[sergiocavaleirocosta]

Hello,
I am trying to develop a code to, after some time, copy the temperature of a solid to another solid with the same geometry and similar mesh. I intend to simulate a transient solution of similar moving objects without the computational effort of calculating and remeshing every time step. This way the object would "jump" to the next position every few specified time.
In order to do this I have developed the UDF:

DEFINE_ADJUST(temp_adjust, domain)
{
	real current_time;
	current_time = CURRENT_TIME;
	
	div_t divide;
	real dt;
	dt = 0.5;
	divide = div(current_time * 100., dt * 100.);
	
	cell_t c;
	
	int i;
	real Temp1[408];
	real Temp2[408];
	
	Thread *t1 = Lookup_Thread(domain, 18);
	Thread *t2 = Lookup_Thread(domain, 19);
	
	if (divide.rem == 0){
		/*----------------body 1 -----------------*/
		i = 0;
		begin_c_loop (c, t2)
		{
			Temp1[i] = C_T(c, t1);
			C_T(c, t1) = 300.;
			i ++;
		}
		end_c_loop (c, t1)
		
		/*----------------body 2 -----------------*/
		i = 0;
		begin_c_loop (c, t1)
		{
			Temp2[i] = C_T(c, t2);
			C_T(c, t2) = Temp1[i];
			i ++;
		}
		end_c_loop (c, t2)
		
	}
}

I am trying to store the temperatures of the first solid in Temp1 to replace the second solid's temperature and the same thing to the second solid to propagate for further solids (not being used for now for simplicity).
The code is compiled without issues, yet during the run, when it is evaluated for the first time the Fluent crashes.

Can anyone help me with this? I can't figure out what may be the issue, even because I am new to UDFs.

Thanks in advance.

[AlexanderZ]

your temperature array has 408 elements

Temp2[408]

are you sure, that your finite element volume has less that 409 elements?

best regards

[sergiocavaleirocosta]

Originally Posted by AlexanderZ

your temperature array has 408 elements

Temp2[408]

are you sure, that your finite element volume has less that 409 elements?

best regards

Yes, I even believe that there are less than that. I am using a very coarse mesh for testing.
Even because this mesh refers to the solid elements where there is only conduction.

[AlexanderZ]

was

		begin_c_loop (c, t2)
		{
			Temp1[i] = C_T(c, t1);
			C_T(c, t1) = 300.;
			i ++;
		}
		end_c_loop (c, t1)
		
		/*----------------body 2 -----------------*/
		i = 0;
		begin_c_loop (c, t1)
		{
			Temp2[i] = C_T(c, t2);
			C_T(c, t2) = Temp1[i];
			i ++;
		}
		end_c_loop (c, t2)

tobe

		begin_c_loop (c, t1)
		{
			Temp1[i] = C_T(c, t1);
			C_T(c, t1) = 300.;
			i ++;
		}
		end_c_loop (c, t1)
		
		/*----------------body 2 -----------------*/
		i = 0;
		begin_c_loop (c, t2)
		{
			Temp2[i] = C_T(c, t2);
			C_T(c, t2) = Temp1[i];
			i ++;
		}
		end_c_loop (c, t2)

that could be the reason

best regards

[sergiocavaleirocosta]

Originally Posted by AlexanderZ

was

		begin_c_loop (c, t2)
		{
			Temp1[i] = C_T(c, t1);
			C_T(c, t1) = 300.;
			i ++;
		}
		end_c_loop (c, t1)
		
		/*----------------body 2 -----------------*/
		i = 0;
		begin_c_loop (c, t1)
		{
			Temp2[i] = C_T(c, t2);
			C_T(c, t2) = Temp1[i];
			i ++;
		}
		end_c_loop (c, t2)

tobe

		begin_c_loop (c, t1)
		{
			Temp1[i] = C_T(c, t1);
			C_T(c, t1) = 300.;
			i ++;
		}
		end_c_loop (c, t1)
		
		/*----------------body 2 -----------------*/
		i = 0;
		begin_c_loop (c, t2)
		{
			Temp2[i] = C_T(c, t2);
			C_T(c, t2) = Temp1[i];
			i ++;
		}
		end_c_loop (c, t2)

that could be the reason

best regards

Thank you so much AlexanderZ. That was definitely an issue, yet I changed the code according to your suggestion and I am still with problems. I have placed:

Message("Ti = %g \n", Temp1[i]);

inside the second loop and the output in the console is 0 in the temperature diverging my solution. Then I did the same in the first loop to check and temperatures were correct! How can this be possible?

