[jpc]

i have an assembly that is composed of a tunnel with 2 props within it
the props are held on the axis of the tunnel by a support that is connected to the top of the tunnel

i have placed this in a large environment composed of water
but i'm not familiar with autodesk 360 CFD's boundary conditions for this type of case

in SolidWorks flow simulation the boundary of these faces would automatically have an infinity condition applied to them, which seems similar to an "unknown" boundary condition.

however similar problems have been setup with pressure condition at both ends with 0 gage static pressure. and on the other faces "slip" condition applied. (similar to a wind tunnel where the walls have been ignored)

this seems reasonable but something inside me thinks that one side should be static gage 0 and the other should be total gage 0.

let me know what you think

[matt.brown.ae]

I am not sure I understand what you are modeling. Can you post a shot of your geometry? Your description says external but then you talk about a tunnel. I want to make sure I understand what you are trying to model before discussing boundary conditions.

[jpc]

hope this helps

brown is a boat
boat is on the surface of the water
it is propelled by the double prop thruster

so from an analyis perspective, you could run it as an internal analysis where your BCs are at the end of the "tunnel" the props are in
or you could put the tunnel in a larger environment to minimize those end effects

[matt.brown.ae]

If I understand correctly, you are only concerned with what I have boxed in, (i.e. the ducted propeller)?

If you knew what the inflow conditions were at the front of the duct you could probably get away just modeling the inside of the duct. However, the velocity distribution at the inlet is going to be a function of (a) the velocity of the boat, (b) shape of the inlet lips (i.e. round, blunt, sharp) and also whatever effect the boat itself is having on those distributions.

Also, I am not sure that Simulation CFD will model the liquid/gas interface at the water surface. You will probably need a more sophisticated piece of software for that, however, I could be wrong. I have never tried it myself.

What I would recommend is modeling the duct by by itself surrounded by a massive circular fluid volume that is at least 10 times the diameter of the duct and extends 5 diameters up stream and 10 diameters downstream. On the forward circular face and cylindrical faces of the fluid volume apply velocity at whatever magnitude and direction the boat is traveling. On the aft circular face apply a zero gauge pressure BC.

I am sorry if I am still off base with this. However, I have had success modeling ducted turbines using this approach. Just keep in mind that Simulation CFD doesn't always give good results, even for the best of models.

[matt.brown.ae]

Forgot the attachment.

[jpc]

the water surface isn't important. we can assume the thruster is significantly deep enough that the surface effects are minimized and also that the water is deep enough that the bottom effects are minimized and also that it is far enough from shore that those effects are minimized.

regarding your approach, that is basically the approach that I used in both Adesk360 and solidworks flow simulation. except that i used a box.

is there a reason you didn't apply a boundary condition to the cylindrical wall? wouldn't those be considered no-slip walls? from the documentation, they currently act like the walls of a wind tunnel. if your comp domain is large enough this probably isn't an issue, but still curious.

second, if the boat was being held to the shore by a rope such that it was stationary. would you still apply a velocity? or would you apply something else to have the flow in the model (inlet and outlet) be specifically developed by the rotating blades?

third, is static pressure = 0 an "open condition"? meaning that both at the inlet/outlet it will converge to a solution or does it force that pressure to be 0Pa static pressure and only converging to a solution at the inlet where the velocity is?

[matt.brown.ae]

see comments in red

the water surface isn't important. we can assume the thruster is significantly deep enough that the surface effects are minimized and also that the water is deep enough that the bottom effects are minimized and also that it is far enough from shore that those effects are minimized. Ok, so no boat and no sea (or lake) bed.

regarding your approach, that is basically the approach that I used in both Adesk360 and solidworks flow simulation. except that i used a box. Box vs cylinder makes little difference, other than it reduces your computational domain a little. I usually use a box if I am doing external aerodynamics for an aircraft and a cylinder if I am doing wind turbines or propellers.

is there a reason you didn't apply a boundary condition to the cylindrical wall? wouldn't those be considered no-slip walls? from the documentation, they currently act like the walls of a wind tunnel. if your comp domain is large enough this probably isn't an issue, but still curious. Perhaps I confused the issue. The cylindrical face and the upstream circular face will have free stream velocity. The downstream circular face will be zero (gauge) pressure.

