Community
CFD Forum
Welcome to Autodesk’s CFD Forums. Share your knowledge, ask questions, and explore popular CFD topics.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

spinning disc in sim cfd

17 REPLIES 17
Reply
Message 1 of 18
robert.camilleri
479 Views, 17 Replies

spinning disc in sim cfd

Hi, I'm trying to simulate a spinning disc in sim cfd.  the idea is to be able to get a value of the heat transfer coefficient from a spinning disc.  however i was wondering if it would be possible to model just a quarter of the model (to make the model easier/faster) and what should the boundary conditions that allow this be. thanks. rob

17 REPLIES 17
Message 2 of 18

Hello, has anyone tried to simulate heat transfer from a spinning disc in autodesk simulation please? thanks. rob

Message 3 of 18

Hi Rob

 

Are you looking at cooling also? Or does the disc stay at a constant temp?

Without knowing the orientation of the disc in the air it is hard to say how best to run this, could you upload a sketch?

Message 4 of 18

Rob,

 

A spinning disc could be done with motion, or it could be done with a rotating region.

 

I would use the rotating region over motion as it will be more stable.

 

For 1/4 you could slice it and then use Periodic Boundary Conditions for the planar faces of the cut to represent the matched set (check out the help as we do walk through looking at 1 blade of a fan with a rotating region and periodic conditions).

 

Alternatively, depending on what you are striving for, you could also setup the model as SteadyState with a Rotational Velocity BC assigned to the 'spinning' faces of the solid and not sure motion/rotating region. If you chopped it in to 1/4 you would still need the Periodic conditions though

 

More information could better help us direct you

 

Apolo

Message 5 of 18

Hello,

In my problem I am trying to run the transient motion simulation for a disk about its centre of revolution, speed at 40rad/s - please see attachment pic of the disc spinning around its centre of revolution in a bigger disc of air (hidden).  i would then like to determine the heat transfer coefficient (HTC) on the disk so will have to run a thermal analysis.  

 

here are the problems i am facing at the moment:

1) for the whole disc, i tried to calculate the Reynolds number and HTC from my previous analysis, but there seems to be a discrepancy in both when compared to theory.  can you please advice what the dimensionless length in the Reynolds and Nusselt number is normall taken in Sim CFD?

2) when running the thermal analysis, should the solution be switched to steady state? - (when the motion analysis is solved this will be in transient)

3) will it be best to apply an internal heat load or constant wall temperatures on the disk walls?  

 

4) inorder to make the simulation quicker (or increase the mesh size), i have also attempted to run a quarter of my model but has been unsuccesful because i get air filling the void left by the disc once this passes through .  can you pelase advice on how the periodic and slip conditions should be?

 

attached is a pic of my whole model.  

 

cheers, 

rob

Message 6 of 18

Robert,

Please check the Help as we walk through how this would be done for Periodic.
As I referenced in my previous post, for Periodic we would use a Rotating Region for the movement, not Solid Motion (using the Motion dialog)

 

We would solve the model as Transient for both flow and thermal. when you switch back to steadystate if you still have the rotating region (or motion) assigned this can complicate how the solution is computed.

 

What you may want to try is what I was leaning towards

 

SteadyState model with Rotating Velocity boundary condition on the spinning faces

you could have a heat generation to the solid.

 

For thermal you would need some other thermal condition (like an inlet temperature) but you could then run this as SteadyState Flow and Thermal.

 

If you are looking to get the HTC from CFD, use the wall calculator and select the surface of interest, uncheck the box (Use Near Wall Temp) and specify a reference temp - such as your inlet) and see what the HTC is reported

Message 7 of 18

thanks Apolo,

one last question: since the air is not a closed region, as with your impeller example, am i right to think that my model will now require to have the disc, enclosed in rotating region - enclosed in air? cheers, rob

Message 8 of 18

If you are going to do the rotating region, yes you would need to cad that volume

 

Disc - Rotating Region - Air

 

 

If you tried the steady state approach, you would not need additional volumes.

Message 9 of 18

Dear Apolo, 

thanks! both of these solutions seems to work though i quite prefer the rotating region solution.  just to be clear, can you please advice when you would use the motion and not the rotating region?

 

Also moving on to a more complex situation... Would it be possible to use the rotating region say with air together with a liquid flow?  for instance in an electric motor you may have part which requires a rotating region but another part which will be liquid cooled (totally independent and separate of the rotating region) - could you please advice if this would be possible and how would you go about it?  

