A furnace with dimensions of its cross-section specified in Fig. 6.1 is constructed from two materials. The inner wall is made of concrete with a thermal conductivity, k_c = 0.01 W/m K. The outer wall is constructed from bricks with a thermal conductivity, k_b = 0.0057 W/m K. The temperature within the furnace is 673 K and the convection heat transfer coefficient k₁ = 0.208 W/m² K. The outside wall of the furnace is exposed to the surrounding air, which is at 253 K and the corresponding convection heat transfer coefficient, k₂ = 0.068 W/m² K.

Determine the temperature distribution within the concrete and brick walls under steady-state conditions. Also determine the heat fluxes through each wall.

This is a 2D problem and will be modelled using GUI facilities.

6.2.2 Construction of the model

From the ANSYS Main Menu, select Preferences. This frame is shown in Fig. 6.2.

Depending on the nature of analysis to be attempted, an appropriate analysis type should be selected. In the problem considered here, [A] Thermal was selected, as shown in Fig. 6.2.

From the ANSYS Main Menu, select Preprocessor → Element Type → Add/Edit/Delete. The frame shown in Fig. 6.3 appears.

Clicking the [A] Add button activates a new set of options, which are shown in Fig. 6.4.

Fig. 6.4 shows that for the problem considered, the following were selected: [A] Thermal Mass → Solid and [B] 4node 55. This element is referred to as Type 1 PLANE55.

From the ANSYS Main Menu, select Preprocessor → Material Props → Material Models. Fig. 6.5 shows the resulting frame.

From the right-hand column, select [A] Thermal → Conductivity → Isotropic. As a result, the frame shown in Fig. 6.6 appears. Thermal conductivity [A] KXX = 0.01 W/m K was selected, as shown in Fig. 6.6.

Clicking the [B] OK button ends input into Material Number 1. In the frame shown in Fig. 6.7, select from the top menu [A] Material → New Model. A database for Material Number 2 is created.

As in the case of Material Number 1, select [B] Thermal → Conductivity → Isotropic. The frame shown in Fig. 6.8 appears. Enter [A] KXX = 0.0057 W/m K and click the [B] OK button as shown in Fig. 6.8.

In order to create numbered primitives from the ANSYS Utility Menu, select PlotCtrls → Numbering and check the box area numbers.

From the ANSYS Main Menu, select Preprocessor → Modelling → Create → Areas → Rectangle → By Dimensions. Fig. 6.9 shows the resulting frame.

Input [A] X1 = − 15; [B] X2 = 15; [C] Y1 = − 15 and [D] Y2 = 15 to create an outer wall perimeter area as shown in Fig. 6.9. Next, the perimeter of the inner wall is created in the same way. Fig. 6.10 shows a frame with appropriate entries.

In order to generate the brick wall area of the chimney, subtract the two areas that have been created. From the ANSYS Main Menu, select Preprocessor → Modelling → Operate → Booleans → Subtract → Areas. Fig. 6.11 shows the resulting frame.

First, select the larger area (outer brick wall) and click the [A] OK button in the frame of Fig. 6.11. Next, select the smaller area (inner concrete wall) and click the [A] OK button. The smaller area is subtracted from the larger one, and the outer brick wall is produced. This is shown in Fig. 6.12.

Using a similar approach, the inner concrete wall is constructed. From the ANSYS Main Menu, select Preprocessor → Modelling → Create → Areas → Rectangle → By Dimensions. Fig. 6.13 shows the resulting frame with inputs: [A] X1 = − 6; [B] X2 = 6; [C] Y1 = − 6 and [D] Y2 = 6. Pressing the [E] OK button creates rectangular area A1.

Again, from the ANSYS Main Menu, select Preprocessor → Modelling → Create → Areas → Rectangle → By Dimensions. A frame with inputs: [A] X1 = − 5; [B] X2 = 5; [C] Y1 = − 5 and [D] Y2 = 5 is shown in Fig. 6.14.