second, if the boat was being held to the shore by a rope such that it was stationary. would you still apply a velocity? or would you apply something else to have the flow in the model (inlet and outlet) be specifically developed by the rotating blades? Here you would want to replace the freestream velocity BC's (cylindrical and upstream circular faces) with zero velocity in all three components. If your domain is properly sized you should be far enough away that these faces remain unaffected by what your prop is doing. The prop will pull fluid in and push it out the back toward the zero pressure (outlet) face.

third, is static pressure = 0 an "open condition"? meaning that both at the inlet/outlet it will converge to a solution or does it force that pressure to be 0Pa static pressure and only converging to a solution at the inlet where the velocity is? the static pressure = 0 (i.e. zero gauge pressure) is just a numerical way to define an outlet. You will probably not want to put this on the upstream circular face as it will most likely not converge.

Despite the fact that you have a ducted propeller, this is really an external flow problem because you are looking at the impact of not just the prop, but also the duct on the flow. I have modeled wind turbines, ducted propellers and aircraft with (admittedly mixed) success using this method.

Hope this helps,
Matt

[jpc]

hi matt, when i say "cylindrical" face (vs circular face at the ends), i'm talking about the cylindrical boundary. essentially the boundary to the rest of the environment. i would expect this to either be a slip condition or static pressure = 0.

as for the opening velocity = 0, that is an interesting idea. i'm surprised that would converge any better than setting static pressure = 0.

[matt.brown.ae]

I have never tried to use zero pressure on the cylindrical face. It might work, but I just don't know. All of the external flow analysis we do is accomplished in the manner I described. The company I work for was actually one of the first to use the original CFDesign (now Simulation CFD) for this type of analysis. The boundary conditions were direct recommendations from the original software distributer. They have some decent example which show setup using this method, or at least they used to.

As for slip/symmetry I think that is a wrong choice. Here is what the help files say about this BC:

'The slip condition causes the fluid to flow along a wall instead of stopping at the wall, which typically occurs along a wall. Fluid is prevented from flowing through the wall, however. Slip walls are useful for defining symmetry planes. The symmetry surface does not have to be parallel to a coordinate axis.'


If you have any success using zero pressure, I would be interested to know.

[matt.brown.ae]

Also, on the zero velocity BC for the static case: I have never actually had to model this. All of our analyses have a forward speed. My recommendation of zero velocity is pure speculation. I would actually need to run a case or two to get a feel for how that would behave.

[matt.brown.ae]

Another option is to do a model with periodic symmetry. Here you can cut up your model and domain to isolate one blade and the corresponding section of your duct. So for a 3 blade model you will only model 120 deg of the annulus. (Think of a slice of pizza or pie). On what is left of your upstream circular face and your cylindrical face you will define the freestream velocity condition like we discussed before. Same deal on what is left of the downstream circular face, you will apply zero pressure.

The trick here is to apply periodic symmetry (simply called 'periodic' in simulation CFD) to the flat faces of the fluid volume. Read the help files for more info on this. There used to be a decent example they distrubted with the software for an axial fan back when it was called CFDesign. I am not sure if that example is still distributed with the software or not. If you cannot find it and are interested, let me know and I will elaborate.

[jpc]

it seemed to solve fine with zero pressure BC on the front. i didn't get to try zero velocity though.

as for the zero pressure on the cylindrical face or a slip condition, when i had nothing, it treated it like a solid wall. since I didn't have a HUGE computational domain, that may have affected the results. i think it would be best to have A BC there if your domain isn't huge but if it is, it probably doesn't make a difference. in flow simulation we'd leave that as an "open" condition (default BC for external analyiss) if we used an external analysis, if there was a real wall, you'd treat it like a wind tunnel and run it separately and remove that part of the data or run with slip condition (ideal wall) which isn't something you could do in a real wind tunnel.

the idea of periodicity is interesting. i've never attempted that with a frozen rotor or moving mesh solution. i'd be weary of the results on that one.

thanks again for all your insight.

[satishorion]

Hi,
I am also trying to solve a ducted propeller problem. I am the problem with estimation of thrust using Fluent. I tried the direct normal force on the prop surfaces and also the momentum balance approach. The results are different. How to estimate the thrust for the ducted propeller cases?

Regards
Satish