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 timestep size present relaxation factor omega= 3.000E01 present timestep size delt= 1.107E02 maximum residual= 1.45033E+36 at i= 2 j= 201 k= 3 ****** t= 1.1068E02 cycle= 1 iter= 314 delt= 1.1068E02 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. 1e10. 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 : FLOW3D 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 4.43E02/cy 1.00E10 3.96E+05 1.1E+01 23:45:22 *** pressure iteration diverging  restarting cycle with smaller omega and timestep size t= 6.5090E08 cycle= 72 iter= 319 delt= 3.1948E09 block 1 *** pressure iteration diverging  restarting cycle with smaller omega and timestep size t= 7.4608E08 cycle= 83 iter= 316 delt= 1.3660E09 block 1 *** pressure iteration diverging  restarting cycle with smaller omega and timestep size t= 9.4526E08 cycle= 111 iter= 313 delt= 1.3388E09 block 1 *** pressure iteration diverging  restarting cycle with smaller omega and timestep size t= 1.1542E07 cycle= 140 iter= 312 delt= 1.3776E09 block 1 *** pressure iteration diverging  restarting cycle with smaller omega and timestep size t= 1.3551E07 cycle= 168 iter= 310 delt= 1.3501E09 block 1 *** pressure iteration diverging  restarting cycle with smaller omega and timestep size t= 1.5520E07 cycle= 196 iter= 310 delt= 1.3232E09 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 multiblock 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 FLOW3D 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 
All times are GMT 4. The time now is 09:08. 