Hi, I am trying to implement a moving mesh model which has 5 sliding interfaces using ASI in parallel mode in linux. It is a huge model with around 5000000 cells. I have divided the mesh manually into 8 sets ensuring that the attach boundaries at an interface are in the same set. I run the moving mesh on a separate node and so in total use 9 nodes for processing. But after the code runs for about 1000 secs it errors out saying sigkill signal has been sent from the node running the moving mesh. When I check the mvmesh.log file I find that star-cd has defined some parameters as given below which I have not defined either in the macro file nor in the .cgrd file.

*SET ITER 0 0.0

*SET EVNO -1 0.0

*SET EVEX 1 0.0

*SET LSTP 1 0.0

*SET TIME 0.00000000 0.0

*SET ETIM -1.0000000 0.0

*SET YPST 0.00000000 0.0

Also there is no further use of these parameters in the mvmesh.log file. The events run as defined once for time=0 and then it stops. I would be grateful if anybody could help me out.

Regards

Huge is a relative thing. Now days some folks think 5M cells is normal. And a few think that's small!

Those parameters are generated by STAR to assist in the event process. It is up to the user to do something with them.

Going from memory, I believe they are:

ITER = current iteration

EVNO = next event to be executed

EVEX = last event executed

LSTP = current load step - from the old multi-step transient approach

TIME = current simulation time

ETIME = time next event occurs

YPST = Piston position - for IC engine jobs - works with the evparm,piston command

Since your run goes for 1000sec, you must have a bunch of stuff correct. Having the moving grid node sigkill makes me suspect your grid change commands did something ugly. Hard to say without knowing the specifics. Does the problem repeat? Does it repeat at exactly the same time? Is it near or past your last event? I would be looking for something that creates a divide by 0 or array out of bounds type condition.

Hi,

Thanks for helping me out in understanding the variables. The error actually was a pretty stupid mistake in the moving mesh commands. The model is running now.

Hello Mr. Karteek, I am also trying to do moving mesh in parallel mode, could you please help me on SETS, how to do manual sets. Which command do i have to use (like decompmethod = sets..) model has about 180000 cells.

thanks an advance for your help.

Hi, You would need to manually define sets using prostar with the setw command ( try help setw). Once you define them a file casename.set is created. While using star when you use decompmeth=s star-cd uses the .set file