[csaban]

I'm trying to compare the effect of using a brake duct on an assembly for an open wheeled racing car.

At the moment I only wish to setup a rotating ventilated disc in a stationary domain with an inlet of air at 50ms-1 and an outlet with 0 relative pressure. I am currently just running a steady state simulation and will go on to transient when I can get it working.

I'm working on the principal that a general connection frozen rotor with specified pitch angles of 360 degrees will enable me to see velocity change on a plane through the middle of the disc in post.

I believe that the interfaces are where I'm running into trouble as I get this message 1. The interface contains radial faces (parallel to the axis). |
| If this is the case, please split the interface into two parts, |
| so that the purely radial sections could be transformed |
| properly. The transformation type (axial or radial) is chosen |
| automatically based on the largest interface extent. |
| 2. This message may be generated because of a tolerancing issue |
| when the mesh resolution in the radial direction is very |
| small (e.g. at the hub or shroud). If this is the case, you |
| may ignore this message. |
+----------------------------

There are 30 cooling veins in the system and I have grouped theese into 4 groups of internal faces namely 'curve left, curve right, is faces and os faces'.
Any remaining faces have been grouped if they are parrallel such as each brake surface of the disc.

I'm currently using a sst turbulence model

Any help would be mcuh appreciated.

Thanks

[ghorrocks]

I would start this model, and do the basic sensitivity studies on a stationary rotor. This means it can be easily modelled in a single stationary domain. Once you have the parameters required for accurate simulation on this simple model then you should move to the more complex rotating model.

For the rotating model, I would have a domain which entirely encompasses the rotor and put a GGI on it. Frozen rotor should be OK for most circumstances. This will be much easier than trying to get the GGIs working for each passage.

Finally - I presume you don't need to model the heat transfer in the rotor. This means the rotor will be a cavity inside your mesh, not modelled as a solid.

[csaban]

Thanks for the reply ghorrocks,

Firstly, I do intend to eventually add brake pads in and apply the heat source at the contact surface. Then I wish to compare how after a given amount of time at speed (say 20 seconds at an average of 50ms-1) the temperature decreases with and without an inlet at the centre of the cooling veins.

I assume you are saying that I should set the disc to a temperature and the air inlet at 50ms-1 and ensure that the model is mesh dependant before moving to a rotating domain.

When you say 'a domain which entirely encompasses the rotor' do you mean I should boolean subtract the disc and create a two domains like that (i.e. a air domain with the disc perfectly sutracted. Or do you mean create a perfectly cylindrical domain slightly larger than the overall disc as i've seen in propeller tutorials on youtube.

I tried this technique with a simplified solid disc and found that air in the very centre of the disc would have an un-natural angular velocity. I expected to see rotation being effected by the rotating disc due to the no slip condition on the disc and the viscosity of air but instead the velocity plot in the cente showed air velocity just increased as the mesh was rotating not the solid.

When you say frozen rotor should be ok, are you saying that I can select all 132 faces of both domains and create just one interface if using frozen rotor method?

Lastly I'm not currently worried about measuring conduction if thats what you mean by 'heat transfer in the rotor'. In this instance are you suggesting suppressing the disc and setting the walls as a no slip boundary if so I'm unaware how to get that to rotate.

Really appreciate the help,
Thank you

[ghorrocks]

I assume you are saying that I should set the disc to a temperature and the air inlet at 50ms-1 and ensure that the model is mesh dependant before moving to a rotating domain.

Yes, I recommend preliminary verification and validation be done on a simple case. It makes the V&V much easier and quicker.

When you say 'a domain which entirely encompasses the rotor' do you mean I should boolean subtract the disc and create a two domains like that (i.e. a air domain with the disc perfectly sutracted. Or do you mean create a perfectly cylindrical domain slightly larger than the overall disc as i've seen in propeller tutorials on youtube.

Making the cylindrical domain slightly larger than the rotor.

I tried this technique with a simplified solid disc and found that air in the very centre of the disc would have an un-natural angular velocity. I expected to see rotation being effected by the rotating disc due to the no slip condition on the disc and the viscosity of air but instead the velocity plot in the cente showed air velocity just increased as the mesh was rotating not the solid.

Which technique did you try? Please show some images of your results as I don't understand what you are saying.

When you say frozen rotor should be ok, are you saying that I can select all 132 faces of both domains and create just one interface if using frozen rotor method?

No, this is not how interfaces work. Have you done the CFX tutorial examples using interfaces? You just apply the GGI, and the frame change model which goes with it, to the cylindrical domain encompassing the rotor.

Lastly I'm not currently worried about measuring conduction if thats what you mean by 'heat transfer in the rotor'. In this instance are you suggesting suppressing the disc and setting the walls as a no slip boundary if so I'm unaware how to get that to rotate.

This comment suggests you have misunderstood the basic methodology of doing simulations like this. Please make sure you do the tutorial examples on rotating machinery so you know how to do it.

