hi CFX users i am doing transient analysis of brake drum initially at 600 deg. i tried to do it defining brake drum as rotating wall but it is not working. any one can suggest me how to proceed.

Hi,

Step 1 is to properly describe what you are trying to do. You will need to describe what you are trying to model and the problems you are currently having for us to have any chance to help you.

Glenn Horrocks

Hi Glenn I am doing transient heat analysis of rear wheel brake drum. I have modeled a complete jeep outer frame. In the rear wheel I have modeled a tyre, wheel rim with elliptical vent holes and a brake drum. Now when the vehicle moves there will be turbulent flow of air over the brake drum through vent holes. On application of brakes the brake drum gets hot. Experimental setup gives the maximum temperature of 600 K. I have to find out the temperature after 10 sec, 20 sec, 30 sec after the application of brake. The flow of air over the brake drum is the only cooling medium to be considered. So there is flow analysis part over which heat transfer part is dependent. I have already tried giving rotating wall option to brake drum, rubber tyre, and steel wheel rim. This only gives the flow part but not heat transfer part. I even tried giving volumetric heat source to brake drum making a separate sub domain for the brake drum and rotating wall to tyre and wheel rim. In this case the brake drum doesn't show cooling.

Hi,

What do you mean by "I have already tried giving rotating wall option to brake drum, rubber tyre, and steel wheel rim. This only gives the flow part but not heat transfer part."?

I would think modelling the drum as a solid domain would be the best method, connected to the air domain with a domain interface. Also I think you will find that at 600K radiation may well also have a significant contribution to the heat transfer.

Glenn Horrocks

Hi Glenn I am doing as you said. I have created a solid domain for brake drum and a subdomain named heater with value 10000 of heat source. Now how to see the results?. This is what I am doing in CFX 5.7 Post, "I double click the brake drum from the list of names. Then I change color to variable > temperature". This shows a constant 600 k for the complete brake drum. No temperature difference is shown on the surface of the brake drum. Is there any different procedure to be adopted for viewing results in CFX 5.7 Post.?

Regards, wilson

Hi,

Check: 1) you have the interface between the solid and fluid domains correctly defined 2) your heat equation in the solid is properly converged, the heat equation in the solid often converges far slower than the fluid section unless you accelerate it 3) Check your model is properly converged.

Glenn Horrocks

hi domain interface seems good as such it comes by default since i have only one solid domain. initially i am giving steady state flow analysis with solve energy option put of from expert parameter keeping only the solve fluids and solve turbulence option true. Then in the next stage i give transient analysis with heat source and keeping only the solve energy option true. my initial file is the earlier steady state flow RES file. now by doing this i get good convergence but cannot say which one is faster fluids or energy because i am solving both seperately. should i use decreasing heat source by defining a step function expression?

regards wilson

Hi,

Why are you solving them seperately? They are coupled and should be solved together. Also, as for your domain interface - are you getting a heat flow across it?

Glenn Horrocks

Hi If I give flow and heat equations together the temperature of brake drum remains at 600 K. if I separate them then I get some temperature drop over the surface of brake drum. besides this solver takes less time to solve. Can u suggest me a method to calculate the heat transfer coefficient over the brake drum. Is this one correct "volumeAve(htc)@subdomain". Here I have given volumetric heat source named heater as subdomain.

Regards wilson

Hi,

You do not choose a solution technique because the solver takes less time to solve. You might as well forget CFX and use Paintshop to draw what you want to answers to be. There is a problem in your simulation with getting the heat and fluid flow equations when solved together to converge properly and that should be fixed, rather than trying to generate an artificial simulation which may or may not have the relevant physics.

CHT problems are harder to converge that purely fluid flow simulations. Some recommendations: 1) I highly recommend activating "Conservation target" as part of your convergence criteria. Convergence in CHT problems is more often determined by the heat balance across the interface rather than the residuals. 2) Also under the convergence tab there is a "Solid Timescale Factor" setting. This accelerates the converge in the solid domain as the timescales associated with the solid domain are often far slower than the timescales in the fluid domain. This allows the solver to better match these different timescales. The best value to use is problem dependant, but if you are simulating a brake drum which is a fairly large lump of metal a value of about 1000 should be OK. The heat transfer equation in the solid is a linear equation so it is not as sensitive to divergence with large timesteps as the non-linear fluid equations.

Hope this helps.

Glenn Horrocks

hi thanks glenn its working. regards wilson