Conjugate heat transfer of ventilated disc brake
 

Dear Sir/Ma'am
My project aim is to find conjugate heat transfer coefficient of brake disc while rotating at a particular speed in atmospheric air and decelerating from 27.7 m/s to 0 m/s in 4 sec. Heat flux on the disc through pads is 14968558.86W/m2.Could you please answer the following questions as I am not able to solve this problem?
1. Should I take complete disc or a sector of disc for analysis? What difference would it make?
2. What type of enclosure should I make around the disc? What portions to provide as Inlet, Outlet, Opening, Symmetry and Wallto get accurate results?
3. How many domains and interfaces to create in cfx-pre ( I have used three domains and two interfaces- stationary / fluid domain, (box) rotating/fluid domain (cylinder) and a rotating/solid domain (disc)) and what boundary conditions to have to have best possible results?
4. Do I need to subtract the disc from rotating cylinder domain using boolean operation in design modeler? Why so?
5. Any particular specifications for mesh which could make difference in results or a generalized default mesh could be used?
6. I am unable to find Heat transfer coefficient as my output in cfx-post? How to calculate it as an output?
I have used these conditions -

Fluid Stationary domain(box) -
Inlet (one side) - velocity and atm. temp.
Outlet (one side) - relative pressure
opening (four sides)- relative pressure and atm. Temp.

Fluid Rotating domain(cyl.) -
Angular velocity same as that of brake disc

Solid Rotating domain(disc) -
Heat flux - pad area on both sides of disc

Interfaces -

Fluid Stationary -Fluid Rotating
Fluid Rotating - Solid Rotating


I know these are a lot of questions. Sorry for that. But anyone with the answer of this problem can explain it one by one.
Thank you so much for your upcoming valuable guidance.

Regards
Sharang Kaul

First of all, please do not PM copies of posts on the forum. I do not respond to CFD questions by PM.

I cannot answer your questions as I do not know what you are trying to do. What is the conjugate heat transfer coefficient? Most people want to know the temperatures in the rotor in situations like this, not the HTC.

I am so sorry for PM you. I had not gone through the forum rules before. None the less, you are right. Even if i am trying to find the temperature of disc. Could you please elaborate that how can I run this problem in ansys cfx? I have mentioned all my data.

1. what sector to use depends on three things: your geometry , if you can neglect the ongoing speed, location of the brake disc (is the brake disc in the wheel rim?)
If you can neglect the ongoing speed and you think that this will not efect your results? than you can use the smalest posible sector that geometry lets you in your case It is posible to use a wery small sector as geometry just radialy repeats itselve and is relatively simple.

2. Enclosure depends partialy on your geometry again if you want to include the rim that is also posible

3. If you will neglect the ongoing speed of the vehcicle than you can use 1 rotationg domain in CFX. If not than you will need at least 2 (rotating fluid and stationary fluid).
And if you will do a CHT simulation you will need 2 (one fluid one solid) domains with ongoing speed neglected and 3 domains if included (fluid stationary, fluid rotating, solid rotatiing).

4. Yes you need to substract the geometry from the air domain. if you want to include brake disc in the simulation than this will be a CHT (conjugate heat transfer simulation) and you would need both the air surounding the disc domain and the disc solid domain itselve.

5. Definitly use wery thin inflation layers and SST model is recomended, for proper wall heat transfer treatment, with y+<1, you can see y+ values later in post these will depend on mesh layer thicknes and velocity of air near the wall so roughly (your angular velocity* radious of the brake discs surface+(some other contributions)).
If you are new to the cfd do not complicate your simulation too much as things can get messy.
Just try a simple mesh at first but than vhen the simulation is already in working condition go back to mesh and definitly improove it a lot the solver will still run on bad mesh so focus on the CFXpre if you are new to cfd.

6. You will have to set the expert parameter for T-bulk temperature to constant ambient air temperature. You will than be able to see tha HTC contour in cfx post

____________
You will have to read some theory behind this simulation: I recomend that you find some papers on this topic there are some that will guide you threw the whole brake disc simulation.

If you need only the HTC:
I recomend that you start with a simulation that does not include the brake disk, keep it simple at first: just one rotating air domain with constant brake disc wall temperature let say 100°. I have found out that average HTC will not change much with temperature, 2% max in some of my cases for a temperature range of +-200°C so that can be neglected.

That is why you can simplyfy things at the begining as CHT simulation will take some additional interfaces and knowledge about heat sources...