[dccfd]

Hi Everyone,

I am trying to simulate a drone midflight, which can be seen by the attached image and to do this I have used disks to simulate the rotors which I have made as two separate sub domains with an inlet and outlet. When I try and simulate it, I get the below error:

"If the isolated regions do not have the pressure level set either
by the boundary conditions or using a reference pressure equation,
you may encounter severe robustness problems.

This situation may have arisen because a domain interface was not
properly defined during problem setup. Please carefully check
the setup.

The solver will stop now and write a results file. The isolated
regions can be visualised in CFX Post by making plots of the
variable "Isolated Volumes".

If you are sure that the pressure level is set in each isolated
fluid region then you can force the solver to turn off this check
by setting the expert parameter "check isolated regions = f"."

I have been looking on other threads with a similar issue and other people have said that the domains are not connected. Can someone please explain how to resolve this, or should I just force the solver to turn off this check?

Any information you could provide would be greatly appreciated.

Thanks!

[ghorrocks]

The normal way of modelling something like a rotor blade is using a momentum source term. It is simpler and better models the true flow condition on the rotor.

Why are you modelling this with multiple domains anyway? It looks like it can be done in one domain to me. That would fix the isolated domains error straight away.

But to answer your original question - the error is because you have not put interfaces to join the domains up. You need to put interfaces in to join the domains up. But I would not bother, address the issues I mention in the previous two paragraphs and you will only have 1 domain anyway.

[dccfd]

Hi Glenn,

Thank you for getting back to me. The reason I did a sub-domain is that I wanted to simulate just air passing through these discs which meant I didn't have to simulate an actual rotating blade which would of had too many variables.

Is it possible to do this with the momentum source term? And if so how would I go about implementing it into CFX?

[ghorrocks]

Is it possible to do this with the momentum source term?

Yes. It is also much simpler and more physically correct than the approach you proposed.

For details on how to implement it look in the CFX documentation and search this forum. I do not know of any tutorials which use it unfortunately.

[dccfd]

Hi Glenn,

Sorry to bother you again but I am quite stuck on these momentum equations. I want to simulate air passing through those discs, going at a velocity of 20m/s, they have a radius of 0.2m, they're 0.01m thick. How would I go about solving the equations for the x-momentum, y-momentum and z-momentum? Or would it be easier to put into cylindrical co-ordinates?

Any advice you could give would be greatly appreciated.

[ghorrocks]

Do you want the rotors to generate a flow of 20m/s? Or do you want to use a fan curve?

You don't solve the equations with momentum source terms, you just add a new factor into the equations which acts as a momentum source (or sink). So continuity and everything else is still conserved, it is just the momentum in the source term region is modified to reproduce the momentum added to the flow by the rotors.

[dccfd]

I don't have a fan curve for the rotors, so them just producing a flow at 20m/s would be my best bet.

What would be the inputs at this stage?

[ghorrocks]

Make sub-domains of the rotor regions. Use one domain for the entire thing, but the rotors need to be in sub-domains.

Set the momentum source term in the sub domain to:
X: 0
Y: -C*(v-20[m/s])
Z: 0
Source term coefficient: -C

And set C to a large number, say 1e6.

[dccfd]

Hi Glenn,

Thank you very much for that, everything is running now. Just one more thing, is it possible to input the momentum source as a force rather than a velocity?

[ghorrocks]

Yes, but it is a force per unit volume. You have to be very careful about units with source terms.

[dccfd]

So I would be able to simulate a thrust in terms of force, as I know the volume of the rotor? What would an example be of the equation for the force?

[ghorrocks]

Well, the total force applied by the source term would be the source term times the volume the source term is applied over.

[dccfd]

Hi Glenn,

I have be running the simulation with the following values for my source term in the x,y and z:

The X: 0
The Y: -1.992e7 kg m^-2 s^-2
The Z: -1.743e6 kg m^-2 s

With a source coefficient of 1e6, as you recommended.

I used the equations that you said to above, and then broke the 20m/s into its respective component (Y and Z, at 5 degrees).

In my post processing, this is yielding a 600m/s at the rotors which I don't understand why.

Could you please provide some insight as to why this might be happening? And possibly how to correct it?

[ghorrocks]

For those momentum source terms the momentum source term coefficient should be 0.

Read the documentation on setting the momentum source term coefficient - it should be equal to the derivative of the source term function WRT the equation variable.