Centrifugal Fan Model - Frozen Rotor
I have some general questions about how to best setup a centrifugal fan simulation using frozen rotor settings.
The primary item of interest is the mass flow rate through the system. We currently have two fans of similar design (only difference being the overall width of the unit) and we are trying to design a third unit which will move more air simply by widening the existing design. The idea is to use CFX to confirm the appropriate width based on the CFM requirement.
The model consists of two inlets (stationary domain), an impeller (rotating domain), and a volute with outlet (stationary domain). There are essentialy two domain interfaces - between the OD of the inlet 'cylinders' and the ID of the rotating domain, and between the OD of the rotating domain and the ID of the volute. Both are set to 'Frozen Rotor', 'General Connection' and 'GGI'.
The boundary conditions are: Total Pressure Inlets = 0, and Static Pressure Outlet = 0, with a domain reference pressure of 1 atm. The fluid is air at 25 C and heat transfer is not considered.
I am using the SST turbulence model, and the rotating domain has an angular velocity of 1500 rpm. This is a steady-state simulation with auto timescale.
1. Convergence is acceptable, with imbalances typically below 1%, monitors (mass flow, torque) pretty well stabilized, but residuals usually flatline above 1E-3.
2. Depending on the specific geometry, walls are put up on the outlet as recirculation develops - but usually not until ~100 iterations are run.
3. Depending on the geometry, using the above BCs will immediately cause walls to be put up on the inlets (100% walls), so I typcially need to change the outlet BC to a mass flow for the first few iterations, then change back to static pressure= 0 to get it to run.
4. The volute geometry (specifically the tongue) has little impact on the resulting mass flow rate, seems to only affect the total pressure at the outlet. This make sense physically and coincides with previous testing of these blowers.
1. Is this simulation setup appropriately for what we are trying to do?
2. Based on the CFM numbers of the two other blower units, a straight interpolation of blower width vs. CFM suggests that we need a blower width of ~ 18" to meet flow requirements. However, if we trust the results of the simulations we have run, the resulting flow rate is falling short of this prediction by almost 100%. Any idea why that might be?
2. Why do the residuals flatline while imbalances and monitor points seem to converge?
3. Why does the number of iterations run seem to influence whether or not recirculation at the outlet is present?
4. Is the recirculation at the outlet physically valid? It has never been observed during physical testing.
A screenshot of the model and the end of a typical .out file is attached.
have you read the best practises guide for turbomachinery in the CFX documentation. It has very useful information about this sort of modelling.
Most of your questions are about accuracy - there is an FAQ on this: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F
I have done the similar simulation with geometry a bit more complex, having porous media and housing after blower unit. I am using the exact BC and frozen rotor interface between rotating fan and stationary domain.
Result is same with velocity and turbulence residual straightening around E^-03 and not converging beyond. Monitors (mass flow, Pressure) do stabilize to fair extent but not perfectly straight. I am also finding mass flow from simulation. There is deviation from experimental data but it varies between 5-15% for different cases. Your deviation of 100% is certainly not correct. Check your mesh quality. You are using SST model, r u generating prism layer.
I am using RNG k-e since my mesh is all tet. My turbulence residual is not converging beyond E^-03 although mesh quality is >0.25. How good is your turbulence converging? Since its single phase flow I believe its turbulence that is causing convergence issue when all mesh quality factor are good. Can u attach pictures of your residual plots.
The convergence slowing down or stopping is a FAQ: http://www.cfd-online.com/Wiki/Ansys...gence_criteria
I will go through the accuracy and convergence FAQs, thank you.
Mat_Cfd, attached are my residual plots.
What is a prism layer? Are you referring to mesh inflation or something else?
I'll check my mesh and ensure it is of high quality.
my mesh metric are as follows:
~1.8M elements, 430K nodes
5 inflation layers, 0.05" thick first layer
I donít know which preprocessing software u r using. I used ICEM CFD . Your lower limit for quality and skewness looks problematic for that software. They should be above 0.2. But your residual look good provided that u r using high resolution. U can run it more say abt 500 itrns. Also plot monitors( mas flow , velocity) separately as they have diff limits.
Also as per your velocity monitor one inlet is behaving as outlet with hardly any flow going out through actual outlet you specified in CFX. Check ur Flow streamlines.
By prism layer( in ICEM CFD) I mean boundary layer which seems to same as Inflation layer u r taking abt. I wish to know where all ur are growing boundary layer and r u able to get the required mesh quality in Fan region and other are with sharp turn.
Both inlets are flowing correctly - one is negative because the flow is going in the negative y-direction, since this fan design has two inlets which are opposed (The monitor point is an expression, AreaAve(Velocity v)@Inlet1 and Inlet2).
