I have successfully created a few flow models, but I have now been tasked with showing how heat from equipment within a building.
I have read through the documentation and watched some of the videos, but none have helped. I have tried to create the model with Total Heat Generation (in W) and with surfaces set to a Temperature (F), but I am not getting what I expected.
This building houses several generators and engines. I created a pretty simplified model in Revit, I setup two options in this file, one using Total Heat and the other with surface Temperature.
Ambient is 97F
Engines operate at 214f (large polygonal)
Exhaust and Turbo operates a732f (60"d Duct and boxes)
Generators (Boxes opposite end from Exhaust) operate at 241f
all openings in walls are outside air for cooling (18m3/s)
vents in roof
Please can you share a CFZ file with us? We cannot open a CFDST without the associated files, which are all created when you double click a CFZ.
There will be one (_support) in the folder above or you can save one from the interface 'S' -> Save Share File.
Here is my base model with only materials and (air) boundary conditions assigned. This model was working earlier but now refuses to solve.
This should be a pretty easy and quick fix, there are 2 rules to note and making these changes should see this running well:
- We cannot have pressure and flow Boundary Conditions (BC) on the same surface. The inlets look good, v and T makes sense. The outlets should just be P=0 and nothing else
- You cannot have internal surface BC's. You have a pressure and Temperature on the floor. All BC's must be on the external surfaces of what we are meshing. You could use a film coefficient on the underside of the entire model to allow heat to escape if that is the goal? 5W/m2/K at 97F is sensible.
Otherwise, this looks great, nice work.
What I am really trying to show is how the heat for the engines, exhaust, and generators build up within the envelope of the building so we can see where we can and can not run cable tray (derating due to excessive heat). Once we have a base line done, I will change the location(s) and size(s) of the inlets to see how the changes things. Lastly, we may design some kind of additional HVAC to cool the areas where the cable trays are.
I have taken everything except inlet volume and outlet press out of the model. it looks to be running.
Would you recommend using total heat generation or temperature to represent the heat gain (from the equipment) into the space?
Volumetric heat load is probably best. You could use a fixed temp if you suppressed the engines from the mesh, I would have thought this would be less realistic?
(Atleast) one more question....
the generator actually have an internal fan that blows the heated air up into the ceiling space. if I can't have a BC within the model space, how should I show that air/heat flow?
There are 2 approaches here.
- If you have a known temp, supress the generator and have a recessed cylinder in the top - the end of which you will have a temp and flow rate Boundary Condition assigned.
- If the temp is not known and you are just pulling local air from one side of the fan to the other, we have an axial/internal fan material for this exact purpose. You would need to model a cylinder to represent the blades, a shroud around the outside (suppressed from the mesh if you choose).
There is a decent reference in the Wiki on Axial Fans here. The inlet to that model is less than ideal though, very short.