hi all,

what would be the best possible bc for a compressor problem to be run on CFX 5.4.1. and other factors of influence.

thankyou for your time.

regards joseph

Assuming your are running subsonic; Ideally you want to apply a <b/>total pressure[/b] at the inlet and <b/>static pressure[/b] at the outlet, allowing the mass flow to be determined by the solution.

If either your inlet Ptotal or outlet Pstatic are unknown, and you have a desired mass-flow, apply your known pressure appropriately and a mass-flow at the other boundary. You may then want to replace the mass-specified boundary with the mass averaged pressure at that location.

You may have to tweak your pressure to obtain the correct mass-flow in the Ptotal-in -> Pstatic-out scenario. Use the 'Edit' command in the solver monitor to do this without going back to CFX-Build each time.

Download the pre-release version of <b/>CFX-Post[/b] from the CFX website to access more advanced post processing tools than those available from Visualize. The mass averaged quantities, or integral quantities such as mass flow calculated by this new post processor are exactly true to those calculated by the solver.

Robin

hai robin thanks for the info. the problem I am facing is that the inlet is total pressure and total temp and exit is mass flow rate.

but it keeps crashing so I am tweaking on the time step will this affect the solution?

Regards joseph

Can you give more info? What is your rpm? Is the flow compressible? If so, are you using real gas or ideal gas?

Start with a reasonable initial guess; use the turbo initial guess generator to get started.

In general, you want to start with a reasonably large timestep, dtime=1/abs(omega1) or perhaps 0.1/abs(omega1), any smaller and you will have difficulty.

Once you have gotten past the initial transient stage, after about 5-10 iterations, bump up the timestep to 5 or 10 over omega. You should be able to achieve a convergence rate of about 80% per iteration.

If your flow is compressible, try running incompressible first, then turn on compressibility. If you are close to choking conditions, start at a lower mass flow, perhaps 75%, and ramp it up.

Robin

(1). By the way, is this the "trial-and-error-in-CFD"? (2).Well, it is a joke, there is still a long way to go to reach 99 cases.

It's not trial and error, it is a process which is extremely effective in the hands of a well informed, experienced user. Forums like this one allow the new users to gain confidence with the help of more experienced users. Anything constructive to add? ...John?

Robin

Oops. I was thinking in terms of TASCflow there.

CFX-5 should cope well with a fairly rough initial guess. The timestep should still be on the order of 1/abs(omega) however. It sounds like you are running compressible flow too, so the recommendation about starting away from choke will still apply. You can change the mass flow by editing the CCL portion of your .def or .res file between runs.

If you are still having trouble, contact a CFX office for support, it is included in your license.

Are you using the 2nd order High Res scheme?

Robin

hai robin,

I have sent some stuff to ur mail id too. I am using first order scheme to get some initial convergence .

regarding initial guess how shall I give it should be the average condition at inlet or outlet or the full flow domain presently I am using the average inlet codition.

joseph

(1). Based on my experience with CFX-TASCflow (which has been said to be quite similar to CFX-5, 99% I guess), it is hard to get the iteration process to continue running. (2). But once it starts to behave, the convergence is good. (3). My feeling is: a more tightly coupled solution algorithm is more sensitive to the initial flow field, which is just arbitrary guess and has no physical meaning at all. (4). I did tried various approaches, but I could not get a consistent guidline from my experience. (5). There are two possible source of difficulties, (a). your geometry is complicated, (b). in the iteration, you have flow separations, which is common in the compressor flow. (6). And sometimes, it is due to the selection of the turbulence model. (7). The boundary condition is not a critical issue, you can use simple velocity inlet, or total pressure inlet and static pressure outlet. (8)My suggestion is: if you still have the problem, try to run flow with simpler geometry first to get the feeling about how to get converged solution. Then move on step-by-step to a more realistic geometry. (9). Is the compressor radial or axial?

it is a radial one

(1). I think, radial compressor is more difficult to handle than the axial one. (2). Anyway, as I have said, try a simple geometry first to get a feeling for the process of convergence.

Joseph,

I responded to your email with further instructions.

What is your tip radius? Are you operating near choke?

Robin