[fabioacfoz]

Hello all

Im modeling an office environment with inlet air from the air conditioner at 17 and an return plenum duct. In this, people ate cilinders with the medium adult human area (1,8 m²), computers with heat flux and temperature walls taken from Energyplus simulations. But my simulation is diverging, i think because of my inlet-outlet boundary conditions and my timestep. I have three questions:

1) A coarse mesh can make my simulation diverge?

2) What should be the inlet-oulet conditions for the model? (I already tryed massflow-massflow, velocity-velocity, volocity-pressure)

3) What could be the bigger timestep that should not make the simulation diverge?

(What always happen is the overflow error, due to mommentum and mass errors in the linear solver)

Thanks 4 who´ll help!

[ghorrocks]

This might help:
http://www.cfd-online.com/Wiki/Ansys...gence_criteria

[fabioacfoz]

Aparently, the problem is that the momentum and mass equations (U-mom, V-mom, W-mom and P-mom) are diverging. The error is: Point Exceptionverflow.

I read about this error in the forum but nothing really changed. The problem seems to be in the conditions at the inlet - outlet. I forgot to mention, is a transient simulation.

The ideal boundary condition for me would be equal mass flows in the inlet and the outlet, but it gives errors. If i put my outlet flow rate lower than inlet it helps, but after several timesteps it crashes too. Isnt something i dont know about setting the inlet-outlet boundary conditions that i could be doing wrong??

[kingjewel1]

Originally Posted by fabioacfoz

Hello all

Im modeling an office environment with inlet air from the air conditioner at 17 and an return plenum duct. In this, people ate cilinders with the medium adult human area (1,8 m²), computers with heat flux and temperature walls taken from Energyplus simulations. But my simulation is diverging, i think because of my inlet-outlet boundary conditions and my timestep. I have three questions:

1) A coarse mesh can make my simulation diverge?

2) What should be the inlet-oulet conditions for the model? (I already tryed massflow-massflow, velocity-velocity, volocity-pressure)

3) What could be the bigger timestep that should not make the simulation diverge?

(What always happen is the overflow error, due to mommentum and mass errors in the linear solver)

Thanks 4 who´ll help!

1) what is your cell size? and type? Nielsen et al has a formula specifically for the size of HVAC meshes. Roache et al developed the GCI (grid convergence index) to quantify your quality. I'd say from experience that coarse meshes in HVAC won't give divergence, quite te contrary.

2)Do you have an ACH rate? If so flow rate or velocity bconds can work. (outlet might give problems sometimes)

3)Start with adaptive. what is the turnaround time (circulation time) of your air?

4)I think your problems arise from boundary conds (from the looks of it). Look at the ACH rates and your pressure outlets, do they match up. have you got loss? etc

Give more details and we'll try and sort you out!
Best wishes.

[fabioacfoz]

Kingjewel1

My mesh is only tetraedrals, with maximum lenght of 0,5m. The regios of the inlets, outlet, people and computers are refined, with 0,1 maximum face spacing and 0,01 minimum spacing. My environment is an open office , in my simulation a box about 18,45m x 9,4m x 2,7m, with constant flow of air entering by the side of the lights displacements.

The region that represent the inlets are 184 rectangles with 0.1 x 1.2m. The outlet is through the lights, going to the plenum and entering the return duct. The inlet mass flow rate is 1,9 m³/s, obviously the outlet too. I dont think that my mesh is too refined, but not so coarse either.

I´m running with 1 second timestep, and it seems to be running. 5 second make the simulation crash. I think the problem is the timestep, but this comes another problem. 1 second timestep running the system for at least one hour to see the AC cycles is too time consupting, and i need the results for this monday . My objective is to do a simulation of a VAV system to show how the temperature gradient in the zones would fall. I have sucessifully done this in Energyplus, but my boss want me to do in CFD too .

[kingjewel1]

Originally Posted by fabioacfoz

Kingjewel1

My mesh is only tetraedrals, with maximum lenght of 0,5m. The regios of the inlets, outlet, people and computers are refined, with 0,1 maximum face spacing and 0,01 minimum spacing. My environment is an open office , in my simulation a box about 18,45m x 9,4m x 2,7m, with constant flow of air entering by the side of the lights displacements.

The region that represent the inlets are 184 rectangles with 0.1 x 1.2m. The outlet is through the lights, going to the plenum and entering the return duct. The inlet mass flow rate is 1,9 m³/s, obviously the outlet too. I dont think that my mesh is too refined, but not so coarse either.

I´m running with 1 second timestep, and it seems to be running. 5 second make the simulation crash. I think the problem is the timestep, but this comes another problem. 1 second timestep running the system for at least one hour to see the AC cycles is too time consupting, and i need the results for this monday . My objective is to do a simulation of a VAV system to show how the temperature gradient in the zones would fall. I have sucessifully done this in Energyplus, but my boss want me to do in CFD too .

Your mesh I think is ok? Nielsen et al. (Rehva) recommends a rule of thumb formula as : N=44E3*(vol)^0.38 for the approx number of cells to achieve mesh independent results. so in this case you'd need about 500K.

Why have you decided on 5 second timestep? your ACH seems to be 14.6 and so your air residence time is about 4 minutes. (ACH=3600*flowrate/vol=1/tau)

Running steady state and looking at the time on the streamlines will help you with the timescale: look at the longest residence time.

[fabioacfoz]

If it would work, my timestep would be 1 minute, but the overflow error always happen. The only timestep for that it does not apear is 1s. With 1 second, the simulation runs ok, with good results, but loooong computional time, and inviable. What you talked about 500k elements, i will try to do a coarser mesh then, bcause mine has 3600K cells.

Thanks for now! Maybe later more problems will ocurr hehe

[fabioacfoz]

Kingjewel

With a coarser mesh the simulation went fine, my 1 minute timestep was good enought to see the AC on/off status and the expected temperatres at the enrivonment.

But when the solver sucessifully finishes and the CFX-Post open, it doesnot open my result files. the error is this:

DataReader::loadData - Error reading file 'C:\CFX sim\MALHA_004.res':
Error reading number of domains (G/NZN).

I googled it, in the forum and nothing. Do you know why this is happening?? Thanks!