Clicking the [E] OK button creates rectangular area A2. As before, to create the concrete area of the furnace, subtract area A2 from area A1. From the ANSYS Main Menu, select Preprocessor → Modelling → Operate → Booleans → Subtract → Areas. The frame shown in Fig. 6.11 appears. Select area A1 first and click the [A] OK button. Next, select area A2 and click the [A] OK button. As a result, the inner concrete wall is created. This is shown in Fig. 6.15.

From the ANSYS Main Menu, select Preprocessor → Meshing → Size Cntrls → ManualSize → Global → Size. As a result of this selection, the frame shown in Fig. 6.16 appears.

Set the input for the element edge length as [A] SIZE = 0.5 and click the [B] OK button.

Because the outer brick wall and inner concrete wall were created as separate entities, it is necessary to ‘glue’ them together so they share lines along their common boundaries. From the ANSYS Main Menu, select Preprocessor → Modelling → Operate → Boolean → Glue → Areas. The frame shown in Fig. 6.17 appears.

Select the [A] Pick All option in the frame of Fig. 6.17 to glue the outer and inner wall areas. Before meshing occurs, it is necessary to specify material numbers for the concrete and the brick walls.

From the ANSYS Main Menu, select Preprocessor → Meshing → Mesh Attributes → Picked Areas. The frame shown in Fig. 6.18 is created.

Select the first concrete wall area and click the [A] OK button in the frame of Fig. 6.18. A new frame is produced, as shown in Fig. 6.19.

Material Number 1 is assigned to the concrete inner wall, as shown in Fig. 6.19.

Next, assign Material Number 2 to the brick outer wall following the procedure outlined above and select the brick outer wall. Fig. 6.20 shows a frame with an appropriate entry.

Now meshing of both areas can be carried out. From the ANSYS Main Menu, select Preprocessor → Meshing → Mesh → Areas → Free. The frame shown in Fig. 6.21 appears.

Select [A] Pick All option shown in Fig. 6.21 to mesh both areas.

In order to see both areas meshed, from the Utility Menu, select PlotCtrls → Numbering. In the resulting frame, shown in Fig. 6.22, select [A] Material Numbers and click the [B] OK button.

As a result, both walls with mesh are displayed (see Fig. 6.23).

6.2.3 Solution

Before a solution can be run, boundary conditions have to be applied. From the ANSYS Main Menu, select Solution → Define Loads → Apply → Thermal → Convection → On Lines. This selection produces a frame shown in Fig. 6.24.

First, pick the convective lines (facing inside the furnace) of the concrete wall and press the [A] OK button. The frame shown in Fig. 6.25 is created.

As seen in Fig. 6.25, the following selections were made: [A] Film coefficient = 0.208 W/m² K and [B] Bulk temperature = 673 K, as specified for the concrete wall in the problem formulation.

Again from the ANSYS Main Menu, select Solution → Define Loads → Apply → Thermal → Convection → On Lines. The frame shown in Fig. 6.24 appears. This time, pick the exterior lines of the brick wall and press the [A] OK button. The frame shown in Fig. 6.26 appears.

For the outer brick wall, the following selections were made (see the frame in Fig. 6.26): [A] Film coefficient = 0.068 W/m² K and [B] Bulk temperature = 253 K as specified for the brick wall in the problem formulation.

Finally, to see the applied convective boundary conditions from the Utility Menu, select PlotCtrls → Symbols. The frame shown in Fig. 6.27 appears.

In the frame shown in Fig. 6.27, select [A] Show pres and convect as = Arrows and click the [B] OK button.

From the Utility Menu, select Plot → Lines to produce an image shown in Fig. 6.28.

To solve the problem, from the ANSYS Main Menu, select Solution → Solve → Current LS. Two frames appear. One gives a summary of solution options. After checking the correctness of the options, close this using the menu at the top of the frame. The other frame is shown in Fig. 6.29. Clicking the [A] OK button initiates the solution process.

6.2.4 Postprocessing

The end of the successful solution process is denoted by the message ‘Solution is done’. The postprocessing phase can be started. It is first necessary to obtain information about temperatures and heat fluxes across the furnace's walls.

From the ANSYS Main Menu, select General Postproc → Plot Results → Contour Plot → Nodal Solu. The frame shown in Fig. 6.30 appears.