Thank you once again.

[robboflea]

Are you executing the UDF in parallel or in serial solver?

[sergiocavaleirocosta]

Originally Posted by robboflea

Are you executing the UDF in parallel or in serial solver?

Hello robboflea, I am using parallel.

[robboflea]

In this case you have to consider that not all calculation nodes will have access to the whole mesh and that the two arrays Temp1 and Temp2 will exist as a separate copy in each calculation node!


When executing the first loop Temp1 is filled only in the core (or cores) that have a share of cells belonging to that boundary. If the second loop is not executed by the same core (quite likely and in any case something you have no control over) because the faces belonging to such boundary have been assigned to another core by mesh partitioning, then you will be assigning garbage values stored in Temp1 (not initialized at this point) to C_T(c,t2).


I advice you to first execute the UDF in serial mode and check that it works. Then work on the parallel version but for this you need basic understanding of MPI and, in general, how distributed memory calculations work.


Hope it helps,


Roberto

[sergiocavaleirocosta]

Originally Posted by robboflea

In this case you have to consider that not all calculation nodes will have access to the whole mesh and that the two arrays Temp1 and Temp2 will exist as a separate copy in each calculation node!


When executing the first loop Temp1 is filled only in the core (or cores) that have a share of cells belonging to that boundary. If the second loop is not executed by the same core (quite likely and in any case something you have no control over) because the faces belonging to such boundary have been assigned to another core by mesh partitioning, then you will be assigning garbage values stored in Temp1 (not initialized at this point) to C_T(c,t2).


I advice you to first execute the UDF in serial mode and check that it works. Then work on the parallel version but for this you need basic understanding of MPI and, in general, how distributed memory calculations work.


Hope it helps,


Roberto

Thank you robboflea that makes a lot of sense and explains the different issues I have been experiencing during my tests.

I will do has you suggested and try in serial. But if that is the case how can I control the place where data is stored?

Something I have tried, and have abandoned later, was to write temperatures for a txt file and then read from it in the second loop, although I didn't manage to put it to work as well.

Greetings.

[robboflea]

You cannot control it (not that I am aware of).
However if you look in the Fluent manual, in the section named "Parallel UDF considerations" (or something similar) it will explain you in great detail how to deal with parallel UDFs and transfer data to/from nodes.


Rob

[sergiocavaleirocosta]

Thank you for the explanations.

I followed your suggestion and I have been reading the fluent udf parallel information and I have been trying to understand how this code should be adapted to the parallel approach, but I am completely lost!

How can I access to variables? I have been playing with the #if !RP_HOST, #if RP_NODE, node_to_host_real(Temp1), but so far nothing have worked.

Can anyone give me a guide?

Thank you.

[robboflea]

The macros that you mentioned are only used to identify particular nodes. In order to access the solution variables (temperature, velocity...) you need to use the same access macros that you would use for serial implementation. No difference here.


There is a section on "Cell MAcros" on the Fluent manual. For example, to access density in a cell you'd use C_R(c,t).


All the info you need are in the fluent manual. If you have any specific issue you can post it here and me (or other people) may get a chance in guessing what's wrong but without being specific I cannot do anything but refer you to the fluent manual


Good luck!

[sergiocavaleirocosta]

Once again, I am very pleased with your help.

I am trying to solve the issue you mentioned.

Originally Posted by robboflea

In this case you have to consider that not all calculation nodes will have access to the whole mesh and that the two arrays Temp1 and Temp2 will exist as a separate copy in each calculation node!

When executing the first loop Temp1 is filled only in the core (or cores) that have a share of cells belonging to that boundary. If the second loop is not executed by the same core (quite likely and in any case something you have no control over) because the faces belonging to such boundary have been assigned to another core by mesh partitioning, then you will be assigning garbage values stored in Temp1 (not initialized at this point) to C_T(c,t2).

Roberto

From your comment, I understand that the Temp1 array should be passed or to the host node or to all nodes in order to get the data available in the second loop (since I don't know in which node will be the loop). That is why I have been working around with node_to_host_real(Temp1). Nevertheless, when I print the Temp1 array in the second loop I get the non-sense data you pointed out, so I think it means that this loop cannot access to the Temp1 yet. I believe that the issue is, how can I make Temp1 available from the second loop?

Thank you so much.