Specifically - you do not model the rotor as a solid. This is a very common misunderstanding. The rotor should be a region cut out of the fluid domain, defined by wall boundaries. Please have a look at the tutorial examples about how this works.

[csaban]

Thanks again Ghorrocks, this information is very helpful.

Also would like to adress that I asuumed when people said the tutorials they meant the ansys official CFX help videos on youtube and have only just seen the tutorials.

I have set up a poorly meshed example to demonstrate what I mean. I have created a rotating domain encompassing the rotor and removed it as you said creating a void. And set it rotating at 3600rpm.

The stationary domain is air as well with an inlet of 50ms-1, as you can see from the image, there is a clear perfect circle where the velocity changes between the two domains which is of course unrealistic.


After doing some research it appears this is due to the fact that I am veiwing the velocity and not velocity in a stationary domain. However I am unsure why this should differ, I will leave the original text in case others are as stupid as me!

Additioanlly if I now wish to add brake pads to this model how can I keep them from rotating as they would lie in the rotating domain

Lastly, how can I set the temperature of the disc if it isn't a solid domain ?

Thank you

[ghorrocks]

Yes, the jump you are seeing at velocity is due to the rotating frame of reference. There is a brief FAQ on this: https://www.cfd-online.com/Wiki/Ansy...f_reference.3F

If you want to add non-rotating components like the calipers and pads then you need to start thinking about how to model it. The simple approach of an isolated rotor won't work. You probably want to move the interface to the rotor surface, so the GGI is now a solid-fluid interface for most of the area, but there will be some regions of fluid-fluid interface at the rotor channels. This type of modelling is a bit trickier as you need to make sure the non-overlap portions are handled correctly.

If you want the temperature of the disc you will need to model it as a solid. Again, this means there are some more interfaces and issues to consider. But recent versions of CFX should have all the necessary physics for this.

[csaban]

Thanks again ghorrocks,

I understand you are saying to create a circular domain perfectly around the disc will allow me to add pads and a caliper

However if i want to model heat transfer shoukd I not set the disc as a solid. In this case I assume it isn't necessary to place a domain around the disc but instead to suppress the disc from a cube domain to create an air domian, have a seperate mesh for the disc and then link them together in a CFX solver.

If this is what you suggest, when it comes to interfaces as my disc has 132 faces, is it necessary to create 132 solid fluid interfaces.

Thank You

[ghorrocks]

If you want to model heat transfer in the rotor then you will need to model the rotor as a solid.

For your 132 faces, you will need to group them into a single GGI. A face cannot be in multiple GGIs.

[csaban]

Thanks again Ghorrocks,

I have decided to ignore brake pads, and simply focus solely on the rotor.

My end objective is now to set the disc faces at initial temperature of 1000K and set a transient study for example of 20s in length. I would then like to compare temperatures at different points around the disc after this amount of time.

Then I would like to re-run the study with an additional inlet at the internal veins of the disc and compare the temperatures.

It is my understanding that to acheive this I require 3 domains, one rotating solid domain (disc), one rotating air domain (rotating fluid) and one stationary domain with an inlet and outlet (stationary).

I have now set 3 workbench CFX tabs (see image 1)

I have set the disc domain as a solid and set it rotating at the same angular velocity as the rotating air domain (see image 2)
I have set the disc initial temperature at 1000K (see image 3)

The only other change from the model without heat exchnage is I've tried to add an interface 4 as a fluid solid interface, where I have selected all 132 faces on bothe domains (see image 4). It is my understanding that I need this interface to view the heat transfer through the fluid domain.

However as i run the model it comes with the following error:

The orthographic view transformation fa- |
| iled on domain interface "Domain Interface 4". Failure may be du- |
| e to r=0 included in transformed cylindrical coordinates of an in- |
| terface with rotational relative motion. Another reason could be |
| that the interface contains faces that are parallel and others t- |
| hat are perpendicular to the rotation axis. |
+-------------------------------------------------

The message suggests that it is as simple as creating two solid fluid interfaces one with parrallel faces and a second with perpendicular faces
however as ive learnt to expect with CFD its never as simple as it seems.

It is worth noting this is set up as a steady state at the moment, just trying to see the change in steady state conditions first.

In the image it shows I have set the whole rotor at an initial temp of 1000k, I assume I would make a boundary on the rotor brake surfaces and set them to 1000k in order to see convection through the disc as well.

I really appreciate the advice so far it has been very helpful, hopefully for others too.

Thank You

[ghorrocks]

Yes, this sounds like 3 domains.

I see you are doing this in workbench - you can see how workbench is very clunky when you try to do more complex tasks like this. That is why most experienced CFX people use CFX stand-alone, not in workbench.

Having said that, I do not see why you need to split the meshing up into 3 workbench tasks. It should be able to be done in one.

Also, screen dumps from CFX-Pre are not very useful either. The CCL file it generates or the output file is much more useful.

We are not going to be able to help you much with that error message as it refers to specific mesh locators in your simulation. So you are going to have to look at your mesh carefully and see if you can work out the problem.