Compressor simulation issue
 

Hello,

I have a following problem. When running compressor simulation, I cannot get some points to converge. In general this problems occurs in the middle of the measured maps, but at this point the measured speedlines are already falling down or horizontal. it generaly falls on overflow problem.
Is there a way how to change the criterions to prevent the simulation from falling? When i watch the measured parameters etc. evertyhing seems reasonable.

Thanks
Vit

Solver divergence can happen due to a lot of reasons: boundary or initial conditions, solver parameters, equations modeled.

First of all you should take a good look at the best practices:
http://www.cfd-online.com/Wiki/Best_...omachinery_CFD

The CFX documentation also has guidelines that you should check out.

Cheers

This is not that helpfull. Obviously you follow the general standards. The thing, that is missing is for example how to pick the boundary conditions when simulating compressors. For example using static pressure on the outlet is difficult as if you see some of the maps, they do have 2 solutions. If you use mass flow, then you can select a value in the choke?

There is also turbo machinery best practices guide in the CFX documentation. Have you read that?

I am not sure. Is it possible to find it on ansys customer portal?

I wasn't talking about general standards, I was talking about guidelines for simulating compressors. The link I posted has some general guidelines for turbomachineries, but the CFX documentation has specific best-practices for compressors. That includes boundary conditions on choked flows. The documentation can be found at the menu under 'Help > CFX > Contents'. You shouldn't disregard people's comments before you check out what they advise you to do.

Anyway, something else you can do past choking conditions is work with a corrected mass flow. You set a value for thought a CEL Expression and use that value on a second CEL Expression to set this at the outlet:



where




and and are evaluated at the outlet.

With this approach you should be able to set values of corrected mass flows that go past the choking conditions. The solver should adapt pressure and temperature so that they fit the you set. Still, you should first try what the guidelines at the documentation suggests.

Cheers.

Hello,

no, my intention was not at all to diregard someones help. I obviously checked the best practices, but I didnt find anything, that would be usefull in this case. The problem is not occuring at choke, but at the middle of the map. I tried various types of boundary conditions, but no success so far. I am using v12.1. The boundary condition, that I would like to have is pressure loss on the outlet, but this is not possible to use for the outlet type. Only for opening.

V.

I wanted to impose same boundary condition, my question is that I know Wabs, but Ptout and Ttout would be updated in every iteration?
So i need to write expression to update it in every iteration?

Regards,
Saima

and are calculated by the solver. You can create an expression to take their values either locally or by using an average at you outlet condition.

So this expression would be enough:

T02=massFlowAve(Ttotstn)@R1 Outlet
P02=massFlowAve(ptotstn)@R1 Outlet
Wabs = 1.517 [kg s^-1] ;
massflow= Wabs*((sqrt(T02 /288.15 [K])/(P02/101325 [Pa]))

Then i'll choose outlet boundary condition this expression under mass flow. I found another option below that which is "Update Mass Flow", do i need to check on that too? If yes then under which option constant flux?

Thanks in advance!!!

You should, since your boundary condition is not linear. I think it does it by default, but enable it just to be safe.

I don't recall the options for it, so you should check the documentation to see which one to use.

Yes, you are right by default it is enable.

I am running fan optimization by assigning corrected mass flow on exit boundary condition, in every evaluation geometry is changes and I want to assure to have same corrected mass flow. If i re-calculate exit corrected mass flow at the end of solution, i noticed it is not constant. It varies. I want to understand it.

I am not getting the reason how by assigning the corrected mass flows that go past the choking conditions? What is the physical significance?

Thanks in advance!!!

Once you reach choke, mass flow can no longer be increased. But the corrected mass flow also takes local pressure and temperature into account, so even though your actual mass flow is fixed, by varying local temperature and pressure you corrected mass flow can still increase.

That's what I meant.

Hello brunoc,

Choke is not my concern.i use either static pressure or pressure loss at outlet condition . The problem happens approx.in the middle of the measured map where speedline has more or less horizontal direction.

Hi Vit,

That probably means that for a small change in pressure you can have a large difference in mass flow. If that is the case, you should consider setting a mass flow at your outlet region. That will make your case more robust.

Cheers

Hello Brunoc,

no matter what BC I use ( pressure, mass flow etc.) the issue is following:
the simulation runs ok to some iteration - 200-300 and then when all the residuals are already quite low, the momentum in one direction starts to increase and after few iterations, the simulation stops.

V.

This usually means the flow has progressed enough so some tricky flow feature has reached a critical point. This could be a separation reaching an outlet or the inlet fluid first reaching the outlet.

I would save a few intermediate results files leading up to the crash to find out what flow feature is causing it. The fix will almost certainly be to move the outlet boundary further downstream.

Hello,

I have updated this boundary condition & have few blades with same exit corrected mass flow, even though there abs mass is varied.

I have two basic queries:

1. What is forced CFX to keep same exit corrected, I really don't get what is going on behind, how can it is ending up with same exit corrected mass flow only by imposing a simple expression?

2. When I get the blade with exit corrected mass flow, I run the speed line for that by varying P2 at outlet but I have not found the same efficiency that was with exit corrected mass flow boundary. There is a small difference for example it varies from 0.9118 to 0.9109. Can you tell me why is that?

Thank you very much for comments!!!

1. You are prescribing an outlet mass flow that is a function of a constant corrected mass flow and varying outlet pressure and temperature. If outlet pressure and/or outlet temperature changes, you get a change in mass flow, even though the corrected mass flow value did not change.

2. I'm not sure I understand what you meant when you said "varying P2 at the outlet". Does it mean you are using a pressure outlet to see ir the results match against the one with a mass flow outlet? If so, remember that on the mass flow outlet result you probably have a non-constant pressure field, so using a constant outlet pressure on another case would give you a different result. You should export both pressure and temperature fields and use those as boundary conditions. Ideally this should give you the same results as the one with the mass flow outlet.

Yes, right. I wanted to draw speed line for that blade. That means now I have to take mass-flow on the exit if i want get back same efficiency on speed-line?