Selections made are shown in Fig. 6.30. Clicking the [A] OK button results in the graph shown in Fig. 6.31.

In order to observe the heat flow across the walls the following command should be issued: General Postproc → Plot Results → Vector Plot → Predefined. This produces the frame shown in Fig. 6.32.

Clicking the [A] OK button produces a graph as shown in Fig. 6.33.

In order to observe temperature variations across the walls, it is necessary to define the path along which the variations are going to be determined. From the Utility Menu, select Plot: Areas. Next, from the ANSYS Main Menu, select General Postproc → Path Operations → Define Path → On Working Plane. The resulting frame is shown in Fig. 6.34.

By activating the [A] Arbitrary path button and clicking [B] OK, another frame is produced and is shown in Fig. 6.35.

Two points should be selected by clicking on the inner line of the concrete wall and moving in Y-direction at the right angle, clicking on the outer liner of the brick wall. As a result of clicking the [A] OK button, the frame shown in Fig. 6.36 appears.

In the box [A] Define Path Name, write AB and click the [B] OK button.

From the ANSYS Main Menu, select General Postproc → Path Operations → Map onto Path. The frame shown in Fig. 6.37 appears.

In Fig. 6.37, the following selections are made: [A] Flux & gradient, [B] Thermal grad TGX; then click the [C] OK button. Repeating the steps described above, recall the frame shown in Fig. 6.37. This time, select the following: [A] Flux & gradient, [B] Thermal grad TGY, and click the [C] OK button. Finally, recall the frame shown in Fig. 6.37 and select [A] Flux & gradient and [B] Thermal grad TGSUM as shown in Fig. 6.38, then click the [C] OK button.

From the ANSYS Main Menu, select General Postproc → Path Operations → Plot Path Item → On Graph. The frame shown in Fig. 6.39 appears.

The selections made [A] are highlighted in Fig. 6.39. Pressing the [B] OK button results in a graph as shown in Fig. 6.40.

A cylindrical tank is penetrated radially by a small pipe at a point on its axis remote from the ends of the tank, as shown in Fig. 6.41.

The inside of the tank is exposed to fluid with a temperature of 232°C. The pipe experiences a steady flow of fluid with a temperature of 38°C, and the two flow regimes are isolated from each other by means of a thin tube. The convection (film) coefficient in the pipe varies with the metal temperature and is thus expressed as a material property. The objective is to determine the temperature distribution at the pipe-tank junction.

The following data describing the problem are given:

• • inside diameter of the pipe = 8 mm;
• • outside diameter of the pipe = 10 mm;
• • inside diameter of the tank = 26 mm;
• • outside diameter of the tank = 30 mm;
• • inside bulk fluid temperature, tank = 232°C;
• • inside convection coefficient, tank = 4.92 W/m² °C;
• • inside bulk fluid temperature, pipe = 38°C; and
• • inside convection (film) coefficient, pipe = − 2.

Table 6.1 provides information about variation of the thermal parameters with temperature.

The assumption is made that the quarter symmetry is applicable and that, at the terminus of the model (longitudinal and circumferential cuts in the tank), there is sufficient attenuation of the pipe effects such that these edges can be held at 232°C.

The solid model is constructed by intersecting the tank with the pipe and then removing the internal part of the pipe using a Boolean operation.

Boundary temperatures along with the convection coefficients and bulk fluid temperatures are dealt with in the solution phase, after which a static solution is executed.

Temperature contours and thermal flux displays are obtained in postprocessing.

Details of steps taken to create the model of the pipe intersecting with the tank are outlined below.

6.3.2 Preparation for model building

From the ANSYS Main Menu, select Preferences. This frame is shown in Fig. 6.42.

Depending on the nature of analysis to be attempted, an appropriate analysis type should be selected. In the problem considered here, [A] Thermal was selected, as shown in Fig. 6.42.

From the ANSYS Main Menu, select Preprocessor and then Element Type and Add/Edit/Delete. The frame shown in Fig. 6.43 appears.

Clicking the [A] Add button activates a new set of options, which are shown in Fig. 6.44.

