[LilBort]

Originally Posted by ghorrocks

Hi,

"The inlets and outlets have fixed velocities, and the room should pressurize." - this sounds like rubbish to me. The room will just keep increasing in pressure as time progresses. If you want to want to pressurize the room you need to specify the inlet and outlet flow curve and any leakage paths. Then the room will naturally find its pressure level between the inlet and outlet.

"I am considering turning radiation off all together" - work out the radiation heat fluxes. If they are insignificant compared to the convection and conduction fluxes then yes, turn them off.

"Once I get my model to run correctly I will increase the number of loops" - this is not a good way of quickly getting a starting point. You need the timesteps to come close to converging or you can get very misleading results. Use a max coeff loops of 10 or more right from the start.

"I increased the memory allocation because I was getting overflow errors" - then fix the overflow errors. This shows there is something seriously wrong with your model and you only been lucky that increasing memory allocation allowed it to continue. I doubt the results are sensible, you could get anything.

Glenn Horrocks

Glenn Horrocks

I have given your comments consideration, and I have chosen to set my return outlets with 0 Pa relative pressure to keep the room from constantly increasing in pressure.

[LilBort]

Originally Posted by Simulation Engineer

Hi - a couple of thoughts and maybe you already have these:

Did you set up Domain Interfaces of solid - fluid type between all the solid cylinders and air in the room?

did you use buoyancy and set gravity vector direction and ref density for fluid?

did you use Air Ideal gas model for air if it is natural convection?

- How do you set domain interfaces between solid and fluid domains?

I have since redesigned the mesh to include the humans and room all into one domain. I will not have a humans domain, just cylindrical indents in the floor of the room. And I will set a heat flux on the cylinder surfaces. But it would be nice to be able to add additional domains after the fact, so that I do not need to redesign the mesh every time I need at add people or equipment to the room.

- Yes, yes and yes. Displacement ventilation relies on the physics of buoyancy to stratify the room air into a temperature gradient. Cold air comes in near the floor and when it hits a heat source the hot air rises to the ceiling moving contaminants with it. This is why there is a noticeable temperature gradient from ceiling to floor.

- Yes I am using Air Ideal Gas

[ghorrocks]

Hi

You don't need to remesh. In CFX-Pre just delete the solid domains. You just won't use that bit of the mesh.

Glenn Horrocks

[LilBort]

Originally Posted by ghorrocks

Hi

You don't need to remesh. In CFX-Pre just delete the solid domains. You just won't use that bit of the mesh.

Glenn Horrocks

When I do this, I get the Isolated Fluid Regions Error.

[ghorrocks]

Hi,

The isolated fluid regions warning is saying you have two or more domains which are not connected in anyway. This means that you have not properly deleted the solid region. You can delete it either at the mesh level (on the top of the tree in CFX-Pre) or at the domain level by not specifying any domain to use the solid region, then deleting the default domain which is generated to use the solid domain.

Also - Don't use air ideal gas for buoyancy unless you have large temperature/pressure variations. Use an incompressible flow with the thermal buoyancy coefficient set instead.

Glenn Horrocks

[pulgarcito]

Hi to all,

I dont understand your interesting in simulate solid regions. Just simulate only fluid domain and represent human bodies as a wall using heat flux (total or convective deppending if you plan to simulate radiation or not). In my experience, displacement ventilation simulation works great with boussinesq aproximation for buoyancy. You will encounter more numerical stability using boussinesq rather than real gas state equation.

perhapls helps you to run calculations in transient mode, reducing g value to add an extra "relaxation" for momentum equations. Then increase g value untill the desired conditions.

Sorry for my english

Regards

Originally Posted by ghorrocks

Hi,

The isolated fluid regions warning is saying you have two or more domains which are not connected in anyway. This means that you have not properly deleted the solid region. You can delete it either at the mesh level (on the top of the tree in CFX-Pre) or at the domain level by not specifying any domain to use the solid region, then deleting the default domain which is generated to use the solid domain.

Also - Don't use air ideal gas for buoyancy unless you have large temperature/pressure variations. Use an incompressible flow with the thermal buoyancy coefficient set instead.

Glenn Horrocks

[Blob]

Hi, maybe you've resolved all the issues by now, but I had a few thoughts. From your simulation screen shots, it seems like the stratification interface is a little low and there is too much mixing. Did you set the inlet volumetric flow rate correctly relative to the heat flux entering the room? Also, what kind of turbulence model are you using?

[flyingd]

Originally Posted by pulgarcito

Hi to all,

I dont understand your interesting in simulate solid regions. Just simulate only fluid domain and represent human bodies as a wall using heat flux (total or convective deppending if you plan to simulate radiation or not). In my experience, displacement ventilation simulation works great with boussinesq aproximation for buoyancy. You will encounter more numerical stability using boussinesq rather than real gas state equation.

perhapls helps you to run calculations in transient mode, reducing g value to add an extra "relaxation" for momentum equations. Then increase g value untill the desired conditions.

Sorry for my english

Regards

I meet the same error,but if there is no free surface the model is ok.
why: