# FLUENT

 Register Blogs Members List Search Today's Posts Mark Forums Read

 January 1, 1999, 19:58 FLUENT #1 Adrian Guest   Posts: n/a I'm currently doing on a thermal effect on a sudden expansion flow. I'm having problem with the heat source input. I'm suppose to patch a heat source of 10kw/m3 into node 42 until 401 in the x-direction. And i had a flow from the inlet of Re=200 which is u(y)= 0.133024-332.56y2. It seems that the effect of heat source doesn't work. Is it that i'm lack of other input? And i did read about an article that it suppose to reduce my recirculation length but it seems doesn't work.How?

 January 4, 1999, 13:50 Re: FLUENT #2 John C. Chien Guest   Posts: n/a I don't think it will have any effect on the incompressible flow at all. For compressible flow or variable density flow, first check the temperature and density contour plots to determine whether you have compute the flow field properly.If the density does not change much, then you can increase the heat source to change the density difference. Maybe it is easier to specify the wall temperature. In this way the problem is simpler. At Re=200, I think the flow is still laminar.

 January 4, 1999, 14:29 Re: FLUENT #3 Adrian Guest   Posts: n/a Thanks for replying, John. You did said that it is easier to specify the wall temperature, I was given only the value of 10kW/m3 of heat source. So, what formula should i use to obtain the temperature at the wall? thanx.

 January 4, 1999, 15:27 Re: FLUENT #4 John C. Chien Guest   Posts: n/a Do it this way: (1) set the inlet temperature to room temperature, (2) set the wall temperature ( certain section ) to ( room temperature + 350 degree C. ) (3) compute the flow field, (4) check the temperature field field, (5) check the density flow field, (6) check the wall heat flux. At this point, you should have some idea about the wall temperature and the heat flux. (7) scale the temperature up or down to match the target heat flux ( the one given to you ). (8) with the new wall temperature, recompute the flow field, (9) go through steps 4,5,6 and compare the computed heat flux with the target heat flux. and so forth. 10KW/m3=100W/(10cm)3=one regular 100Watt light bulb/(10cm)3. This approach will tell you whether the heat transfer through the wall is affecting the density and the size of recirculation or not. Once this is established, you can add heat source in different ways. ( you may want to get help from someone with direct access to Fluent code to make sure that the input is properly set.)

 January 4, 1999, 15:33 Re: FLUENT #5 John C. Chien Guest   Posts: n/a Oh, the heat source is only a 10Watt light bulb/(10cm)3, not a lot!.

 January 4, 1999, 21:02 Re: FLUENT #6 Sung-Eun Kim Guest   Posts: n/a Dear client, Assuming that you are trying to model a mixed convection problem (natural and forced), I wonder if you specified the gravitational accereration and the density vs.temperature reationship (e.g. thermal expansion coefficient) properly.

 January 10, 1999, 04:21 Re: FLUENT #7 P.N.Madhavan Guest   Posts: n/a Dear Mr. Adrian: I want to make one item clear, that is patching of a variable will not affect the final solution for a given problem. Normally patching is done to increase the convergence rate of a given problem (steady state problems). Hence to find the thermal behaviour of ur problem, the heat source effect should come in form of a seperate boundary condition. After specifing the boundary condition its ideal to patch that zone and i expect the problem will work as one anticipates. All these will work only for a steady state problem. For a transient problem the patching will be considered as an initial condition. Any how i strongly feel u will get rid of this problem if u feed in the heat soruce information in form of a seperate boundary condition. madhavan

 January 10, 1999, 14:29 Re: FLUENT, Patching, Unique Solutions #8 Jonas Larsson Guest   Posts: n/a Getting a bit off the original topic here, but anyway, this is an interesting subject - Patching a variable (Fluent speak for explicitly setting a flow variable in a certain region to something known), or starting from a different initial flow field can, for some cases, affect the final converged stationary flow-field. There isn't always just one unique solution to the Navier-Stokes equations and you can have hysteresis effects. I'd imagine that these effects are more common in ventilation problems and such, where bouancy is important. Anyone have any good examples of these hysteresis effects? I remember one example from a PhD presentation that I attended a few years ago. It was a fully symmetric ventilation case with an air-jet that, depending on which field you started from, either turned left or right. It is not very common in the applications I usually work with (turbomachinery), although I guess you would have to think about this if you are dealing with complex separations and perhaps shock/boundary layer interactions. Anyone have any thoughts about when hysteresis effects are especially important?

 January 11, 1999, 03:58 Re: FLUENT, Patching, Unique Solutions #9 Robin Bornoff Guest   Posts: n/a It is more likely to happen with jets/plumes issued into open spaces that suffer the coanda effect as a result of interactions with the space walls. i.e. HVAC applications. We've found that incorporation of geometry that is initially considered irrelavant can lead to the diffusion of the jet and thus a 'settling' of the flow to single state. Geomtric simplification can often lead to unstable solutions!

 Thread Tools Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Volker Pawlik FLUENT 7 May 22, 2014 22:30 knight Fluent UDF and Scheme Programming 11 December 8, 2013 10:00 Steven Fluent UDF and Scheme Programming 4 September 20, 2013 16:30 renyun0511 OpenFOAM Running, Solving & CFD 8 July 6, 2010 06:24 Lourival FLUENT 3 January 16, 2008 17:48

All times are GMT -4. The time now is 15:49.