ROOM AIR CONDITIONING PROBLEM DESCRIPTION: The problem considered here is a closed room with a heat generation source inside. The conditioned air injected into the room to m aintain proper conditions which alternately cools down the component and prevents overheating. The model consists of an inlet vent at the bottom of a wall. There is an outlet vent on the ceiling and a heat source in the middle of the room as shown. Software used are GAMBIT and FLUENT.
GEOMETRY: 1) Open GAMBIT , under operation panel select GEOMETRY COMMAND BUTTON,
. select create vertices
(7,0,0) (7,7,0) (0,7,0) enter these values in global -> APPLY .
create 4 vertices at (0,0,0)
2) Select EDGE COMMAND BUTTON
next to vertices, select CREATE EDGE
.select
two vertices (hold shift+left click every time to select the specific vertex,edge,face,volume etc)->
APPLY . Join all the vertices to make a square.
3) NEXT, select FACE COMMAND BUTTON
next to edge button. Select
. Select all
four edges (holding shift+left click )-> APPLY . 4) To generate the room volume, create one more edge by repeating steps 1 and 2 . USE MOVE/COPY
. Pick the vertex at origin (0, 0, 0) select copy and enter (0, 0, 7) in global window. This will create vertex at ( X=0 Y=0 Z=7). Join them.
5)
Select volume
next to face button. Right click on
. Select
sweep face from drop-down list. Select t he FACE in face, then, click in window next to edge to activate it (it will turn into yellow) and select just drawn edge, (to change the direction to be extrude hold shift+middleclick) -> APPLY. this case is extruded in –ve “Z” Direction.
6)
Now, create Heat source (repeat the steps 1-5 with some changes). 6.1) create vertices at (X=2.5, Y=0, Z=-2.5) and (X=4.5, Y=0, Z=-2.5) in global. Copy both vertices by entering global values (0, 3, 0). 6.2) join all the vertices using by EDGE COMMAND BUTTON. 6.3) Form a FACE. 6.4) create vertex at (0, 0, 2) (use copy functions) and join them.
6.5) Repeat step 5 to extrude it.
7) Creating inlet and outlet vent. 7.1) For inlet vent create two vertices at (3, 0.3, 0) and (4, 0.3, 0) 7.2) copy them at (0, 1, 0) 7.3) For outlet vent make two vertices at (1, 7, -2.75) and (1.5, 7, -2.75) 7.4) copy them at (0, 0, -1) 7.5) join all the vertices and form faces.
8) Before generating mesh, split the faces and volume.
8.1) Go to face panel, select SPLIT/MERGE faces
. Select face1 and under that select
face14-> APPLY . NEXT select face6 and under that face15-> APPLY .
8.2) Go to volume in geometry. Select SPLIT/MERGE volume,
. Select volume1 in the
above, then, select volume2 in the lower volume window-> APPLY and save the model.
MESHING:
1) Select mesh button in operation panel
select edge mesh
then select
. Under this
. Select all the edges of the room and define the
interval count 20 units(interval count can be obtained by right click on interval size bar).
2)
Assign 10 no’s(interval count) for longer edges and 6 for the samller edges of HEAT SOURCE.
3) for inlet vent assign 4 no’s(interval count) for all edges. 4)
Assign 4 no’s for longer and 3 for smaller edges of outlet vent.
5) Select volume command button
, under this panel select, mesh volumes
keeping interval size default, change ELEMENTS--- to TET/HYBRID mesh the volume1 and
volume2.
APPLYING BOUNDARY CONDITIONS:
1) Select ZONE COMMAND BUTTON
BOUNDARY TYPES COMMAND
, select SPECIFY
select the faces of the room, assign them
according to their position(right, left, top etc), select the appropriate FACE(top, bottom, front) in
ENTITY, select WALL in TYPE (right/left click and hold to scroll betew een BC’s)-> APPLY. 2) Apply the same BC for the server. 3) Select INLET face and apply VELOCITY INLET and PRESSURE OUTLET for OUTLET vent.
4) Select solid in “type” and volume2 in “volumes” in SPECIFY CONTINUUM TYPE
, name as
HEAT SOURCE. 5) Select solver as FLUENT5/6 in SOLVER in MAIN MENU. 6) Now save and EXPORT the mesh
MAIN MENU> FILE> EXPORT Save as XXXXX.msh
SOLVING THE PROBLEM: OPEN FLUNT, Select 3ddp from the list of options and click Run. The "3ddp" option is used to select the 3-dimensional, double-precision solver. In the double-precision solver, each floating point number is represented using 64 bits in contrast to the single -precision solver which uses 32 bits. The extra bits increase not only the precision but also the r ange of magnitudes that can be represented. The downside of using double precision is that it requires more memory.
1) Import the saved mesh FILE->READ-> CASE (navigate to saved folder). 2) Check for any errors in the grid—GRID->CHECK. Check the grid to make sure that there are no errors. 3) Scale the mesh GRID->SCALE-> SCALE (it is important to scale the mesh as fluent reads it in meters).
4) EXAMINE the imported mesh DISPLAY->GRID.