Here it is my current code:

DEFINE_ADJUST(temp_adjust, domain)
{
	real current_time;
	current_time = CURRENT_TIME;

	div_t divide;
	real dt;
	dt = RP_Get_Real("dt");
	divide = div(current_time * 100., dt * 100.);
	
	cell_t c;
	
	int i;
	real Temp1[408];
	real Temp2[408];
	#if !RP_HOST
		if (divide.rem == 0){
			Thread *t1 = Lookup_Thread(domain, 18);
			Thread *t2 = Lookup_Thread(domain, 19);
			/*----------------body 1 -----------------*/
			i = 0;
			begin_c_loop (c, t1)
			{
				Temp1[i] = C_T(c, t1);
				C_T(c, t1) = 300.;
				i ++;
			}
			end_c_loop (c, t1)

			node_to_host_real_1(Temp1);
			
			/*----------------body 2 -----------------*/
			i = 0;
			begin_c_loop (c, t2)
			{
				Message("Temperatura = %g \n", Temp1[i]);
				Temp2[i] = C_T(c, t2);
				C_T(c, t2) = Temp1[i];
				i ++;
			}
			end_c_loop (c, t2)
		}
	#endif
}

[robboflea]

What are you trying to achieve is not easy and you are not using the correct strategy. Is your mesh conformal at the interface? Do you have an exact mapping between the nodes at the interface of the two domains?

If not you have to interpolate your data when passing the information and that is not easy. Also another issue is that you're passing data by node ID. Your first loop fills Temp1[i] with the cell temperature but, even if you were to pass correctly this array to the second wall, you cannot be sure that C_T(c,t2) corresponds to the same node where Temp1[i] has been recorded. You have to check that the coordinates are the same (within tolerance). You cannot even be sure that the second loop is shorter than the first one. If not your code will segf when trying to access Temp1[i] on a out of bound index.

Also, when passing arrays between nodes you have to first communicate the dimension of the array. I suggest you study a bit of MPI to understand how data communication works.

Have you tried communicating boundary conditions by just exporting and reading boundary profiles from Fluent? Fluent can interpolate those data on non conformal grids for you (not sure about the quality of the interpolation, I always work with conformal grids) but I think it's worth a shot

[sergiocavaleirocosta]

Originally Posted by robboflea

What are you trying to achieve is not easy and you are not using the correct strategy. Is your mesh conformal at the interface? Do you have an exact mapping between the nodes at the interface of the two domains?

If not you have to interpolate your data when passing the information and that is not easy. Also another issue is that you're passing data by node ID. Your first loop fills Temp1[i] with the cell temperature but, even if you were to pass correctly this array to the second wall, you cannot be sure that C_T(c,t2) corresponds to the same node where Temp1[i] has been recorded. You have to check that the coordinates are the same (within tolerance). You cannot even be sure that the second loop is shorter than the first one. If not your code will segf when trying to access Temp1[i] on a out of bound index.

Also, when passing arrays between nodes you have to first communicate the dimension of the array. I suggest you study a bit of MPI to understand how data communication works.

Have you tried communicating boundary conditions by just exporting and reading boundary profiles from Fluent? Fluent can interpolate those data on non conformal grids for you (not sure about the quality of the interpolation, I always work with conformal grids) but I think it's worth a shot

You have just referred to some of my fears!
In reality, both solid have similarly structured mesh. Nevertheless, I am not sure if both have the same cell numbering order (most probably not). Because both meshes are "equal", with the same number of volumes, I believe I can avoid the interpolation you mention. It is just a translation of the temperature with step size.
My first approach was writing coordinates and temperatures to a file, but I got the same kind of issues so I gave up. Do you believe it would be a better approach? Is there a way to refer to a cell by its coordinates?

Thanks.

[robboflea]

There is no way to refer to the cell by coordinates but it is possible to access to the cell centroid and check its coordinates. With this you may be able to check that you're passing the information between the same node. However it is a very time-consuming and tedious process (and you don't want to do this every time you do the passing of information).


If I were you I'd just avoid using UDFs in your situation and use .prof files.

[sergiocavaleirocosta]

Originally Posted by robboflea

There is no way to refer to the cell by coordinates but it is possible to access to the cell centroid and check its coordinates. With this you may be able to check that you're passing the information between the same node. However it is a very time-consuming and tedious process (and you don't want to do this every time you do the passing of information).


If I were you I'd just avoid using UDFs in your situation and use .prof files.

Thank you, robboflea, you are the best!
I will see profile files then.