[tufygo]

i have a discs which i have to rotate,is anyone have a tutorial?

thanks
with respect

[ghorrocks]

Tutorials on immersed solids are available on the ANSYS customer webpage.

But if you are modelling spinning discs you do not need immersed solids to do this. A normal wall boundary with a tangential velocity will model it much more accurately and more easily.

[tufygo]

Originally Posted by ghorrocks

Tutorials on immersed solids are available on the ANSYS customer webpage.

But if you are modelling spinning discs you do not need immersed solids to do this. A normal wall boundary with a tangential velocity will model it much more accurately and more easily.

thanks for reply,but i am wondering how can normal wall boundary with a tangential velocity is more accurately ? because discs are spinning with flow,i mean discs are influencing flow after that starts turning so that disc velocity is not same during the process,it's changing with time,if i define wall boundary with a tangential velocity disc velocity will always same.Also i wil do tesla disc turbine simulation so disc space will be small so that boundary layer effects the rotation.Thanks a lot
with respect

[ghorrocks]

You can make the tangential velocity a function of time or anything else you like. It does not need to be constant.

A normal wall with a tangential velocity is more accurate when applicable as you can mesh proper inflation layers and get good resolution on the boundary layer. You cannot do this nicely with immersed solids.

[tufygo]

Originally Posted by ghorrocks

You can make the tangential velocity a function of time or anything else you like. It does not need to be constant.

A normal wall with a tangential velocity is more accurate when applicable as you can mesh proper inflation layers and get good resolution on the boundary layer. You cannot do this nicely with immersed solids.

thanks a lot for answer
i think discs torque higly related to flow momentum and boundary layer effect how can i define tangential velocity which is related to boundary layer effect and momentum ?
UDF?
with respect

[ghorrocks]

You can define a tangential velocity in the CFX-Pre GUI using simple CEL expressions. It is very simple stuff.

[tufygo]

Originally Posted by ghorrocks

You can define a tangential velocity in the CFX-Pre GUI using simple CEL expressions. It is very simple stuff.

Thank you for your kindness. Im so sorry to make it so long but read the comments that I wrote before, I think I need to explain more. I need to simulate tesla turbine. The disc rotations are driven by the flow. So, we do not know the tangential velocity at each point exactly. Also, In tesla turbine, motion of the discs are directly related with boundary layer flow. We must not model boundary layer, we have to solve it. Boundary layer mesh resolution must be very fine.

I think we have 3 options. One is immersed solid, second is overset mesh in fluent third one is to use dynamic mesh. But third option is a heavy and complex solution. Under the lights of these info, is there any recommandations ?

Thanks in advance

[Gert-Jan]

Why do need such complicated approaches? It looks like you trying to kill a mosquito with a bazooka. Really unnecessary.

For this application:
- Forget Immersed Solid. By far not accurate enough.
- Forget Overset mesh. Too demanding in terms of computer resources since it requires very small timesteps (at least in Star-CCM+).
- Forget Dynamic meshing. Unecessary complex.

As Glenn already mentioned the only option is: Let your domain with Tesla Turbine rotate with an increasing speed (CEL Expression) and let the outerwall counterrotate to have it stand still. Use a fine mesh it you really need to solve the complete boundary (Y+<1?).

You write that the flow drives your turbine. How can flow drive a Tesla turbine? That is almost impossible since the discs are flat. You have tangential inlet? Even then the torque will be small.
Nevertheless, in the simulation you have to set a rotational speed. This can be a function of the (by CFX calculated) torque on all discs (and shaft) using a CEL expression.

[tufygo]

Originally Posted by Gert-Jan

Why do need such complicated approaches? It looks like you trying to kill a mosquito with a bazooka. Really unnecessary.

For this application:
- Forget Immersed Solid. By far not accurate enough.
- Forget Overset mesh. Too demanding in terms of computer resources since it requires very small timesteps (at least in Star-CCM+).
- Forget Dynamic meshing. Unecessary complex.

As Glenn already mentioned the only option is: Let your domain with Tesla Turbine rotate with an increasing speed (CEL Expression) and let the outerwall counterrotate to have it stand still. Use a fine mesh it you really need to solve the complete boundary (Y+<1?).

You write that the flow drives your turbine. How can flow drive a Tesla turbine? That is almost impossible since the discs are flat. You have tangential inlet? Even then the torque will be small.
Nevertheless, in the simulation you have to set a rotational speed. This can be a function of the (by CFX calculated) torque on all discs (and shaft) using a CEL expression.

thanks for your answer

https://www.youtube.com/watch?v=mrnul6ixX90

in tesla turbine purpose is finding of the shaft rotational velocity and with that finding of power.
i dont get it ,if you define tangential velocity by yourself you cant define all of those effect
with respect

[Gert-Jan]

Nice video, but you have an ill posed problem and should think for yourself first.......

The velocity of your turbine is determined by balance of the energy you put in (tangential inlet) and the energy you take out. So you need to know what is it drving and how much torque this requires.........
- Is it driving a dynamo? This will result in a low speed.
- Is it nothing, meaning freely rotating in the air? This will result in a high speed. But then you need to know the friction of the seals and include the drag with surrounding air.

You somehow should provide CFX with this input. Don't expect CFX, to know the application beforehand and sets the rotational speed for you.

[ghorrocks]

The normal way of determining operating speed in devices like this is you simulate a range of operating speeds and get a torque versus speed function. You then look at your system and determine the torque versus speed function for the system it is driving. Where the turbine function intersects the system function is your steady state operating point.

[tufygo]

Originally Posted by ghorrocks

The normal way of determining operating speed in devices like this is you simulate a range of operating speeds and get a torque versus speed function. You then look at your system and determine the torque versus speed function for the system it is driving. Where the turbine function intersects the system function is your steady state operating point.

i am sorry but i cannot understand how can i do that

[ghorrocks]

You simulation a range of rotation speeds as steady state (possibly frozen rotor) simulations. You extract the torque on the rotor to get a torque versus speed curve. Then you plot your system torque versus speed curve and the intersection of those two curves is your steady state operating point.

[tufygo]

Originally Posted by ghorrocks

You simulation a range of rotation speeds as steady state (possibly frozen rotor) simulations. You extract the torque on the rotor to get a torque versus speed curve. Then you plot your system torque versus speed curve and the intersection of those two curves is your steady state operating point.

i hope i understood , i am starting simulations