Fig. 6.44 indicates that for the problem considered here, the following was selected: [A] Thermal Mass → Solid and [B] 20node 90.

From the ANSYS Main Menu, select Material Props and then Material Models. Fig. 6.45 shows the resulting frame.

From the options listed on the right-hand side, select [A] Thermal as shown in Fig. 6.45.

Next select [B] Conductivity, Isotropic. The frame shown in Fig. 6.46 is built up by pressing the Add Temperature button. When all five temperatures and corresponding KXX are entered in accordance with Table 6.1, the OK button should be pressed.

By selecting the [C] Specific Heat option in the right-hand column (see Fig. 6.45), the frame shown in Fig. 6.47 is produced.

Using a similar approach to that described above for conductivity, appropriate values of specific heat versus temperature, taken from Table 6.1, are typed as shown in Fig. 6.47.

The next material property to be defined is density. According to Table 6.1, density is constant for all temperatures used. Therefore, selecting [D] Density from the right-hand column (see Fig. 6.45) results in the frame shown in Fig. 6.48.

A density of 7888.8 kg/m³ is typed in the boxes for various temperatures shown in Fig. 6.48.

All the above properties were used to characterise Material Number 1. The convection of the film coefficient is another important parameter characterising the system being analysed. However, this is a property belonging not to Material Number 1 (material of the tank and pipe) but to a thin film formed by the liquid on solid surfaces. It is a different entity, and is therefore called Material Number 2. Therefore, from the top menu Material (shown in Fig. 6.45), select New Model number 2. Next, [E] Convection or Film Coef. (see Fig. 6.45) should be selected and the frame shown in Fig. 6.49 created. Appropriate values of the film coefficient for various temperatures, taken from Table 6.1, are introduced as shown in Fig. 6.49. The consecutive temperatures T1, T2, T3, T4 and T5 and corresponding specific heat values are obtained by pressing the Add Temperature button.

6.3.3 Construction of the model

The entire model of the pipe intersecting with the tank is constructed using one of the three-dimensional primitive shapes, that is, a cylinder. Only one quarter of the tank-pipe assembly will be sufficient to use in the analysis. From the ANSYS Main Menu, select Preprocessor → Modelling → Create → Volumes → Cylinder → By Dimensions. Fig. 6.50 shows the resulting frame.

In Fig. 6.50, as shown, the following inputs are made: [A] RAD1 = 1.5 cm; [B] RAD2 = 1.3 cm; [C] Z1 = 0; [D] Z2 = 2 cm; [E] THETA1 = 0; [F] THETA2 = 90.

As the pipe axis is at right angles to the cylinder axis, it is necessary to rotate the working plane to the pipe axis by 90 degrees. This is achieved by selecting from the Utility Menu WorkPlane → Offset WP by Increments. The resulting frame is shown in Fig. 6.51.

In Fig. 6.51, the input is shown as [A] XY = 0; YZ = − 90 and the ZX is left unchanged from default value. Next, from the ANSYS Main Menu, select Preprocessor → Modelling → Create → Volumes → Cylinder → By Dimensions. Fig. 6.52 shows the resulting frame.

In Fig. 6.52, as shown, the following inputs are made: [A] RAD1 = 0.5 cm; [B] RAD2 = 0.4 cm; [C] Z1 = 0; [D] Z2 = 2 cm; [E] THETA1 = 0; [F] THETA2 = − 90.

After that the working plane should be set to the default setting by inputting in Fig. 6.51 YZ = 90 this time. As the cylinder and the pipe are separate entities, it is necessary to overlap them in order to make one component. From the ANSYS Main Menu, select Preprocessor → Modelling → Create → Operate → Booleans → Overlap → Volumes. The frame shown in Fig. 6.53 is created.

Pick both elements (cylinder and pipe) and press the [A] OK button to execute the selection. Next, activate volume numbering, which will be of use when carrying out further operations on volumes. This is done by selecting from the Utility Menu PlotCtrls → Numbering and checking the VOLU option in the resulting frame.

Finally, a three-dimensional view of the model should be set by selecting the following from the Utility Menu: PlotCtrls → View Settings → Viewing Direction. The resulting frame is shown in Fig. 6.54.

