an error
 

hi
i am trying to simulate a boat on a free surface , but when the software begins i am getting this error

pressure iteration diverging - restarting cycle with smaller omega and time-step size present relaxation factor omega= -3.000E-01
present time-step size delt= 1.107E-02
maximum residual= 1.45033E+36 at i= 2 j= 201 k= 3
******
t= 1.1068E-02 cycle= 1 iter= 314 delt= 1.1068E-02 block 1
******
excessive pressure convergence failures -- calculation terminated
end of calculation at t= 0.000E+00 cycle = 1
excessive pressure convergence failures
elapsed time (seconds) = 2.560E+02
cpu= 1.555E+03


the boat is 1 meter from the sea ( no contact)



thanks

If you see the error message right at the beginning of the simulation, please try specifying a smaller initial time step. The other thing is you may use a bigger subspace size (mrstrt) of 15 if you are using GMRES pressure solver.

yes i am getting the error in the beginning, i change the initial to 0.00001 and then mrstrt to 15 and then to 20 but the error continued, any other option?

Could you please another even smaller initial time step, ie. 1e-10. If you still see the error, you may need to look at the results, such as pressure, velocity to see if there is anything unphysical.

ok did that , but i still can not get any results....
this is my solver output

Solver starting

program title : FLOW-3D
program version : hydr3d: version 9.3 win64 2008
version id : double
DOUBLE precision version
process identification number for this job= 1


job name: mtfh
problem date: 05/14/2009
problem time: 23:45:1600

Title


************************************************** *****************************
prep3d: version 9.3 win64 2008 warning messages:





*************************************
** warning **
** selected data request for **
** srfht **
** cancelled, name **
** not recognized or duplicate **
*************************************


************************************************** *****************************




*** estimated uncompressed solver output file size (flsgrf): 6 gb ***


*** running parallel code on 8 processors ***

***
restart and spatial data available at t= 0.00000E+00
***

t cycle iter dtstbl/code delt vl cpu clock
--- ----- ---- ----------- ---- -- --- -----
0.00E+00 0 0 4.43E-02/cy 1.00E-10 3.96E+05 1.1E+01 23:45:22
***
pressure iteration diverging - restarting cycle with smaller omega and time-step size
t= 6.5090E-08 cycle= 72 iter= 319 delt= 3.1948E-09 block 1
***
pressure iteration diverging - restarting cycle with smaller omega and time-step size
t= 7.4608E-08 cycle= 83 iter= 316 delt= 1.3660E-09 block 1
***
pressure iteration diverging - restarting cycle with smaller omega and time-step size
t= 9.4526E-08 cycle= 111 iter= 313 delt= 1.3388E-09 block 1
***
pressure iteration diverging - restarting cycle with smaller omega and time-step size
t= 1.1542E-07 cycle= 140 iter= 312 delt= 1.3776E-09 block 1
***
pressure iteration diverging - restarting cycle with smaller omega and time-step size
t= 1.3551E-07 cycle= 168 iter= 310 delt= 1.3501E-09 block 1
***
pressure iteration diverging - restarting cycle with smaller omega and time-step size
t= 1.5520E-07 cycle= 196 iter= 310 delt= 1.3232E-09 block 1

the message you just posted doesnt affect the accuracy of the results. it really matter you see the message you posted on the top.

fyi, the other thing you may think about is to apply some compressibility.

as mentioned, the message could be related to physics process as well. you may need to read the results and see what really went wrong.

hello

thanks a lot for the help, this is the last message that the solver gives me at the end or iterations


1. check for poor mesh aspect ratios. 2. use ADI or GMRES solver.
3. try autot=2.0.
4. increase convergence tolerance epsi.
5. if nmat=1, try some compressibility
by setting rcsql > 0.
6. reduce alphamb for multi-block cases.


any idea???????


thanks a lot

hello eleazar,
are you using an "implicit" method for the GMO? With boats you must use the implicit one (IMPMOB=1), not the explicit, otherwise you may get in errors. If you are using explicit, turn to implicit.

hello

i am using the implicit method, can someone tell me about the units? what kind of units we have in SI????? i believe the units are KG M N SEC, isn't correct???????

yes, it is correct.
Maybe is the mesh: can you describe how did you mesh your problem?

well my ship is 35 meters long and i put it in a mesh of 100 meters to 40 meters and 30 meters high, the mesh is 0.7 meter, the code without the ship is working perfect but when i import the ship it can not solve !!!! shout i use laminar or turbolence?????

I think laminar or turbulent it shouldn't compromise the solution.
You can easily check if the problem is the ship by changing it with a FLOW-3D primitive sphere. Remove the ship and put a sphere.
If with the sphere the simulation is good then the problem is with your ship, otherwise is something else.

dear sir

i did the example with the sphere. after i solve it i delete the GMO and insert the ship model (stl) the simulation is running until the ship hit the water, then the ship shit down for one frame and then moving up the next frame when simulation stops due to the high velocity of the water more than 2million m/sec.... what should i look for this? do you believe it is a moment of inerta error? shall i put the moment of inertia and not the density?

If the simulation with the sphere run correctly then I think it is an error quite easy to identify and solve, once that the Support have the the prepin file and the geometry.
If you have access to the technical support, they'll solve it in few minutes!

i find out what was wrong , i was putting a density mass , went i change it to
center mass , mass, inertia tensor.... it can run perfect...

thanks a lot

With this problem, any one know exactly, how to fix it?
I am doing similar simulation and met the same problem.