[Tianxu]

Hi guys,

This is quite urgent!

I am doing 2D rotating detonation engine (RDE) simulation in ANSYS Fluent.
For pressure inlet boundary condition, there are three possible cases:
1. Pi > Po, where Pi is the pressure inside the domain immediately at the inlet and Po is the total inflow pressure. In this case the pressure inside the RDE at this point is very high and blocks inflow of new mixture through the inlet face. The inlet boundary acts as a wall.
2. Pcr < Pi < Po, where Pcr is the critical pressure. In this case the inlet is not chocked and new mixture flows into the RDE according to: mass flow rate = the integral of (rho*u*dA).
3. Pi < Pcr, in this case the pressure inside the domain is low. The inlet at this point is choked, so maximum flow rate of fuel is flowing into the domain. Pcr is calculated from isentropic relation.

My UDF (mass flow rate inlet BC) compiles successfully which means the code is grammatically correct. When I tried to initialise the solution, the following errors appeared.
Node 0: Process 3524: Received signal SIGSEGV.

================================================== ============================
================================================== ============================

Node 1: Process 10032: Received signal SIGSEGV.

================================================== ============================
================================================== ============================

Node 2: Process 11508: Received signal SIGSEGV.

================================================== ============================
================================================== ============================

Node 3: Process 12336: Received signal SIGSEGV.

================================================== ============================

999999: mpt_accept: error: accept failed: No error

999999: mpt_accept: error: accept failed: No error

999999: mpt_accept: error: accept failed: No error

999999: mpt_accept: error: accept failed: No error

999999: mpt_accept: error: accept failed: No error
MPI Application rank 0 exited before MPI_Finalize() with status 2
The fl process could not be started.

I tried standalone mode of Fluent, it also didn't work....

I think this may because the logic of the code, or this UDF is not suitable for Fluent.

My code is the following:

#include "udf.h"
DEFINE_PROFILE(inlet_mf,th,i)
{

face_t f;
cell_t c;
Domain *d = Get_Domain(1);
Thread *t = Lookup_Thread(d,5);

real pw;
real po;
real pcr;
real To;
real gamma;
real v;
real vmax;
real R;
real rho1;
real rho2;
real area;
real A[ND_ND];

R = 368.9; // J/kg k
gamma = 1.29;

po = 1013250;
pcr = po * pow( (2/(gamma+1)), (gamma/(gamma-1)) );
To = 300;
vmax = sqrt( (2*gamma/(gamma+1)) *R*To );

begin_f_loop(f,th)
{

pw = F_P(f,th); //pressure on one face

F_AREA(A,f,th);
area = NV_MAG(A); // Find area of one face

if(pw >= po)
{
F_PROFILE(f,th,i) = 0.0000001;
}

else if(pw > pcr && pw < po)
{
v = sqrt( (2*gamma/(gamma-1)) *R*To * (1 - pow(pw/po, (gamma-1)/gamma)) );
rho1 = F_R(f,th);
F_PROFILE(f,th,i) = rho1*v*area;
}

else if(pw <= pcr)
{
rho2 = F_R(f,th);
F_PROFILE(f,th,i) = rho2*vmax*area;
}

}
end_f_loop(f,th)

}


Could anyone give me some advises and help?

Thanks very much!

[Tianxu]

For someone may get confusion. I'm adjusting mass flow inlet.

[AlexanderZ]

code seems to be good,
the only thing you can do, which is not mandatory, you can add math library

#include "math.h"

are you sure you are using small enough timesteps?
when did you get this error? on the first iteration?

you may check, if the problem in UDF or not, using very simple profile

#include "udf.h"
DEFINE_PROFILE(inlet_mf,th,i)
{

face_t f;

begin_f_loop(f,th)
{
	F_PROFILE(f,th,i) = 0.0000001;
}
end_f_loop(f,th)

}

[Tianxu]

Originally Posted by AlexanderZ

code seems to be good,
the only thing you can do, which is not mandatory, you can add math library

#include "math.h"

are you sure you are using small enough timesteps?
when did you get this error? on the first iteration?

you may check, if the problem in UDF or not, using very simple profile

#include "udf.h"
DEFINE_PROFILE(inlet_mf,th,i)
{

face_t f;

begin_f_loop(f,th)
{
	F_PROFILE(f,th,i) = 0.0000001;
}
end_f_loop(f,th)

}

Hi,

Thanks for the reply!

The error appears when I initialise the domain. I wasn't able to run the simulation.

I tried to add ''#include math.h", it still didn't work..

Regards

[AlexanderZ]

did you try simplified code?

may be the problem with your code is that you are using pressure and density.
to initialize domain fluent applies boundary conditions
In other words there is no pressure and density yet

what you can try, initialize your case with constant mass-flow value and hook profile after that

[Tianxu]

Originally Posted by AlexanderZ

did you try simplified code?

may be the problem with your code is that you are using pressure and density.
to initialize domain fluent applies boundary conditions
In other words there is no pressure and density yet

what you can try, initialize your case with constant mass-flow value and hook profile after that

Hi,

That sounds a good idea, I'll get back to you once I try that!

Thanks

[Tianxu]

Originally Posted by AlexanderZ

did you try simplified code?

may be the problem with your code is that you are using pressure and density.
to initialize domain fluent applies boundary conditions
In other words there is no pressure and density yet

what you can try, initialize your case with constant mass-flow value and hook profile after that

Hi,

I initialize the case with constant mass-flow inlet value and ambient pressure value. Once I tried to hook the UDF on mass flow BC, the same error appeared.

In my code, I used F_R, do I need to get the density value from a cell rather than a face?

