hvac boundry conditions
 

hello,
i want to ask that where to put the ambient temperature boundry condition on the oulet of the AC or the wall of the room.

Boundary Condition
 

Depends on the domain. If you are simulating the flow within the room, then walls of the room can be given an ambient temperature; though it is not a very good condition but still an appropriate one. However, if you are simulating flow within the AC, then the room may not even be part of the domain and boundary condition has to be applied at the vent.

Thank you very much for your reply. I want to do CFD of the surrounding of an empty room with no windows or anything. i have a oulet at top of ac . when i give boundry conditions at the wall too then it stills shows simulation insides the ac . the velocity countour shows from inlet to outlet within the ac not with the surroundings. kindly help me with this..

Again thankyou
Regards :)

mtalha976, do you have some pictures of your domain, boundary conditions and other settings? It's a little hard to imagine based on your description and it's hard to diagnose without knowing more details.

srsel6

Iam attaching Geometry and Meshing Diagram . In the geometry there is inlet at front of Ac and 2 oulets at top of Ac. The inlet Speed is 3m/s and inlet temperature is 290k. The ambient temperature is 318k . It is transient solution and hybrid initialization . and number of timestep is 500 and size is 1 and iterations is 20.

Simulation in the room
 

The reason for that is the existence of the AC. Only the inlet and outlet boundaries of the AC need to be there, not the body representing the AC. There should only be one body at the Ansys Meshing stage. That should be of the room. The boundaries of the AC and room are shared. So, after removing the AC body, the boundaries will still be there.

Another approach to do this is within Fluent. Check your cell zones. If it shows two cell zones, then you need to identify which one represents AC. If you have already used relevant names, then just go to Mesh > Zones > Delete. Select the zone of the AC and delete it.

If the names are not representative then you can do a mesh check and look at the number of cells reported in two cell zones. Assuming AC has lesser number of cell, check the ID of the zone reported in the mesh check with lesser number of cells. Then, go to Mesh > Zones > Delete and delete the relevant one. If this process is not very clear then you may do it the following way.

Go to Surfaces > Zone and then select both, AC and Room, cell zones in the list on the left and click on Create. This will create two surface. Go to Display > Graphics > Mesh and display one of the newly created surfaces. Since the names are same as those of cell zones, you will be able to identify which one is AC and which one is room. Delete the AC.

The above is doable only if you have two zone. Considering the statements in your post, you appear to have two zones. So, the above should work.

The picture attached shows it has one zone. what should i do now?

thankyou :)

A step back
 

In that case, you should not have AC body at all. If it is there, then I'd suggest you take a step back or may be two, go to your CAD model, and ensure that there is no body representing AC. It should only be the imprint of the boundaries of AC and not a body representing AC.

Thank you for your cooperation .

I want to ask how can i represent Ac and Room as one body. when i do boolean operation of subtract it makes a rectangular slot on the face where Ac is attached . kindly help me with this.

Regards
Muhammad Talha

It's supposed to be like that. Your CAD model must only contain the fluid. So now you apply your boundary conditions on the rectangular face where the AC is supposed to be attached.

AC and room
 

Since the objective is to study the flow in the room, body of the AC is not required. Hence, you should remove the AC body. The rectangular slots are required because those are the boundaries to be used for applying inlet and outlet in Fluent. AC is not important here, only room is. But the boundaries that are shared by the AC with the room should be considered. Since those are shared, those exist within the room body as well.

I want to represent the ac body as well.. Because i want to study air at different angles of the ac grill and want to make it inlet. Is there any way to make as one body of both .

Thanks

Objective
 

If the objective would have been to study the flow in the AC, then the body of the AC makes sense. To apply flow at angle, you just need to provide the angle at the inlet to the room, i.e., outlet vent of the AC.

In case you really want to consider the AC, then there won't be any external boundary for you to apply any condition. You will have to consider a small surface or volume within the AC to represent its blower and apply a momentum source. If the objective is only to consider the angle of the flow at the grill, then this would still not serve the purpose.

Hence, it would be advisable to not consider the AC and apply the condition at the vent with any angle of the flow that you want. You may also change the angle with time.

Thank You vinerm.
My objective is to study the effect of room Due to HVAC . My AC model is split type which means after changing grills angle i can flow in any direction. i want AC to be there also so that i can give inlet at grills and study the room effects.
Can you help me with this.

Effect of Grill
 

If you want to model the effect of the grill angle, you can just specify the angle at the inlet to the room. If you want to simulate the grill, then you have to create a model of the grill not the AC. The flow within the AC is much more complicated than in the room and will not be of any use for the simulation of the room.

vinerm,

My objective is CFD Analysis of Air Conditioning in Room Using Ansys Fluent. at different angles of grill and different parameters. for this purpose i have to represent a Ac in room to see the simulations coming out from Ac into the room . but it represent a two bodies in design modular. but i want to b represent as one body(i-e the Ac and face combined) i have seen simulations where it is taking as duct straight. my model is split type Ac

Scenario
 

Let me rephrase the scenarios and then you can choose which one you want.

The room has a split AC fitted with one outlet and one inlet. Outlet of AC is inlet to the room and outlet of room is inlet to the AC. Objective is to predict the flow and thermal field in the room. Angle at the inlet can be changed; this can be changed during the simulation or it could be multiple cases with different angles. Mass flow rate or velocity inlet can be applied at the inlet of the room (outlet of grill) and pressure outlet or mass flow rate at outlet of the room (inlet of the AC). AC body is not required. This is scenario 1. All you need to know is flow rate or velocity vector from the grill and its temperature.

Now, imagine that you include the body of the AC as well. Since the room and the AC are connected to each other via walls, grill (AC outlet), and suction window (AC inlet), you do not have any boundary where you can apply a boundary condition. AC could be a simple box or the ducted path as it is exists in a real split indoor unit. Since there is no external boundary, the option is to apply momentum and energy source within the AC body. Momentum source will represent the blower and energy source (it will be negative) will represent the evaporator coil. By including the complexity of determining these source values, which would require you to know the blower profile and AC rating, the extra information that you will get is flow inside the AC box, which it appears is not your objective. So, in this scenario, you will increase the complexity with no extra, useful output.

Simulation can be done both ways, depending upon what information you have and what do you wish to achieve.

Thank you very much vinerm. The Objective of my problem was solved when i followed your steps . You helped a lot for me to understand this.
.
i want to ask how many step size or number of time steps should be needed to give me good results. i have tried 500 and 1000 with 0.01 step but it is not giving me a lot of information ,small part of room is only studied. kindly help me with this.

Thanks again :)

Transient or Steady-state
 

If the objective is to study the time required to reach a certain temperature, then you need to run for as many number of time-steps as many needed to reach the required temperature. If the objective is to study the thermal field in the room, then you do not require a transient simulation. Run a steady-state simulation with at least 2000 iterations or until the thermal field becomes stable.

vinerm,

My objective is too study CFD of the Surroundings of the room. For this purpose ,which is more convenient?

Thanks.