CHT_ Application
 

Hi all,
Application: Drill tool application. tool with an internal cooling channel.
Time when I start the Simulation: After the holes are drilled and the tool is at a certain high temp. (more than 600K).
My objective: to see the temperature Profile Variation with time on the drill tool surface. The surface seen below is after 10s.
Attachment 49576.

Modeling strategy for the above results:
4 paths of heat loss considered:
1. Conduction into solid.
2. covection through the cooling channel.
3. convection to the outer Domain.
4. Radiation losses. which are Hand calculated analytical formulae developed and inserted as CEL condition.

conditions implemented:
1. Steady state Simulation with fixed temp. at this edge for 100 iterations.
2. Using this file as intial BC for my transient Simulation. applying BC on the surface for HTC (negative HTC applied for heat loss. I tried with positive also.)so that it loses heat to the surroudings.
3. convection at the Interface is modeled using Domain Interface condition where the heat Transfer condition in enabled.

I do not see reasons why the surface does not lose heat so fast. in 10s there is barely a Change of 2K. !


(Checks I did: I am using time steps small enough to satisfy Courant condition and the yplus value at the Interface is less than 11, GGI Domain Interface mesh Connection.)

This is a steady state simulation, so statements like "in 10s there is a change of 2K" is meaningless. Time does not come into steady state simulations.

If you are not getting the temperature you expect:
1) FAQ: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F
2) In particular check that your heat transfer boundaries are correct.

My objective is to see the temp. profile variation with time, not just when the solution is converged. Temp. is time dependent.
I performed a steady state solution and got results. The transient solution shows great convergence for mass and momemtum equations but for the control points which I am interested shows absoultely no convergence. (for transeint case. )

You can't get a temperature profile from a steady state run, even if it uses time. You need to do a transient simulation to get time histories.

What do you mean the transient case did not converge at your control points? What are your control points? How are you defining convergence?

Yes. I am using a transient simulation. My monitor points are the points where I expect the temperature to converge with time. But there is absolutely no change in the temp. profile at these monitor points.
I should be using a turbulant model, but currently I am using a laminar model.
Incompressible, viscous, thermal energy model.

Do you need to run it for longer time as the thermal change has not had time to propagate?

Hi,
Thanks for your replies. I do not know what I would have done without your replies and guidance. I will be mentioning your name in my thesis acknowledgements.
Part 1:
I am running for 10s with 1e-4 time steps. The temp. does not converge with time.
Part 2:
Well, I defined a source point in the solid which shows gives me convergence. But does this make sense? Adding a source point to the solid so see temp. profile?

I am glad to have helped.

Does it simply need more than 10s? Run it for a lot longer to check this.

Is 1e-4s time steps small enough? Do a time step sensitivity check to find out.

I assume you mean a monitor point. Yes, if the final temperature of the block is important than this sounds like a sensible approach.

So I can understand what you are doing, can you:
* Post an image of the entire simulation
* Post an image of the time history you are talking about
* Post your CCL or output file.

1.small time steps reasons:
I have a very fine mesh and thus to Satisf courant number I use small time steps.
2. I did 2 simulations:
1st simulation:
I use a simplified geomtry just to see the modeling parameter effects.
I have a cooling channel. and want to see the cooling of the face with the monitor points as below.
Attachment 49679
I run the simulation for steady state. Use output of this as initial condition for transient simulation and observe the temp. profile for these control points .
Attachment 49677.
No change at all.

2nd simulation:
I define a source point at the point where I expect high temp. This source term is added in the energy equation.
And then I see some temp. profile variation with time. I am still running the simulation. So I can post this photo after a while.
But does adding a source point to the solid make sense ?

Small time steps:

How do you know Courant number = 1 is sufficient for accuracy? You still need to do a sensitivity analysis on this to show it is OK. I know of simulations which require time steps far smaller than Courant number = 1, and others where time steps much larger than 1 are OK.


No change at all.

Are you sure? That graph has a very big scale. I would remove the velocity curve and zoom in on the temperature results to see how much variation you really are getting.


A source point adds or subtracts heat at that point. What heat source or sink do you have at that point?

@Courant number.
I decide this also based on the number of iterations it takes at the time steps. IF I take higher time steps, solution is not converged at the time steps(I give 10 iterations per time step). If I satisfy this Courant condition, then I get convergence in around 3-4 iterations.
@Monitor Points:
I get your Point. I checked the values from the solver file at the time steps. It changes really slowly. To be precise I exported the values and the time steps. the slope of the curve is -1.2 degrees. :P.
@source Points:
Since this is a Drilling application, heat is added into the cutting tool due to friction from a Point. But I am trying to simulate the process after Drilling has been completed. So I thought of giving a Point heat source.
I would ideally like to add heat at Initial time step and let the graph converge with time to steady state temp. which is 293K.

If the temperature change is a small and roughly constant rate of heat up then the heat input to the system is simply heating the system up. You can estimate how long it will take to get to temperature by m*Cp*dT.

When the drilling is completed, does not that mean all heat input stops, and all which happens is the temperature field in the system starts to even out and heat is lost to the surroundings? I can't see how a heat source is going to be helpful in reproducing that. I would suggest you run a simulation where you model the drilling process which will give you the thermal profile of the device, and then a second simulation where you turn the drilling heat source off.

Yes. Thanks for the suggestions. Would work on this. !
What would I have done with your help!:o