The following inputs should be made (see Fig. 6.54): [A] XV = − 3; [B] YV = − 1; [C] ZV = 1 to plot the model, as shown in Fig. 6.55. However, this is not the only possible view of the model, and any other preference may be chosen.

Certain volumes of the models, shown in Fig. 6.55, are redundant and should be deleted. From the ANSYS Main Menu, select Preprocessor → Modelling → Delete → Volumes and Below. Fig. 6.56 shows the resulting frame.

Volumes V4 and V3 (a corner of the cylinder) should be picked and the [A] OK button pressed to implement the selection. After the delete operation, the model should look like that shown in Fig. 6.57.

Finally, volumes V5, V6 and V7 should be added to create a single volume required for further analysis. From the ANSYS Main Menu, select Preprocessor: Modelling: Operate: Booleans: Add: Volumes. The resulting frame asks for picking volumes to be added. Pick all three volumes—V5, V6, and V7—and click the OK button to implement the operation. Fig. 6.58 shows the model of the pipe intersecting the cylinder as one volume V1.

Meshing of the model usually begins with setting the size of elements to be used. From the ANSYS Main Menu, select Meshing → Size Cntrls → SmartSize → Basic. A frame, shown in Fig. 6.59, appears.

For the case considered, [A] Size Level—1(fine) was selected, as shown in Fig. 6.59. Clicking the [B] OK button implements the selection. Next, from the ANSYS Main Menu, select Mesh → Volumes → Free. The frame shown in Fig. 6.60 appears. Select the volume to be meshed and click the [A] OK button.

The resulting network of elements is shown in Fig. 6.61.

6.3.4 Solution

The meshing operation ends the model construction and the Preprocessor stage. The solution stage can now be started. From the ANSYS Main Menu, select Solution → Analysis Type → New Analysis. Fig. 6.62 shows the resulting frame.

Activate the [A] Steady-State button. Next, select Solution → Analysis Type → Analysis Options. In the resulting frame, shown in Fig. 6.63, select the [A] Program chosen option.

To set the starting temperature of 232°C at all nodes, select Solution → Define Loads → Apply → Thermal → Temperature → Uniform Temp. Fig. 6.64 shows the resulting frame. Input [A] Uniform temperature = 232°C, as shown in Fig. 6.64.

From the Utility Menu, select WorkPlane: Change Active CS to → Specified Coord Sys. As a result, the frame shown in Fig. 6.65 appears.

To re-establish the cylindrical coordinate system with Z as the axis of rotation, select [A] Coordinate system number = 1 and press the [B] OK button to implement the selection.

Nodes on the inner surface of the tank should be selected to apply surface loads to them. The surface load relevant in this case is convection load acting on all at all nodes located on the inner surface of the tank. From the Utility Menu, choose Select → Entities. The frame shown in Fig. 6.66 appears.

From the first pull-down menu, select [A] Nodes; from the second pull-down menu, select [B] By location. Also, activate [C] X coordinates button and enter [D] Min,Max = 1.3 (inside radius of the tank). All four required steps are shown in Fig. 6.66. When the subset of nodes on the inner surface of the tank is selected, then the convection load at all nodes has to be applied. From the ANSYS Main Menu, select Solution → Define Load → Apply → Thermal → Convection → On nodes. The resulting frame is shown in Fig. 6.67.

Press [A] Pick All to call up another frame as shown in Fig. 6.68.

Inputs into the frame of Fig. 6.68 are shown as: [A] Film coefficient = 4.92 and [B] Bulk temperature = 232. Both quantities are taken from the problem description.

From the Utility Menu, choose Select → Entities in order to select a subset of nodes located at the far edge of the tank. The frame shown in Fig. 6.69 appears.

From the first pull-down menu, select [A] Nodes; from the second pull-down menu, select [B] By location. Also, activate [C] Z coordinates button and [D] enter Min,Max = 2 (the length of the tank in Z-direction). All four required steps are shown in Fig. 6.69. Next, constraints at nodes located at the far edge of the tank (additional subset of nodes just selected) have to be applied. From the ANSYS Main Menu, select Solution → Define Loads → Apply → Thermal → Temperature → On Nodes. The frame shown in Fig. 6.70 appears.

