k and ω boundary condition type for outlet/ Dirichlet or Neuman

alinik · July 9, 2017, 13:37

Hi all,

I have two questions regarding the "Specified Flux" option that become available in UDS tab once we activate UDS and also k and ω boundary condition type:

1) what type of boundary condition does fluent use for pressure outlet in terms of k and ω. (Dirichlet or Neuman?) does the solver specify a value for the scalar at the outlet or the derivative of the quantity?

2) Is the specified flux boundary condition type in UDS tab, a Neuman-type condition? In other words, if I set it equal to zero for the scalar φ, does that impose 𝜕φ/𝜕n=0 at the outlet or 𝜕φ/𝜕n+ Un φ=0 ?

I did not found any information about this in the theory guide.

Thanks,
Ali

vcvedant · July 10, 2017, 18:22

Hi Ali,

I have similar issue while describing boundary condition for UDS. Please post here if you find the solution to this.

Vedant

LuckyTran · July 11, 2017, 17:34

As far as I know, at a pressure outlet the BC is the zero gradient type.

I don't follow your question on the UDS. You can't (at least you shouldn't) specify ��φ/��n+ Un φ=0 at the outlet, that would be a impermeable wall.

alinik · July 19, 2017, 10:56

Hi all,

This is the response I got from an ANSYS rep:

at a pressure outlet, the k and omega, will be interpolated from the inside and the value at the face set to the same value as the adjacent cell center. No diffusive flux is computed, only the convective value is computed at such boundary.
For the UDS, if you specify the gradient, only the diffusive term will be set to that value, the convective term will be computed as for the k.

Does anyone know how to implement that with UDS?
If one wants to reproduce(and later modify) a turbulence model, they have to use UDS and the only options for UDS boundary conditions are specified flux and specified value which I believe are Neuman and Dirichlet BC respectively.
I am kind of lost and need help here.

LuckyTran · July 19, 2017, 11:34

Are you asking about only the pressure outlet or a generalized boundary condition? For an outlet, it is precisely written what here what happens:

Quote:

Originally Posted by alinik

at a pressure outlet, the k and omega, will be interpolated from the inside and the value at the face set to the same value as the adjacent cell center. No diffusive flux is computed, only the convective value is computed at such boundary.
For the UDS, if you specify the gradient, only the diffusive term will be set to that value, the convective term will be computed as for the k.

For k and omega, diffusive fluxes are zero gradient. Advective fluxes are calculated per the discretization scheme, which is usually an upwind biased scheme. Hence for a UDS you have the option to specifying the same zero gradient for the diffusive flux so that the same advective discretization is used.

alinik · July 19, 2017, 15:39

Tran,

Thank you for the description.
Please correct me if I am wrong: what we specify in the UDS tab of the pressure-outlet BC, does not include the convective fluxes and if we set the Specified flux to zero, we have in fact eliminated the diffusion flux and the convective flux would still be there. Is that right?

July 9, 2017, 13:37	k and ω boundary condition type for outlet/ Dirichlet or Neuman	#1
alinik Senior Member ali Join Date: Oct 2009 Posts: 318 Rep Power: 17	Hi all, I have two questions regarding the "Specified Flux" option that become available in UDS tab once we activate UDS and also k and ω boundary condition type: 1) what type of boundary condition does fluent use for pressure outlet in terms of k and ω. (Dirichlet or Neuman?) does the solver specify a value for the scalar at the outlet or the derivative of the quantity? 2) Is the specified flux boundary condition type in UDS tab, a Neuman-type condition? In other words, if I set it equal to zero for the scalar φ, does that impose 𝜕φ/𝜕n=0 at the outlet or 𝜕φ/𝜕n+ Un φ=0 ? I did not found any information about this in the theory guide. Thanks, Ali saihasil likes this.

July 10, 2017, 18:22		#2
vcvedant Member Vedamt Chittlangia Join Date: Feb 2016 Posts: 64 Rep Power: 9	Hi Ali, I have similar issue while describing boundary condition for UDS. Please post here if you find the solution to this. Vedant

July 11, 2017, 17:34		#3
LuckyTran Senior Member Lucky Join Date: Apr 2011 Location: Orlando, FL USA Posts: 5,674 Rep Power: 65	As far as I know, at a pressure outlet the BC is the zero gradient type. I don't follow your question on the UDS. You can't (at least you shouldn't) specify ��φ/��n+ Un φ=0 at the outlet, that would be a impermeable wall.

July 19, 2017, 10:56		#4
alinik Senior Member ali Join Date: Oct 2009 Posts: 318 Rep Power: 17	Hi all, This is the response I got from an ANSYS rep: at a pressure outlet, the k and omega, will be interpolated from the inside and the value at the face set to the same value as the adjacent cell center. No diffusive flux is computed, only the convective value is computed at such boundary. For the UDS, if you specify the gradient, only the diffusive term will be set to that value, the convective term will be computed as for the k. Does anyone know how to implement that with UDS? If one wants to reproduce(and later modify) a turbulence model, they have to use UDS and the only options for UDS boundary conditions are specified flux and specified value which I believe are Neuman and Dirichlet BC respectively. I am kind of lost and need help here.

July 19, 2017, 15:39		#6
alinik Senior Member ali Join Date: Oct 2009 Posts: 318 Rep Power: 17	Tran, Thank you for the description. Please correct me if I am wrong: what we specify in the UDS tab of the pressure-outlet BC, does not include the convective fluxes and if we set the Specified flux to zero, we have in fact eliminated the diffusion flux and the convective flux would still be there. Is that right?