hi, i'm trying to simulate flow in a radial turbine rotor passage.i'm using pressure inlet BC as my inlet and pressure outlet BC as my outlet. i've modelled a single passage with rotationaly periodic sides.i'm using moving reference frame with angular velocity of 64000 rpm. Velocity formulation is absolute and specification in the BC menu is according to convenience where moving walls are specified as stationary relative to adjacent cell and stationary walls are specified as stationary in the absolute frame. The flow is supposed to expand from 3.5 atm to 1 atm with the inlet total temperature being 1123K. the flow is compressible.

my problem is,the simulation diverges right after the first iteration and the error message is as follows, Error: divergence detected in AMG solver: temperature

before the error message,also the statement that temperature is limited to 1.000e00 and absolute pressure limited to 1.000e00 appears...which somehow seems not right to me.

can anybody please help and let me know if there's anything wrong and how to overcome this? also, any ideas regarding the approach to simulate this turbomachinery problem would be most welcome. been stuck for awhile trying to change some parameters but to no avail.please help.

thanx a lot and best regards

Could be your mesh. Could be your solver. Could be your setup.

A common mistake is for people to set the fluid volume as rotating in the opposite direction that the geometry's rotating... what you want is for the fluid volume to rotate with the geometry (you're not rotating the "fluid" relative to the walls, just the computational domain that's analyzing the fluid, and that should be moving with the walls). Not saying you did that, but it's a common mistake so I thought I'd throw it out there.

That's a strong pressure ratio and a high temperature... I'm thinking the coupled solver is the right solver for this situation. You traditionally don't have to mess with the solver limits when using the coupled solver, but you probably want to drop the courant number at first.

Also, the FMG initialization seems to help out a lot when the model blows up at the first few iterations. Use the TUI command "solve init fmg y" to run FMG.

Last thing is to check your mesh using Grid->Check and look through the info to see if there's any warnings.

Hope this helps, and good luck, Jason

thanx a lot jason.nope, the common error was not the problem, i modelled like u said where the geometry is rotating with the flow. my grid check is ok, there are no warnings.i've checked the grid in Gambit before exporting the mesh and i rechecked the grid in fluent. before this i was thinking of lowering the under relaxation value and i checked the forum for previous threads discussing AMG error but, i'm not sure, but i think doesn't really suit my problem.anyway, if i understand u correctly,if i change it to coupled solver, i can just use the default setting?i'l do that. tried the FMG initialization? i tried using the command but it displayed invalid command.

thanx a lot

Which version of Fluent are you running? FMG is available from 6.2 on. An older version won't have that command, sorry about that.

With the coupled solver, you still may need to lower the Courant number, especially at first.

Hope this helps and good luck, Jason

I recieved the same error message in one of my simulations where the temperature changes by only a fraction of a degree. The only way I could reconcile the problem was by changing the under relaxation factors.

thanx jason, and thanx geoff. i'm using fluent 6.2. managed to initialize my flow field and started iterating..yup, i did change the courant number like u said jason,i set it at 0.005.this time it did not blow up after the first iteration.however quite the contrary,the iteration just keeps on going and the residuals do not seem to be changing much if its changing at all.after a few thousand iterations i interrupted the calculations because it did not seem to be getting anywhere. any idea of what i should try? by the way, to decrease the under relaxation value,what's the suitable value to use? apart from that,my understanding is for a turbine, reverse flow should not occur but my simulation so far has some value for reverse flow.

thanx a lot

nanda

.005 is extremely small for a courant number... it's taking forever for the residuals to do anything, becuase you're restricting any change in the flow. If you do go down to .005, I would only do that for 10 or so iterations, and I would gradually increase the courant until you get to 1... and if the model's still behaving you can try higher values as well.

Hope this helps, and good luck, Jason

thanx jason. did as u said.and initialy the residual plot seemed encouraging however the same problem seem to occur even after i gradually increased the courant number.i also tried to decrease the under relaxation factor.but the residual for continuity especialy seem to be oscillating/fluctuating but without moving towards the convergence criteria..care to advise?

thanx a lot

It sounds like a problem with your setup, but I'm not sure what it could be. You need to start looking at the solutions and seeing where it's having a problem. We tried the simple solutions, now you have to start digging into where the model is blowing up, and once you know where, then you can start trying to figure out why. Residuals are available in the Plor->Contours, so start looking at those. Also, check your pressures and temperatures. Do you have a density going off to 0 or infinity? That type of thing. Once you start find the problem, then you can start trying to address the problem further.

I thought the FMG initialization was available for everything from 6.2 on... in the TUI, you can type "solve" and then "init" to get into the initialization menu... then hit return to see the available commands. Maybe on the early releases of 6.2 the quick command I gave you didn't work, or maybe it's just not available, but that's how you can check.

Another thing you may want to try are running it inviscid and incompressible to get an initial result... then you can turn both back on and try from there. Or you can turn them on one at a time (I would turn on viscocity first).

Hope this helps, and good luck, Jason

thanx jason.

i tried to do what u told me and i started with laminar and incompressible flow for the first 80 iterations and i also used lower rotational speed before increasing it to the nominal operating speed. initialy the residual plots seemed encouraging but in the very end when i reach the nominal speed it goes on iterating without any sign of ever converging..i've copied the residual plots in word document and plan to see someone bout it.i would like to ask, when u mentioned earlier bout checking if the density is goin to infinity or something in that line of thought, how do i do it? is it sufficient to check the integrals or are there other things which i should check? i'd also like to ask, since the inlet temperature for my simulation is high (1223K) and the flow is being exhausted to atmospheric conditions, do i hav to modify any values for the wall properties, and what are the way to get the temperature variation?

thanx a lot

nanda

What I was talking about with checking the density is post-processing your solution (even though it's not converged). Look at pressure, velocity, Mach, density, Temperature, Turbulent Viscocity Ratio, etc. It's not a converged solution, but you can learn a lot about what Fluent thinks is going on and this will give you better ideas as to how to approach the problem.

I didn't say try laminar, I said try inviscid... turn off all of the viscous calculation... this will basically give you an Euler solution, and then you can add viscocity back into that (in a highly turbulent flow, I've seen Laminar models cause more problems than they help, so if you're at high Reynolds, I wouldn't even bother with the laminar model... go from inviscid to which ever turbulence model you're going to use).

Hope this helps, and good luck, Jason