 

Last note... can you please advice where i can find a better mathematical explanation of the effect of the near wall button on the HTC?  perhaps somewhere on the guide which i am missing?

 

thanks! rob

Message 10 of 18

If the object is spinning continually i tend to use Rotating Region

Solid Angular motion, I'll use for small angles (such as valves / partial rotations)

 

I cant say that I follow your description of the more complex situation.

We cannot have air and water both in a simulation that uses teh same rotating region.

 

You can have an "air" side of the model that has a rotating region as well as a 'water' side taht could contain a 2nd rotating region. These two fluid domains air vs water would be isolated by some solid material such that they have their own independent inlets and outlets.

 

 

Film coefficientcan be calculated in two ways:

  • Enter a value for the Ref. temperature. The film coefficient is calculated based on the heat flux and the temperature difference between the specified reference temperature and the wall temperature.
  • Use the near wall temperature at every wall node as the local reference temperature. Check the Use near-wall temperatures box. The film coefficient will be based on the difference between the wall temperature and temperature at the closest non-wall (flow) node for every node on the wall.

Think of the basic equation for a Convective Coefficient, the Tsurface - Tx, where Tx is either a Refernce Temp or the Near Wall Node. The Near wall node will typically generate a smaller dT such that h will be larger vs using a specified Reference Temp.

Message 11 of 18

Hi Apolo, quick question please... my CFD results with rotating region seems to have a very oscillating residual velocity (please see pic attached).  i generally know how to solve saw tooth residuals by relaxing moving pressure and velocity sliders, but was wondering if you could help on this.  is this a similar issue or is it a meshing/other issue?  cheers, rob

Message 12 of 18

Rob,

Yes this is typical with rotating regions. As the in-plane rotations (normal to the axis of rotation) will generate oscillations. We would not want those to be 'flat' more so than trying to ensure that they stay stable and do not grow unbounded.

 

 

Message 13 of 18

Dear Apolo, 

i am still trying to model a quarter model of a disc-rotating region-air as suggested in a message earlier, however through my simulation the velocity scale seems to be going far higher than the v=R.angular speed that it should be going to, which to me suggests that something is not right0.

 

can you please advice if this normal during the simulation or could you possibly identify possible causes.

 

My boundary conditions are: slip on disc, periodic on rotating region and slip on the air, with the rotating region set to a constant 40rad/s.  solve is set to transient with 90degrees per iter.  your input is very much appreciated. thanks. rob

Message 14 of 18

Rob,

  Lets for visual aid say you modeled 1/4 of the disc.

 

You would have the 1/4 disc volume, rotating region volume and air domain

 

On the planar faces of the Rotating Region and Air, you should assign Periodic Boundary Conditions (Be sure to pay attention to assigning proper Side # Pair # to the faces - This is outlined in the Help)

There should not be any Slip BCs on the disc

 

I would also use something slightly smaller than 90º as that can be quite a large timestep.

 

Try ~10º to be a little more detailed in capturing the flow solution

Message 15 of 18

thankyou will try this.  can you recommend also a number of inner iterations? thanks rob

Message 16 of 18

Default for rotating regions and motion is 1

 

Message 17 of 18

Dear Apolo, 

Many thanks for your advice earlier.  these boundary conditions seem to work well now, however it seems that when mesh enhancement (3 layers) is applied, an incorrect velocity magnitude results.  Should mesh enhancement be completely switched off during rotating regions?

 

Also the does a rotating region simulation typically converge as in normal flow? I have given this simulatin about 1500 time steps (and still running) but it still seems far off from converging (although the residuals are very smooth - no sinusoidal shapes or sawtooth).  Is it simply a matter of more time, or the mesh being still too coarse, or should i set a stop time instead of -1 ?

 

cheers, 

rob

Message 18 of 18

Robert,

  Mesh enhnacement should not be taken off. We typically turn it off for motion, but we will keep it for Rotating regions (as that is one of the benefits of Regions over motion).

 

You may want to check the mesh quality (as your mesh could be too coarse) to properly capture the effects of the spinning disc.

 

hard to say 1500 iterations, for a spinning disc it will typically take a certain number of rotations (depending on timestep size, that will give you the number of iterations). For fans/pumps we tend to talk about an average of 5-15 revotutions for the flow to develop, with just a flat disc splinning it could be similar range, but you'd have to watch the details in the domain

 

Now the solution will not auto-stop like SteadyState, you will have to manually assess convergence based on the solution and the gradients within the domain.

 

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Autodesk Design & Make Report