Hi, I've been performing a grid size study on the case that I'm currently working on and received the error message after approximately 20 time steps:

divergence detected in AMG solver: pressure correction primitive error at Node 0: floating point exception. Error: floating point exception. Error Object: #f

This error message repeats itself for nodes 1-3. The case is unsteady 2D flow past a rectangular plate in a duct. I'm using a structured grid with 825,000 cells, PISO P-V coupling, and my pressure discretization is set to 2nd order. My case is running in parallel using 4 processors. I previously ran this case using 170,000, 325,000, and 500,000 cells with no problems. I changed the under-relaxation factors to 0.2 and 0.5 for pressure and momentum respectively, but still get the error message after approx. 15-25 time steps. Any help will be greatly appreciated.

change the pressure discretisation to standard, it should not give this error, if it gives then examine your case closely because then the problem is with set up not with discretisation. Fluent is very stable solver.

Thanks, switching the pressure over to standard seems to have solved the problem.

If you wish to switch back to second order , you can do it, once you have some order of convergence by standard scheme.

Hi, Is this true for the 3D-unsteady as well? As I am trying to do a 3d flow over circular cylinder using DES but from the very beginning it gives the NAN (division by zero). Any comments (As i have tried both segregated and couple solvers with same result). Cheers, Endee

I have been doing 3D unsteady cylinder calculations, and yes fluent can give you problems if you chose second order scheme in the start. In fact, i am able to make fluent diverge with 2000 cells, with 1m/s velocity inlet, if i started with second order. You can always switch to higher order schemes after you have some degree of convergence. This is generally true.

thanks...Zxaar Just some queries about simulation with 3D unsteady cylinder at vel of about 70m/s and temp 300 K with legth to dia 2-1. How did you specify the boundary condition? What time step do you recommend and what should be the data saving frequecy to capture the unsteady vortices? cheers, Endee

i have been mostly working around of flow 60m/s, and with LES i have been using 1E-05 as time step since i am using sliding mesh aproach for rotation. You can use NITA also if you do not have any rotating parts. (with sliding mesh NITA always diverges). i am using vel inlet, pressure outlet, with operating condition 0 pressure

[dralosdir]

Originally Posted by zxaar
;124022

change the pressure discretisation to standard, it should not give this error, if it gives then examine your case closely because then the problem is with set up not with discretisation. Fluent is very stable solver.

i have that problem too. where can i set the pressure discretisation to standard?

[krishnaprasad]

hi all
i am working in ansys 12.1 fluent to generate waves using udf. during the solution it is showing,,divergence detected in the AMG solver and stopped the iteration.??
i had tried many times ...can you please help me.

and also i don't know how to set unsteady flow and non iterative time advancement solver controls..please help me.
thank you in adv

[jhthoh]

where can i set the pressure discretisation to standard? i m using ANSYS 12.0 fluent

[sanjose]

Hi! I'm trying to determine a residence time distribution of a plug flow reactor by calculation of an advection-diffusion equation for a tracer (scalar transport) using a user defined scalar (uds).
I receive this message:
divergence detected in AMG solver: uds-0
Primitive Error at Node 2: floating point exception

How can solve this problem?
Thank you.

[hadikhayyamian]

@ dralosdir :
If u r using Fluent 6.3.26 and u would like to set the pressure discretisation to standard then follow:
Main Menu > Solve > Controls > Solution... Under Discretization set Pressure to Standard.