Regards

[Tianxu]

Originally Posted by AlexanderZ

did you try simplified code?

may be the problem with your code is that you are using pressure and density.
to initialize domain fluent applies boundary conditions
In other words there is no pressure and density yet

what you can try, initialize your case with constant mass-flow value and hook profile after that

I also tried simple mass flow UDF. It compiles and runs safely. I think the problem may relate to logic problem...

[AlexanderZ]

I think, that you need values from surface, not from the cell

you can add condition to check, if the face belongs to boundary or not
if (BOUNDARY_FACE_THREAD_P(t))

#include "udf.h"
DEFINE_PROFILE(inlet_mf,th,i)
{

face_t f;
cell_t c;
Domain *d = Get_Domain(1);
Thread *t = Lookup_Thread(d,5);

real pw;
real po;
real pcr;
real To;
real gamma;
real v;
real vmax;
real R;
real rho1;
real rho2;
real area;
real A[ND_ND];

R = 368.9; // J/kg k
gamma = 1.29;

po = 1013250;
pcr = po * pow( (2/(gamma+1)), (gamma/(gamma-1)) );
To = 300;
vmax = sqrt( (2*gamma/(gamma+1)) *R*To );

begin_f_loop(f,th)
{
	F_AREA(A,f,th);
	area = NV_MAG(A); // Find area of one face
	if (BOUNDARY_FACE_THREAD_P(th))
	{
		pw = F_P(f,th); //pressure on one face

		if(pw >= po)
		{
		F_PROFILE(f,th,i) = 0.0000001;
		}

		else if(pw > pcr && pw < po)
		{
		v = sqrt( (2*gamma/(gamma-1)) *R*To * (1 - pow(pw/po, (gamma-1)/gamma)) );
		rho1 = F_R(f,th);
		F_PROFILE(f,th,i) = rho1*v*area;
		}

		else if(pw <= pcr)
		{
		rho2 = F_R(f,th);
		F_PROFILE(f,th,i) = rho2*vmax*area;
		}
	}

}
end_f_loop(f,th)

}

[Tianxu]

Originally Posted by AlexanderZ

I think, that you need values from surface, not from the cell

you can add condition to check, if the face belongs to boundary or not
if (BOUNDARY_FACE_THREAD_P(t))

#include "udf.h"
DEFINE_PROFILE(inlet_mf,th,i)
{

face_t f;
cell_t c;
Domain *d = Get_Domain(1);
Thread *t = Lookup_Thread(d,5);

real pw;
real po;
real pcr;
real To;
real gamma;
real v;
real vmax;
real R;
real rho1;
real rho2;
real area;
real A[ND_ND];

R = 368.9; // J/kg k
gamma = 1.29;

po = 1013250;
pcr = po * pow( (2/(gamma+1)), (gamma/(gamma-1)) );
To = 300;
vmax = sqrt( (2*gamma/(gamma+1)) *R*To );

begin_f_loop(f,th)
{
	F_AREA(A,f,th);
	area = NV_MAG(A); // Find area of one face
	if (BOUNDARY_FACE_THREAD_P(th))
	{
		pw = F_P(f,th); //pressure on one face

		if(pw >= po)
		{
		F_PROFILE(f,th,i) = 0.0000001;
		}

		else if(pw > pcr && pw < po)
		{
		v = sqrt( (2*gamma/(gamma-1)) *R*To * (1 - pow(pw/po, (gamma-1)/gamma)) );
		rho1 = F_R(f,th);
		F_PROFILE(f,th,i) = rho1*v*area;
		}

		else if(pw <= pcr)
		{
		rho2 = F_R(f,th);
		F_PROFILE(f,th,i) = rho2*vmax*area;
		}
	}

}
end_f_loop(f,th)

}

Hi,

I modified the UDF to hook velocity inlet BC, it works fine with no chemistry. The inlet velocity could be adjusted according to wall pressure.

But once I import chemistry (hydrogen air mechanism with 23 reactions and 9 species), the same error appeared. Is my UDF able to work to import chemkin mechanism? I'll attach my code to the next post.

Regards,

[Tianxu]

The up-to-date velocity inlet UDF:

#include "udf.h"
DEFINE_PROFILE(inlet_velocity,th,i)
{
face_t f;
cell_t c;
Domain *d = Get_Domain(1);
Thread *t = Lookup_Thread(d,5);
real po;
real pcr;
real To;
real gamma;
real R;
real p_cur;

po = 1013250; // stagnation pressure
gamma = 1.29;
pcr = po * pow(2/(gamma + 1), gamma/(gamma-1)); // critical pressure
To = 300; // stagnation temperature
R = 368.9; // J/kg k

begin_f_loop(f,th) //to find pi, pressure inside the domain immediately at the inlet
{

p_cur = F_P(f,th); //pressure on one face

if(p_cur >= po)
F_PROFILE(f,th,i) = 0.0000001;

else if(p_cur <= po && p_cur > pcr)
F_PROFILE(f,th,i) = sqrt( 2*gamma/(gamma-1) *R*To * (1 - pow(p_cur/po, gamma-1/gamma)) );

else if(p_cur <= pcr)
F_PROFILE(f,th,i) = sqrt(2*gamma/(gamma+1) *R*To);


}
end_f_loop(f,th)

}

DEFINE_PROFILE(inlet_temperature,th,i)
{
face_t f;
Domain *d = Get_Domain(1);
Thread *t = Lookup_Thread(d,5);
real To;
real p_cur;
real po;
real gamma;

po = 1013250; // stagnation pressure
To = 300; // stagnation temperature
gamma = 1.29;


begin_f_loop(f,th) //to find pi, pressure inside the domain immediately at the inlet
{

p_cur = F_P(f,th); //pressure on one face

F_PROFILE(f,th,i) = To * pow(p_cur/po,(gamma - 1)/gamma); // Temperature

}
end_f_loop(f,th)

}