Click the [A] Pick All button as shown in Fig. 6.70. This action brings up another frame, as shown in Fig. 6.71.

Activate both [A] All DOF and TEMP and input [B] TEMP value = 232°C, as shown in Fig. 6.71. Finally, click [C] OK to apply temperature constraints on nodes at the far edge of the tank. The steps outlined above should be followed to apply constraints at nodes located at the bottom of the tank. From the Utility Menu, choose Select: Entities. The frame shown in Fig. 6.72 appears.

From the first pull-down menu, select [A] Nodes; from the second pull-down menu, select [B] By location. Also, activate the [C] Y coordinates button and [D] enter Min,Max = 0 (location of the bottom of the tank in Y-direction). All four required steps are shown in Fig. 6.72. Next, constraints at the nodes located at the bottom of the tank (additional subset of nodes selected above) must be applied. From the ANSYS Main Menu, select Solution → Define Loads → Apply → Thermal → Temperature → On Nodes. The frame shown in Fig. 6.70 appears. As shown in Fig. 6.70, click [A] Pick All to bring up the frame shown in Fig. 6.71. As before, activate both [A] All DOF and TEMP and input [B] TEMP value = 232°C. Clicking [C] OK applies the temperature constraints on the nodes at the bottom of the tank.

Now, it is necessary to rotate the working plane (WP) to the pipe axis. From the Utility Menu, select WorkPlane → Offset WP by Increments. Fig. 6.73 shows the resulting frame.

In the degrees box, input [A] XY = 0 and YZ = − 90 as shown. Having WP rotated to the pipe axis, a local cylindrical coordinate system must be defined at the origin of the working plane. From the Utility Menu, select WorkPlane → Local Coordinate Systems → Create local CS → At WP Origin. The resulting frame is shown in Fig. 6.74.

From the pull-down menu, select [A] Cylindrical 1 and click the [B] OK button to implement the selection. The analysis involves nodes located on the inner surface of the pipe. To include this subset of nodes, from the Utility Menu, choose Select → Entities. Fig. 6.75 shows the resulting frame.

From the first pull-down menu, select [A] Nodes; from the second pull-down menu, select [B] By location. Also, activate the [C] X coordinates button and [D] enter Min,Max = 0.4 (inside radius of the pipe). All four required steps are shown in Fig. 6.75. From the ANSYS Main Menu, select Solution → Define Load → Apply → Thermal → Convection → On nodes. In the resulting frame (shown in Fig. 6.67), press [A] Pick All and the next frame, shown in Fig. 6.76, appears.

Input [A] Film coefficient = − 2 and [B] Bulk temperature = 38, as shown in Fig. 6.76. Pressing the [C] OK button implements the selections. The final action is to select all entities involved with a single command. Therefore, from the Utility Menu, choose Select → Everything. For the loads to be applied to tank and pipe surfaces in the form of arrows from the Utility Menu, select PlotCtrls → Symbols. The frame in Fig. 6.77 shows the required selection: [A] Arrows.

From the Utility Menu, selecting Plot: Nodes results in Fig. 6.78, where surface loads at nodes are shown as arrows.

From the Utility Menu, select WorkPlane → Change Active CS to → Specified Coord Sys in order to activate the previously defined coordinate system. The frame shown in Fig. 6.79 appears.

Input [A] KCN (coordinate system number) = 0 to return to Cartesian system. Additionally, from the ANSYS Main Menu, select Solution → Analysis Type → Sol’n Controls. As a result, the frame shown in Fig. 6.80 appears.

Input the following: [A] Automation time stepping = On and [B] Number of substeps = 50, as shown in Fig. 6.80. Finally, from the ANSYS Main Menu, select Solve → Current LS and in the dialog box that appears, click the OK button to start the solution process.

6.3.5 Postprocessing stage

Once the solution is complete, the next stage is to display results in a form required to answer questions posed by the formulation of the problem.

From the Utility Menu, select PlotCtrls → Style → Edge Options. Fig. 6.81 shows the resulting frame.

