suggested before?

And also i cant find something about CEL and global length. Can you help some more?

Thanks in Advance

Joe

Like I said before, it's best to set up your own CEL for Froude Number, based on your own characteristic length scale and hull velocity (i.e. inlet velocity). The reason that CFX is not calculating the same Froude number is because it's not using the same length scale as you are.

There are three different length scales which CFX can use:

Lvol = 3√Vol; where Vol is the domain volume.

Lext = max(Lx, Ly, Lz); where Lx, Ly & Lz are the extents of the domain (over all domains).

Lbc = Min√Abc; where Abc is the area of an 'open' boundary (i.e. inlets, outlets or openings).

The internal length scales used when calculating the internal Froude number will depend on length scale option set in the "Solver Control" menu.

Conservative (default):

Lscale = min(Lvol, Lext)

Aggressive:

Lscale = max(Lvol, Lext)

Specified Length Scale:

Lscale = Luser (i.e. set by user)

Therefore, if you set Lscale = hull length, you should get the correct CFX computed Froude number, provided that a consistent velocity scale identical to the hull velocity (i.e. inlet velocity) is being used by CFX.

Creating your own CEL is your best bet if you want to calculate your own Froude number using the correct length/velocity scales. If you've never used CEL to create user functions check the manual. It's pretty straight forward once you've seen someone else's example syntax.

Hope this helps.

James

Thanks for your help James.

Couple of more questions:

1. I am using CFX 5.7 and the operations you mention are not there so are you speaking about another version?

2. In order to create a CEL expression I require to set the length scale as I want it, but how can I do that if I dont know how CFX internally identifies it. I search around the manual and I tried a few variables but no luck.

Any suggestions? Thanks

Joe,

I'm referring to CFX-10, but I think the same internal calculation of length scale is also used in CFX-5.7.1. I can't check, because I've not got CFX-5.7.1 installed.

With regard to the CEL. Just set your own variable for length scale:

UsrLengthScale = 1.0 [m]

UsrHullVelocity = 10 [m s^-1]

UsrFroudeNumber = UsrHullVelocity/√(g*UsrLengthScale)

You can then call "UsrHullVelocity" up when you set the velocity on your inlet boundary.

It's worth installing CFX-10 or even CFX-11 (Preview) if you can, because there are significant improvements with the new free-surface algorithms.

James

Thank you for your help James.

Unfortunately I dont have CFX 10 to use so i ll restrict myself to 5.7

Regards. Joe

Joe

Just download the latest version off the www.ansys.com website using your customer log in.

James