Thermal analysis brake disc section

[awaeryum]

Good afternoon,

I am new to Abaqus, and I am trying to perform a thermal analysis on a section of a ventilated brake disc.

So far, I have followed some tutorials on youtube about generic thermal analysis, so I've defined some properties of the model such as material, section, instances, loads, interactions, steps, mesh, BC.

The principle behind my simulation is: I apply a load (a surface heat flux) on both the surfaces of the disc where the pad would act, for 720 seconds and I plot the increase of temperature against time. The heat flux has been calculated previously, so I just use that value.
After that, I apply two interactions, one is the convection where I define the film coefficient and the ambient temperature and the surfaces where it acts, and the other is the surface radiation where I define the emissivity, ambient temperature and the surfaces.
My boundary conditions are set to don't allow the section to move where it has been cut and don't translate vertically and horizontally.
When I run the simulation and check the results, I obtain that on the surfaces where I applied the heat flux the temperature is only 25.46 degrees Celsius (I expect it to reach approximately 400 after 720 seconds with the flux chosen), while inside the vane is 25 (which is the ambient air temperature that I set previously).

Obviously, as I am new to this, I am sure that I am making a lot of mistakes. Could someone please help me?

Thanks in advance.

 

[FEA way]

Make sure that your units are correct. It's easy to make a mistake in unitless system such as Abaqus, especially in case of thermal analysis where properties are not that obvious. Another thing to do is to make sure that boundary conditions are defined properly (including amplitudes). Also check the step settings - incrementation, max allowable temperature change per increment and so on.

Which type of analysis is that actually ? From what you say it seems that you only solve for temperatures (heat transfer step) but then you mention BCs typical for general static analysis. Or maybe it's coupled temp-displ ?

Can you show a picture of your mesh, BCs and results ?

 

[awaeryum]

Thank you very much for your answer.

I have checked the units several times, cause I too thought that I made some mistake there, but everything seems to be correct.

I am performing a thermal analysis, I just used static BCs as I thought they were necessary due to the deformation of the part caused by the increase in temperature. Obviously I just assumed this, as I said I am new to FE analysis.

These are the screenshots:
Load
Convection
Radiation
Step
Mesh
Results

 

[FEA way]

You can suppress these structural BCs. They won't work anyway (unless you perform thermal stress analysis). When it comes to thermal boundary conditions, I suggest applying convection and radiation only on the surfaces where there's no prescribed heat flux BC (currently all your BCs share the same surfaces). But don't forget about the cyclic symmetry of your model.

 

[awaeryum]

Thanks for the reply.

I have tried to apply the convection and radiation only on the surfaces where the heat flux is not applied and remove the structural BCs. However, the results are almost the same, just the highest temperature now is around 30 degrees Celsius.
Do you have some suggestions? Am I setting the interactions and step correctly? I don't know how steps work, so far I've just created one steady-state step of 720 seconds of duration, and if I change its duration to 1 second or 3600 seconds, the results that I get are exactly the same.

 

[FEA way]

Did you chose steady-state or transient heat transfer step (it's in the first tab, not in the incrementation one you show) ? It should be transient of course. But if your BCs are not time dependent then don't expect significant changes in subsequent steps. It will only approach thermal equilibrium. Your incrementation shouldn't be a problem here.
When it comes to values, it's hard to say whether they are correct with these BCs or not since you don't apply temperature but heat fluxes. Check if the values of these BCs are correct for such analysis. How were they calculated ?

 

[awaeryum]

I thought too that it should be transient, but in every tutorial they use steady-state, so I opted for that. Also, when I change it to transient, the results are even worse.

I have tried to change the heat flux (the load) from total-flux to uniform distribution, and now on the surface I obtain a maximum temperature of around 900 degrees Celsius. In the pillars inside the vane, however, the temperature rises just slightly, with their centre remaining at 25 degrees.

How do I impose my heat flux at the beginning of the simulation with the disc at ambient temperature, leave it to act on the surfaces for a certain amount of seconds, and then plot the results of how the temperature varies through the section?

 

[FEA way]

If you use stead-state then the number of seconds you've mentioned before (720) has no physical meaning and you could actually use 1 as a step time. Especially that you don't use amplitudes.

What you should understand is that when you perform stead-state simulation then Abaqus seeks for a thermal equilibrium when there's no more exchange of heat and temperatures balance out and become constant. If you perform transient analysis of a long enough perios of time then heat flow will decay and you will eventually reach stead-state too.

 

[awaeryum]

When I check the results, I notice that only the first layer of seeds of the mesh is affected by the heat flux acting on that surface, the other layers remain at the initial temperature and are not affected at all even if I modify the duration of the simulation. If I change the size of the seeds, the behaviour is the same.

What did I do wrong?

 

[FEA way]

Can you attach an input (.inp) file used in this analysis ? It will be much easier to help when being able to take a look at the model.

It seems that conductivity of the material is too low or the heat flux too weak and heat can’t reach deeper parts of your model. Plot heat flux (HFL) contour plot and see if it gives you a clue.

 

[awaeryum]

Thank you for your help, I have attached the input file.

 

[FEA way]

It seems that your material properties (and probably also BCs) are in SI units but the geometry was made in SI(mm) units. That’s a common cause of errors when heat is not reaching deep enough.