CFD Online Logo CFD Online URL
Home > Forums > Software User Forums > ANSYS > FLUENT

Transient problem w/ initial values

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

LinkBack Thread Tools Search this Thread Display Modes
Old   July 30, 2002, 13:04
Default Transient problem w/ initial values
Posts: n/a
Hi guys,

Ok, my supervisors are getting demanding...

They want me to do a transient simulation to find out how long it takes for the cold air(temp=288K) at the inlets in my model of a room to cool the room down from 303k to about 296k.

So the initial room temperature, just before the cold air enters, will be 303k. Is it at the Solve/Initialize/Initialize, and do a compute from "all-zones" where i can keyed in the initial room temp to be 303k?

if i do a compute from "inlet" FLUENT will compute and update the Initial Values based on the conditions I specify at the inlet which has an initial temp velue of 288k. so i can only change the initial values by doing "compute from all-zones"

Am I right?
  Reply With Quote

Old   July 31, 2002, 01:53
Default Re: Transient problem w/ initial values
Posts: n/a
Run steady state simulation to get the final temperature i.e. 296K. Now apply the initial condition as you are doing for the problem. The transient problems take long time and the time step should be choosen properly otherwise convergence gets affected.

Run for approx time you think should be okay for getting steady state results.

Bye Ashu

  Reply With Quote

Old   July 31, 2002, 01:54
Default Re: Transient problem w/ initial values
Posts: n/a
If you want to initialize a variable (temperature) to a specific value, enter it in the Init panel field. Don't worry about "compute from all-zones", etc. It is just an aid if you can't decide what to specify as an IC.

Initialize the domain to the hot temp value.
  Reply With Quote

Old   July 31, 2002, 03:03
Default Re: Transient problem w/ initial values
Posts: n/a
My suggestion: (a combination of Ashu's and Lanre's)

-initialise with the hot temperature of 303K -run steady state untill convergence to obtain the flow pattern. Your air-inlet should be 303K now. -set up a monitor to plot the average room temperature -monitor also the outlet-temperature. If your outlet temperature becomes 288K and the average room-temperature is still higher, you've probably dead zones in which the air poorly refreshed. -If you think natural convection is an issue, use the bousinesq model. -Switch the solver to transient -change the inlet-temperature from 303 to 288. -turn of all the convergence checks -save -run, test a few times to find good settings for the time-step.

good luck,

Laika, still orbiting
  Reply With Quote

Old   July 31, 2002, 04:35
Default Re: Transient problem w/ initial values
Posts: n/a
One more thing the room might have sensor ( monitor in case of Fluent)that shows temperature what you want but somewhere there can be hot spots as Laika pointed out.

  Reply With Quote

Old   July 31, 2002, 08:10
Default Re: Transient problem w/ initial values
Posts: n/a
Hi all,

So is that the procedure to run transient simulations? First to run it under steady state until convergence, then switch it to unsteady time mode and run it using time steps?

So to repeat what I have understood:

I init it at initial value of 303K and compute from one of the inlets. Then when I reach convergence, I should get the temperature distribution and air flow in the room. The average temperature in the room should be lower or equal to the temperature at the oulet to demonstrate effective cooling. If not, something must be wrong.

AFter the steady state simulation, I run it under transient mode using appropiate time steps.

But what I dont understand is, 1)Laika, you were saying that my oulet temperature should be 288K, but since I want the average temperature to be 296K (due to some heat flux at a window which represents heat from the sun coming into the room), then my oulet temperature will be slightly higher or equal to 296K since the average room temperature should be around 296K to demonstrate effective cooling.

2)Also, when I run the simulation at transient state, why is it that I change the initial value of inlet temperature from 303K to 288K? Because I will still be modelling cooling down of the room from its initial temp of 303k?

3)Also, when I run the transient simulation, I click off the convergence check, is this because I haf alreday checked for convergence under steady condition, and I do not need to check for converegence again when I run the transient?

4)When I use an monitor for the average temp in the room and at the inlets and outlet, do I plot w.r.t iterations as the x asis?

Thanks again. Sorry if I did not fully understand your answers.

  Reply With Quote

Old   July 31, 2002, 09:57
Default Re: Transient problem w/ initial values
Posts: n/a
**Initialise the entire room with your starting temperature and from 'all zones', not from one of the inlets.

**modelling sun-irradiation with a heat flux through a wall that's stands for a window is not a good approach. You should model it with the discrete ordinates radiation model, and set the window-'wall' to be a semi-transparent wall.

**OK, if you have a heat source, you can waith for ages untill the outlet-temperature = inlet temperature. Just follow the temperature at the outlet and in the room. If your outlet temperature is lower than the average temperature of the room, this can only mean there is fresh air going directly from inlet to the outlet. You'll probably find some dead-zones and some air trapped in recirculation-zones.

**Yes, if you run a steady state with inlet at 303K, you will still have 303K in your room at the beginning of your transient calculation. You must decide yourself if this is a good approach. Maybe this is not completely what you want to model. Maybe you just want to start your transient calculation with all the air at rest. Then forget about the stationary solution and start from the very beginning with a transient simulation.

**unselect the convergence check because it might cause divergence in the next steps. You should let Fluent do in each time-step the maximum number of iterations. Make sure you don't need more than 25 iterations per time-step to have a big drop in residuals. If you don't reach 'convergence' in your time-step within 25 iterations, reduce the time-step.

**No, it's better to plot the time at the x-axis. Write it also to a file. The result will be the average room-temperature versus time plot. This is exactly what you need, isn't it?

greetings, Laika, still orbiting
  Reply With Quote

Old   July 31, 2002, 11:01
Default Re: Transient problem w/ initial values
Posts: n/a

u are very precise and i understood everything!Thanks!
  Reply With Quote

Old   June 6, 2014, 07:22
Default Transient analysis
New Member
Rui Carneiro
Join Date: Mar 2014
Posts: 9
Rep Power: 12
sinvastil is on a distinguished road
Hi everyone,

I am doing a similar study, the difference is that i have one door between the interior and the exterior of room.
In my case the temperatura inside the room is about 278,15K and outside the room is 298,15K.
I want to study the temperature change inside the room, as the door opens, due to the natural convection.
For the exterior i choosed the boundary conditions as Pressure Outlet and to the room were adiabatic walls.
But until now i can't obtain results, can somebody help me?
sinvastil is offline   Reply With Quote


Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

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 Off
Trackbacks are Off
Pingbacks are On
Refbacks are On

Similar Threads
Thread Thread Starter Forum Replies Last Post
transsonic nozzle with rhoSimpleFoam Unseen OpenFOAM Running, Solving & CFD 8 July 1, 2022 06:54
Forces in OF15 richard OpenFOAM Running, Solving & CFD 180 July 9, 2018 10:54
Moving mesh Niklas Wikstrom (Wikstrom) OpenFOAM Running, Solving & CFD 122 June 15, 2014 06:20
Full pipe 3D using icoFoam cyberbrain OpenFOAM 4 March 16, 2011 09:20
ForcesCoeffs ronaldo OpenFOAM 4 September 14, 2009 07:11

All times are GMT -4. The time now is 04:29.