The outlet velocity monitor is actually not appropriate - I mistakenly made the expression AreaAve(Velocity v)@Outlet, but the flow is in the z direction.
As for my mesh metrics, I agree that the mesh quality could be better. The skewness, if I remember correctly, should be as low as possible, so the upper limit of 1 probably could be improved (not the lower limit).
As for the inflation layer (prism), I am inflating all surfaces except the inlets, outlet and domain interfaces. I've attached a couple of screenshots.
For monitor I am saying, plot mass flow separately as it might of order 0.1 to 0.2 kg/s and see if its oscillating or stabilized.
I am facing the same issue in these blower fan simulation
2. Why do the residuals flatline while imbalances and monitor points seem to converge?
As suggested in FAQ we locate max residual are in output file and coarsen the mesh there if there is vortex or recirculation issue there. See if u can find time to try it in your geometry.
It seems from your pics that you have boundary layer on blade as well as all wall surfaces. Skewness in ICEMCFD that I am using for making mesh is defined other way round , so u may have to improve elements on higher side. But I suppose skewness will be issue for inflation layer. You can try with only tet mesh , which certainly would of higher quality and compare two results.
I wasnít able to develop inflation layer in my geometry as I have fan with curved blade profile and also there is big geometry after volute casing. In case you are able to try it or improve convergence issue let me know abt it.
There is also a FAQ on accuracy: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F
Still having some issues with this simulation, so in an attempt to rule out a bad mesh and to quickly get some results, I have setup a simplified simulation.
Instead of a full 3D, I am doing a 2D-type simulation using CFX - basically one element thick (as the help suggests), with symmetric BCs on both sides of the 'slice' of the geometry.
Further, I have eliminated the volute and have replaced it with a simple 'ring' stationary domain, with the outlet on the outer circumference. The other stationary domain is also a ring, with the inlet on the inner circumference. The rotating domain contains the blades, as before and is rotating at 1750 rpm.
My boundary conditions are the same as before: Total Pressure Inlet, Static Pressure Outlet, with the addition of the symmetry BCs to account for the 2D slice.
The mesh quality this time around is quite good, since I can afford to use fairly small elements around the blades without getting a huge mesh. See below and attached screenshot:
| Mesh Statistics |
| Domain Name | Orthog. Angle | Exp. Factor | Aspect Ratio |
| | Minimum [deg] | Maximum | Maximum |
| Rotating | 64.3 OK | 4 OK | 3 OK |
| Stationary | 73.0 OK | 2 OK | 2 OK |
| Global | 64.3 OK | 4 OK | 3 OK |
| | %! %ok %OK | %! %ok %OK | %! %ok %OK |
| Rotating | 0 0 100 | 0 0 100 | 0 0 100 |
| Stationary | 0 0 100 | 0 0 100 | 0 0 100 |
| Global | 0 0 100 | 0 0 100 | 0 0 100 |
CFX Pre Setup:
This is a steady state simulation, auto timescale, SST turbulence model, air at 25C. The interfaces between the rotating and stationary domains are set to 'Frozen Rotor', 'General Connection' and 'GGI'.
The momentum and mass and turbulence residuals flatline above 1E-3, imbalances are less than 0.25%, monitor points converge nicely except for the total pressure at the outlet.
Walls are put up on the outlet, due to recirculation...this is not totally unexpected since the air coming off the blade tips is mostly moving in the tangential direction. What is unexpected is that the flow vectors show a very non-symmetric behavior (around the axis of rotation of the impeller). See attached screenshot.
Why would this occur and is it related to the inlet/outlet BCs? This same behavior was observed when doing the full 3D with volute.
I looked at a Fluent tutorial that is 2D (it does include a volute), and those results show a nice, even flow coming out of all the blades.
There has got to be a simple explanation for this!
The convergence flatlining is discussed in the FAQ: http://www.cfd-online.com/Wiki/Ansys...gence_criteria
Have you read it? I have already given this link before in this thread.
Your mesh is very coarse. I would not trust anything from a mesh that coarse. Refine the mesh and then do a mesh sensitivity check to see what is required to make it accurate.
yes I have read the FAQ. More than once, in fact.
Turns out it was in fact something simple - the coordinate system was not centered on the axis of rotation. I had the right axis selected in Pre, but it was some 6 inches from the center of the impeller.
I don't understand why the solver never threw an error as one thinks it should.
Now that I fixed this, it works like a charm - residuals come way down (1E-5), monitor points converge, no recirculation at the outlet and the flow is symmetric around the axis of rotation.
For future reference, is there a way to display the default coordinate system in Pre?
|All times are GMT -4. The time now is 18:54.|