How do I use the restart analysis in v3.10? I have run a transient analysis of 10000 time steps for a total time of 1 second real time. I now want to use the calculated cell data from the end of last time step and continue with the simulation for another 1 second and 10000 time steps.

Use RDAT REST, and set up a new load step for the second second. Run only load step 2.

Thanks Brian, I'll give that a try but I don't expect it to work since I am not using load steps, but only time steps wherby the inlet boundary conditions change with time by use a table that is read in. What is a load step?

(Is your full name Brian Canoo by anychance?)

Yes, close enough. <grin>

If you're running transient in V3.1x, you're using load steps, believe it or not.

But if you've used "single load step" up to now, it can be hard to get it restarted. What I would suggest is starting a new run, after backing up your .pstt and .pst files. Use the existing .pst file as an initial field (RDAT INIT) and run as before.

Dear sirs,

When I run a transient simulation, it appeared the follow erro!What is the problem?Thank you first.

*** BCDEFI called for boundary *** BCDEFI called for boundary

1 0.00E+00 0.00E+00 0.00E+00 0.00E+00 0.00E+00 0.00E+00 0.00E+00 0.00E+00 0.00E+00 0.00E+00 0.00E+00 0.00E+00 0.00E+00 2.00E+01

0.00E+00 0.00E+00 0.00E+00 0.00E+00 0.00E+00 0.00E+00 0.00E+00 0.00E+00 0.00E+00 0.00E+00 0.00E+00 0.00E+00 0.00E+00 0.00E+00 Warning - server not running, no information sent to starwatch. &&&& -------------------------------------------------------------- --------- -----------------------------------------------------

*** SOLUTION DIVERGES/UNSTABLE.

*** CALCULATIONS TERMINATED; NEW FILE.div WRITTEN

END OF EXECUTION - STAR ELAPSED TIME IS 0.30 CPU TIME IS 0.20

The fact that EVERYTHING is zero in your residuals and monitoring cell most likely indicates that there is no flow at all.

As you're using user coding for your inlet boundary, I would suspect that first. Are you sure that it is calculating actual values? Put a write statement in the user coding (temporarily) to see whether it is actually producing what you expect.

Dear Brian,

I have put write statment "*** BCDEFI called for boundary *** BCDEFI called for boundary " in user subroutine ,and it appeared above the calculation as you can see.

I am trying to model the ocean wave motion,and I am bothered if anyelse is needed since the free surface (water -air) is varying as sine-wave.I only take the transient inlet into account in this case. Should I need put the NEWXYZ subroutine into account? The inlet boundary is varing with TIME ,X and Y.

No, no need for NEWXYZ as you're not moving the mesh.

But write some of the variables like U, V, SCALAR(1) out as well, to see what is being calculated.

Brian Yes, i am using a single load step. I backup up my *.pst file and run a restart analysis with initial field command RDAT INIT. The problem is that the program did not use the previous bondary values to use as staring point on next run. (I can't see any difference in the data between the two runs as i should seen) It ssems to have used the initlal Flow Initialisation for AIR that I defined at start of first run with (init,stan,... ) Thanks for help

It's probably just started at time=0 again. and your boundary condition calculations are based on time. A slight modification to your user coding should fix that. Maybe not the most elegant solution, but a good quick-fix.

Thanks for all help Brian. I managed to solve the problem. I just had to copy only *.pst and *.mdl file to new directory and then restart with initialisation. Also had to change my input time sothat it does not start from time zero, but from last time step.

Dear Brian,

In star-cd ,do scalar(1) represent the F function in VOF method? I try as you said ,but it doesn't go,I do not know the reason!

In my problem,d=water depth, TW=(wave period) dY=cell height in y direction. wh=wave height. The free surface function :

y1= wh*cos(kwa*X-fht*TIME)/2

And now I paste my coding here!Can you tell me what's the matter? Looking forward to receive from you! Here is the codinginlet coding)

PARAMETER(TW=2.5)

PARAMETER(d=1.5)

PARAMETER(wh=1)

PARAMETER(pie=3.141)

PARAMETER(g=9.18)

PARAMETER(dY=0.3)

IF(IREG.EQ.1) THEN

kwa=2*pie/L

fht=2*pie/TW

fhw=pie*wh/TW

fhtw=d+wh*cos(kwa*X-fht*TIME)/2

fhtz=max(fhtw-Y,zero)/dY

fthz=min(fhtz,one)

If(fhtz.gt.small)Then

SCALAR(1)=fthz

U=fhw*cosh(kwa*Y)*cos(kwa*X-fht*TIME)/sinh(kwa*d)

V=fhw*sinh(kwa*Y)*sin(kwa*X-fht*TIME)/sinh(kwa*d)

W=0

ELSE

SCALAR(1)=0

U=0

V=0

ENDIF

ENDIF C-------------------------------------------------------------------------

WRITE(6,*) "*** BCDEFI called for boundary "

RETURN

END

Blackhole - this goes way past the sort of help you should expect from a public forum. Maybe it's time to contact your official support channels.

But I still don't understand why you don't put a statement like this in there:

WRITE(6,*) U,V,W,SCALAR(1)

just to see if you're getting the values you expect.

Dear Brian, Thank you for your kindness.I will try!