Are there any guidelines for modelling tip clearances in turbomachinery applications using Turbogrid 10.0 and CFX 10.0?
I'm using Blademodeler, Turbogrid and CFX 10.0 for designing a liquid (water) pump (Q,H)=(120m3/h, 52m).
The impeller is open so the shroud is stationary and the gap between the blades and the shroud is 0.7 mm (b2 is approximately 16mm). I observe massive degradation of the efficiency when having this gap.
Naturally, according to physics, losses should be introduced with the open impeller and the gap; I just want to make sure that my simulation does not overestimate the loss.
|
There are some general guidelines with regard to modelling tip clearances in turbomachinery applications, but they equally apply to non-tip clearance models and other CFD applications. The key factors are grid densities and your converegence criteria. The most important aspect to predict the losses correctly is to base your simulations on the foundation of an appropriate grid. You should perform grid dependancy studies in the circumferential, hub to shroud and streamwise directions to understand the sensistivity of the flow in these directions and to capture gradients in the flow correctly, so that you obtain numerical solutions that are independent of the grid. Generally, a grid with 100K is adequate per blade passage, with less relative differences as the mesh density is increased, although, this can be application specific and more consideration should be given when modelling tip clearances and leakage flows. You should have at least 10-15 nodes within the tip clearance region to capture the fluxes and mass flow correctly, but once again, you should perform mesh studies to obtain an appropriate level for your application. If possible, try and avoid the tip clearance method that uses a GGI in the tip region, as long as it does not compromise the overall quality of the gird. You should also have sufficient nodes near the walls to capture the boundary layer and any associated losses. In CFX-Pre, there are no special considerations required as the flow is considered incompressible. I would reccomend using the SST model with automatic wall functions. Within the CFX 10.0 Solver, I would use the High Resolution scheme and ensure that the RMS residuals are all below 1e-4 and that all equation imbalances are below 1% (For these settings, imbalances are generally less than 0.1%). For increased accuracy you can solve so that all maximum residuals are below 1e-4. Again studies can be done on converegnece level. You can also set up some Monitor Points forefficiency or pressure difference etc. and monitor these for convergence. |
||
|