[jhtcten]

Hello all,

I am looking to simulate a very simple model of an amphibious model. I've attached a sketch to try to make things clearer. In any case, here are the specifics:

1) I am currently modelling just the treads - this has a constant linear velocity.

2) The treads are completely submerged in water.

3) There will be propulsion as a result, making the vehicle move in the direction indicated.

My questions are:
a) how would I set up the boundary condition for the treads? I know that it is essentially a moving wall boundary, but beyond that I'm lost. I don't believe that rotating frame of reference would work due to the unusual geometry.

b) I also assume this would be a transient simulation due to the forward motion of the vehicle. However, would it still be physically realistic to have a steady state simulation?

Thank you all in advance.

[ghorrocks]

If the device is reasonably stable in the water:

By far the easiest way to simulate this model is to model the device as stationary. Then the tracks are just a tangential velocity on those surfaces. A successful simulation will give you a thrust force, and you can repeat this for different values of the water flowing past the device (with the device still stationary) to get a thrust versus speed curve.

Once you have the thrust versus speed curve it is a simple matter to work out the acceleration, top speed and other motion parameters.

If the device is unstable in the water (ie it bobs about in waves and/or the thrust/drag causes it to pitch/roll/yaw): Then I think the best way to do this is with a rigid body. The thrust can come from a thrust versus speed curve or from a momentum source term.

[jhtcten]

Originally Posted by ghorrocks

If the device is reasonably stable in the water:

By far the easiest way to simulate this model is to model the device as stationary. Then the tracks are just a tangential velocity on those surfaces. A successful simulation will give you a thrust force, and you can repeat this for different values of the water flowing past the device (with the device still stationary) to get a thrust versus speed curve.

Once you have the thrust versus speed curve it is a simple matter to work out the acceleration, top speed and other motion parameters.

If the device is unstable in the water (ie it bobs about in waves and/or the thrust/drag causes it to pitch/roll/yaw): Then I think the best way to do this is with a rigid body. The thrust can come from a thrust versus speed curve or from a momentum source term.

Thanks for the reply!

By modelling the device as stationary, that means there will be an inlet velocity condition, which will be the speed the vehicle is moving in reality, correct?

However, if I just model this as flow around a stationary body, it doesn't give me the interactions between the moving treads and the propulsion generated. Related to that, how exactly would you find the thrust?

[ghorrocks]

You can model the moving treads. They would be modelled as tangential velocity on the tread surfaces.

[jhtcten]

Originally Posted by ghorrocks

You can model the moving treads. They would be modelled as tangential velocity on the tread surfaces.

I think I see what you mean now. But why are we specifying and inlet velocity? What if the boundaries are so far away that they don't affect the flow around the vehicle?

What I'm saying is in reality, the water is still. The vehicle is in the water, let's say it's stationary. Then the treads start moving - this creates flow around the vehicle, however the far field water conditions are still stationary.

I'm not sure if I expressed that properly...

[ghorrocks]

I think I see what you mean now.

I suspect not - but we are getting closer.

This type of model is much easier if you do it as a series of steady state simulations with known inlet velocities. Then you get a thrust versus velocity curve for the device and can construct velocity versus time and maximum speed from that.

But each of these models will have the inlet at the specified velocity, the initial condition at that velocity and the bottom face of the waterway at the velocity. So the fluid will flow from the inlet to the outlet regardless of how long the domain is. Then the device in middle will generate thrust and drag to give a net force. When that converges you have the net force at that speed, and just need to repeat this over a range of speeds.

As I stated in you first post it is possible to do this as a rigid body simulation where you start from zero motion and the device accelerates, but this simulation is much more complex and getting it accurate will be much harder than the simple way I describe.

So I recommend you do the simple method unless you can give a very good reason not to.

[jhtcten]

Originally Posted by ghorrocks

I suspect not - but we are getting closer.

This type of model is much easier if you do it as a series of steady state simulations with known inlet velocities. Then you get a thrust versus velocity curve for the device and can construct velocity versus time and maximum speed from that.

But each of these models will have the inlet at the specified velocity, the initial condition at that velocity and the bottom face of the waterway at the velocity. So the fluid will flow from the inlet to the outlet regardless of how long the domain is. Then the device in middle will generate thrust and drag to give a net force. When that converges you have the net force at that speed, and just need to repeat this over a range of speeds.

As I stated in you first post it is possible to do this as a rigid body simulation where you start from zero motion and the device accelerates, but this simulation is much more complex and getting it accurate will be much harder than the simple way I describe.

So I recommend you do the simple method unless you can give a very good reason not to.

Thank you for the in depth explanation. However, some things are still unclear.

1) What is the physical meaning of the inlet velocity? For example, say the inlet velocity is set as 6 m/s, and the tracks are set with a tangential velocity of 3 m/s.

If the inlet velocity is how fast the vehicle is moving in reality, shouldn't that be a function of the tread velocity? Or does the inlet velocity have a different meaning.

What I mean is, if the tangential velocity is set (since that's all we can control in reality), shouldn't that dictate the vehicle speed (and thus the inlet velocity)? Therefore, how can we set the inlet velocity beforehand?

2) Is there an easy way in CFX to set the tangential velocity? In the menu for a no slip wall boundary condition, when I select a moving wall velocity, I only see three options: Cartesian, Cylindrical, and Rotating Wall. This seems very tedious and complicated if I have a more complicated tread.

I've attached a picture of my geometry simplified even further - if I wanted a tangential velocity of say 6 m/s, I would have to use Cartesian components for the straight parts, and Cylindrical for the Curved parts, correct?

Thanks in advance.

[ghorrocks]

Inlet velocity is just the velocity of fluid entering through that boundary face.

You have to think of this thing as a system. For any forward speed of the device and track velocity it will generate a thrust force and drag force. The steady state speed will be when the thrust equals the drag, so there is no net force. If the device is slower than the steady state speed it will generate more thrust than drag and therefore accelerate; if faster than steady state speed there will be more drag so a negative net force and decelerate.

So the easiest way to simulate these devices is to choose a few forward velocities. From these simulations you will get the net force at different forward velocities. You can graph this and extrapolate to zero net force. That point is you steady state speed.

That is the easiest way to find the steady state speed from a series of steady state simulations at different assumed speeds.