Learning Forum

[schwaral]

Hi, nI have a 3D case that works fine. Now I want to simulate only half of the domain by using a symmetry plane. Thats works fine as well until I introduce the UDS. I couldn't find information about UDS and symmetry plane. Do I have to set UDS gradient =0 at symmetry plane manually? Or what could be the reason for the divergence caused by UDS with symmetry plane?n

[Rob]

I've not seen any issues with symmetry & UDS. Can you check the rest of the mesh and set up? n

[schwaral]

All right, thats good to know. I turned off the UDS source terms but they are not the reason as well. I have even better mesh quality then in my case without the symmetry plane. I initialize in the same way and should not be the problem. Using smaller timestep leads to same divergence in first timestep. I think I will stick to the large domain.n

[Rob]

Check the rest of the set up and that the mesh quality (not cell quality) is good. n

[schwaral]

You were right, Diffusioncoefficient was set to 1. With 0 it works. But it is not running with a Diffusioncoefficient for UDS0=3e-05 and UDS1=1e-10. Do you have any further advice? I do not think it is the mesh quality.

[schwaral]

Could it even possibly be the mesh quality, if it converges with a Diffusion Doefficient (D_c) =0? For small and large D_c the UDS values go towards infinite. I did find people are using linearization of source term. Might this be a problem? When I disable the FLUX Term for both UDS (I think the D_c should not be used then??) the solution diverges as well. This last point confuses me a lot.nnMy Source Term for UDS1/2 are: nC is scalar from UDS 1, M is scalar of UDS2 --- ast. adyn, gst, gdy, C_sat, M_sat are coefficients --- c_vel = velocity.nnsource (C)= -c_density * ((ast + adyn * c_vel) * (1 - M / M_sat) * C + (gst + gdyn * c_vel) * (1 - C / C_sat) * M);ndS[eqn] = -c_density * ((ast + adyn * c_vel) * (1 - M / M_sat) - (gst + gdyn * c_vel)*M/C_sat);nnsource (M)= c_density * ((ast + adyn * c_vel) * (1 - M / M_sat) * C + (gst + gdyn * c_vel) * (1 - C / C_sat) * M);ndS[eqn2] = -c_density*((gst + gdyn * c_vel) * (1 - C / C_sat)+(ast + adyn * c_vel)*C/M_sat);n

[Rob]

Diffusion of zero should fail as it'll divide by zero somewhere, 1e-10 is about right for liquids. User Scalars tend to be more sensitvie to mesh etc than the Fluent ones (energy, species etc) as the solver maths is different. Setting dS = 0 is fairly common. Try turning the scalars off and putting the same equation into UDM and see what values it's giving. That should cause the solver to fail and will give you some idea what's going on. n

[schwaral]

Thank you for the nice answer! nKnow everythings seems to work fine. I think it was the mesh quality that was not good enough.I have one more question that I already posted but could not solve it. You have in the UserGuide an exaple for the UDS_FLUX. When I use it exacly like it is in the example all my equations diverge. Using the Default mass-flow-rate option for UDS the convergence of residuals is more then enough ( 6 orders and more).Short overview of my Case: 3d, slim Porous media with UDS Source Term (see above), 2 UDS in total, K omega-sst, velocity-Inlet, Pressure outlet. nI use only 2 cells in porous media from porous media inlet, to porous media outlet. Can this be a problem for the UDS_FLUX? I really do not want to use more cells in thickness direction for the porous media. n

[Rob]

I don't think that'll cause a problem but check the amount of scalar you're adding in case the mass per volume value is excessive. You could adapt the region and see if that helps, but it shouldn't make much difference. n