DEFINING SOLVER PROPERTIES: 1) MAIN MENU-> DEFINE-> MODELS-> SOLVER -> select GREEN-GAUSS NODE BASED . 1.1) MAIN MENU-> DEFINE-> VISCOUS-> K-epsilon, STANDARD and STD. WALL FUNCTIONS . Under Model , select the K-epsilon turbulence model. We will use the STANDARD model in the k-epsilon Model box ( because Realizable k-epsilon model produces more accurate results for boundary layer flows) Near-wall treatment box, check for standard wall
functions because of no boundary layers.
1.2) MAIN MENU-> DEFINE-> MATERIALS-> in DENSITY select Incompressible-ideal-gas and in
VISCOSITY select SUTHERLAND (three equation method).
DEFINE HEAT SOURCE MATERIAL. MAIN MENU-> DEFINE-> MATERIAL-> under material type change to SOLID (change the name and formula)-> CHANGE/CREATE (do not over wirte aluminium).
OPERATING CONDITIONS: FLUENT uses gauge pressure internally. Any time an absolute pressure is needed, it is generated by adding the operating pressure to the gauge pressure. We'll use the de fault value of 1 atm (101,325 Pa) as the Operating Pressure.
MAIN MENU->DEFINE-> OPERATING CONDITIONS -> select default conditions-> OK
DEFINING BOUNDARY CONDITIONS “VELOCITY INLET” MAIN MENU-> DEFINE-> BOUNDARY CONTIONS-> INLET-> SET-> use magnitude, normal to boundary and velocity magnitude to 1m/s and temperature to 290K in thermal tab.
Specifying Boundary contition for HEAT SOURCE 1) select Heat-source-> SET-> check that heat-source is selected in drop-down (material name) 2) check-> SOURCE TERMS.
2) source term-> edit-> assign no of energy source to 1 ->none to constant-> 1000-> OK.
Outlet In the Boundary Conditions window, look under Zones. Select Outlet to check the details of the boundary condition. The boundary condition type should be default selected to pressure-outlet: if it didn't, select it. Click Edit, and ensure that the Gauge Pressure is default to 0. If it is, close this window.
SOLVE: The order of discretization that we just set refers to the convective terms in the equations; the discretization of the viscous terms is always second-order acc urate in FLUENT. Second-order discretization generally yields better accuracy while first-order discretization yields more robust convergence. If the second-order scheme doesn't converge, you can try starting the iterations with the first-order scheme and switching to the second-order scheme after some iterations.
MAIN MENU->SOLVE-> SOLUTION-> SECOND ORDER(in discrization panel) and rest default-> OK
RESIDUALS: Plotting of residuals-> SOLVE-> MONITERS-> RESIDUAL-> PLOT-> NONE (convergence criterion)-> OK. Change the residual under Convergence Criterion to NONE . Also, under Options, select Print and Plot. This will print the residuals in the main window and plot the residuals in the graphics window as they are calculated.
INITIALIZING: SOLVE-> INITIALIZE-> select INLET in compute from drop-down -> INITIALIZE.
RUN THE SOLUTION:
SOLVE-> ITERATE(set 1000 iterations).
AFTER CONVERGENCE SAVE THE SOLUTION. MAIN MENU-> FILE-> WRITE-> CASE AND DATA. ANALYZING: 1. Verify that mass is conserved.
(a) Ensure Mass Flow Rate is selecte d from the Options list. (b) Select inlet and outlet from the Boundaries selection list. (c) Click Compute. ANSYS FLUENT displays the total mass flux across each boundary selected. _ The mass flow rate for the inlet should be positive (indicating that mass is entering the domain), while that for the outlet should be negative (indicating that mass is leaving the domain). _ The net mass flux appears in the box at the lower right corner of the Flux Reports dialog box. _ The net mass flux (inlet plus outlet) should be almost zero, indicating that mass is conserved.
POST PROCESSING: CREATING ISO-SURFACE 1) MAIN MENU->SURFACE-> ISO-SURFACE 1.1)Select GRID and X-COORDINATE in SURFACE OF CONSTANT drop-down list 1.2)Click COMPUTE and retain 3.5 value in ISO-VALUES. 1.3)Enter name for appropriate ISO-SURFACE. 1.4)Click CREATE. 1.5)REPEAT THE SAME FOR Y(iso-value 0.9) AS WELL AS Z-Coordinate(iso-value -3.5).
DISPLAY CONTOURS FOR DIFFERENT PARAMETERS:
1.1)Make sure that FILLED is selected in OPTIONS 1.2)Check DRAW GRID is selected and select OUTLINE in EDGE TYPE.
1.3)Select PRESSURE AND STATIC PRESSURE in Contours of drop-down list. 1.4)Select X-Coordinate ISO-SURFACE. 1.5)Click DISPLAY. 1.6)Contours for VELOCITY, TEMPERATURE, and TURBULENCE etc can be obtained.
REPEAT THE SAME FOR CONTOURS OF ; 1) TOTAL TEMPERATURE. 2) VELOCITY. 3) PRESSURE (static and total).
DISPLAY VECTORS FOR VELOCITY PROFILE. 1) MAIN MENU-> DISPLAY-> VECTORS. 2) Keep everything default 3) To increase the size of the vector arrows modify range in SCALE . 4) Select any ISO-SURFACE (FLUENT displays interior by
default) and click DISPLAY.
- - - - - - -PLEASE SHARE- - - - - - -
