[86lolo]

Hello everyone.

I am trying to model deposition in tube arrays and I need dynamic mesh.
I compile an UDF that works well in serial and crashes in parallel. I tried to correct it by adding the statements #if !RP_HOST and #endif at the beginning and end of the functions, but still does not work in parallel. Tried in Windows and in Linux with similar result. Has anyone a clue about what's wrong?

Mesh is 2D.

The crash error printed in console is is:

Updating mesh to time 1.00000e+00 (step = 00001)... 
999999 (..\src\mpsystem.c@1172): mpt_read: failed: errno = 10054

999999: mpt_read: error: read failed trying to read 4 bytes: No such file or directory
MPI Application rank 0 exited before MPI_Finalize() with status -1073741819
 The fl process could not be started.

Interrupting...
Done.

The UDF is

DEFINE_GRID_MOTION(movimiento02,domain,dt,time,dtime)
{
	#if !RP_HOST
	Thread *tf=DT_THREAD(dt);
	face_t f;
	Node *node_p;
	real theta, y0, x0, y1,A,C,D2,E,F,DR,sy,xcentro,x0prim,x1prim,sx; 
	int n;
	int cil; 
	
	SET_DEFORMING_THREAD_FLAG(THREAD_T0(tf));
	
	node_p=F_NODE(10,tf,0);  /* mesh consists of 6 cylinders, this is to obtain an ID for cylinder by using the function ordinal_cilindro*/
	x0=NODE_X(node_p);
	cil=ordinal_cilindro(x0) ;
	xcentro=(cil-1)*sl_divD*D; /*these are global defined variables*/
	
	
	A=0.004;
	C=-0.00860338434543819;
	D2= 0.00743270295949046;
    	E=-0.00180871094287687;
    	F= 0.000119719241166301;
	/*coefficients to determine the growth of the layer of deposit in a cyinder through a polynomial function*/
	
	begin_f_loop (f,tf)
	{
				
		node_p=F_NODE(f,tf,0);
			
	
			
		NODE_POS_UPDATED(node_p);
		x0=NODE_X(node_p);
		x0prim=x0-xcentro;
		y0=NODE_Y(node_p);
		if (y0==0) sy=0;
		else sy=y0/fabs(y0); /*sign of y*/
		
		if (x0prim==0) sx=0;
		else sx=x0prim/fabs(x0prim); /*sign of x*/
		
			
		if (y0==0) theta=0;
		else if(x0prim==0) theta=M_PI/2;
		else theta=atan2(y0*sy,x0prim);/*to obtain properly the value of the angle*/
				
		DR=(A+C*pow(theta,2)+D2*pow(theta,3)+E*pow(theta,4)+F*pow(theta,5))/100; /*radius variation*/
				
		x1prim=x0prim+DR*cos(theta);
		y1=y0+DR*sin(theta)*sy;
		
		if (y0==0) 
		{
			y1=0;
			if (x0prim <0)	x1prim=x0prim-2*A/100;
			
		}
		if (x0prim==0) x1prim=0;
			
		NODE_X(node_p)=x1prim+xcentro;
		NODE_Y(node_p)=y1;
			
	}	end_f_loop(f,tf)
	#endif
}

[86lolo]

By modifying the UDF to small displacements, it works fine during few time-steps. But then in crashes again. Never crashes in Serial, crashes after few time steps in parallel, what makes me think there must be a problem when the mesh is modified (remeshing) and FLUENT tries to repartition it. But still can't figure out what is wrong here.
Anyone has a clue?

[pakk]

I really don't have any idea, I have no experience with a parallel udf.
I only came here to say that you have a good way of asking questions: you explain what you want, what you tried, what went wrong, the code you used, and you show your attempts to solve the problem. You even used a title for this thread that describes the problem.

I may in the future refer to this question to show other users how they should ask questions here. I really, really hope that there will also be an answer, to show that this way of asking questions really helps...

[86lolo]

Thanks for your compliment
I think that if you request anonymous help, you must be very accurate and precise. Otherwise, the a helper may just pass by. Maybe he/she even knows a solution, but does not understand the problem because of a bad explanation.

I have being trying with that, but still I haven't been able to find out what is wrong.
I have tried that UDF in a different simplified meshes and it works in some of them, not in most. This demonstrates that the code is OK. However, for some reason I don't know, it crashes in parallel.

I have also found out that unsteady tracking of particles using DPM makes FLUENT to crash (again, not in serial at all, but in parallel). Error displayed in the console was similar.

It is horrible that I have to do the calculations in serial. Gonna take 1 week each .

[tombyk]

Hello 86lolo,

please did you solved the problem? I have exactly the same error like you had, also with DEFINE_GRID_MOTION UDF. I tryed the same solutions, like you did, but didn't help.

Please it would be very helpful, if you know, how to solve it.

Thanks a lot!

[86lolo]

Unfortunately, not.
I could not make it. The only way I could skip the problem (not actually solving) was to code another program which will run FLUENT externally (you can do this with Matlab, Bash, or similar). Since my model only needed to update the grid once every 1000 time-steps, I coded that:
-Start loop

-Run Fluent in parallel, read case and data, simulate in parallel 1000 time-steps, write case and data.
-Run Fluent in serial: read case and data, activate dynamic mesh, move the mesh, deactivate dynamic mesh, save case and data

-End loop

I am not yet happy with this. I actually did not solve the problem, just could avoided it, I was in a hurry to get the results and that trick somehow worked out. However I still would like to know why it was crashing.

To clarify sth else: My domain is a rectangle with 4 holes (2D simulation of flow over array of cylinders). I checked, surprisingly that:

- This crashed in that mesh, but when I cut the mesh off the centre of the 1st cylinder (thus, there is not any full hole in the domain), it works fine.
- This made me suspect that maybe it crashes if partition boundaries fall in the moving zones: I manually re-partitioned the domain so that the partition boundaries did not touch them, tried it out, did not work.
- Now that I think again about this... would it fail because my moving boundary was a circle? (I mean, start and end nodes were the same)? I don't see why it would crash in that condition, but I think it's worth checking: split the moving thread into 2 parts, will it work now? If you try, please, let us know

Tell me, tombyk, how is your geometry?

[tombyk]

Hey 86lolo!

I managed the problem. It seemed there is a bug using partitioning in version of Fluent 14.5.7. It worked for me in version 6.3 and now it is working perfectly in the latest version 15.0.

Maybe worth trying also for you!

tombyk

[86lolo]

Well, I don't have either version 6 or 15. I will try to obtain them and check, but anyway, thanks a lot for your answer. It is nice to realize that it was a bug and not my fault