Select [A] All/Edge only and press the [B] OK button to implement the selection; this will result in the display of the ‘edge’ of the object only. Next, graphic controls should be returned to default setting. This is done by selecting from the Utility Menu PlotCtrls → Symbols. The resulting frame, shown in Fig. 6.82, contains all default settings.

The first plot is to show temperature distribution as continuous contours. From the ANSYS Main Menu, select General Postproc → Plot Results → Contour Plot → Nodal Solu. The resulting frame is shown in Fig. 6.83.

Select [A] Temperature and press the [B] OK button as shown in Fig. 6.83. The resulting temperature map is shown in Fig. 6.84.

The next display of results concerns thermal flux at the intersection between the tank and the pipe. From the ANSYS Main Menu, select General Postproc → Plot Results → Vector Plot → Predefined. The resulting frame is shown in Fig. 6.85.

In Fig. 6.85, select [A] Thermal flux TF and [B] Raster Mode. Pressing the [C] OK button implements selections and produces thermal flux as vectors. This is shown in Fig. 6.86.

Ribbed or developed surfaces, also called fins, are frequently used to dissipate heat. There are many examples of their use in practical engineering applications, such as computers, electronic systems, and radiators, to mention a few.

Fig. 6.87 shows a typical configuration and geometry of a fin made of aluminium with thermal conductivity coefficient k = 170 W/m K.

The bottom surface of the fin is exposed to a constant heat flux of q = 1000 W/m. Air flows over the developed surface, keeping the surrounding temperature at 293 K. The heat transfer coefficient between the fin and the surrounding atmosphere is h = 40 W/m² K.

The task is to determine the temperature distribution within the developed surface.

6.4.2 Construction of the model

From the ANSYS Main Menu, select Preferences to call up a frame shown in Fig. 6.88.

Because the problem to be solved is asking for temperature distribution, [A] Thermal is selected, as indicated in the figure. Next, from the ANSYS Main Menu, select Preprocessor → Element Type → Add/Edit/Delete. The frame shown in Fig. 6.89 appears.

Click the [A] Add button to call up another frame as shown in Fig. 6.90.

In Fig. 6.90, the following selections are made: [A] Thermal Mass → Solid and [B] Tet 10 node 87. From the ANSYS Main Menu, select Preprocessor → Material Props → Material Models. Fig. 6.91 shows the resulting frame.

From the right-hand column, select [A] Thermal → Conductivity → Isotropic. In response to this selection, another frame, shown in Fig. 6.92, appears.

Thermal conductivity [A] KXX = 170 W/m K is entered and the [B] OK button is clicked to implement the entry, as shown in the figure.

The model of the developed area will be constructed using primitives, and it is useful to have them numbered. Thus, from the ANSYS Utility Menu, select PlotCtrls → Numbering and check the [A] box area numbers, as shown in Fig. 6.93.

From the ANSYS Main Menu, select Preprocessor → Modelling → Create → Areas → Rectangle → By Dimensions. Fig. 6.94 shows the resulting frame.

Input [A] X1 = − 165; [B] X2 = 165; [C] Y1 = 0; [D] Y2 = 100 to create a rectangular area (A1) within which the fin will be comprised. Next, create two rectangles at the left and right upper corners, to be cut off from the main rectangle. From the ANSYS Main Menu, select Preprocessor → Modelling → Create → Areas → Rectangle → By Dimensions. Fig. 6.95 shows the resulting frame.

Fig. 6.95 shows the inputs to create a rectangle (A2) at the left-hand upper corner of the main rectangle (A1). They are: [A] X1 = − 165; [B] X2 = − 105; [C] Y1 = 85; [D] Y2 = 100. To create right-hand upper corner rectangles (A3), repeat the above procedure, inputting the following: [A] X1 = 105; [B] X2 = 165; [C] Y1 = 85; [D] Y2 = 100. Now, areas A2 and A3 have to be subtracted from area A1. From the ANSYS Main Menu, select Preprocessor → Modelling → Operate → Booleans → Subtract → Areas. Fig. 6.96 shows the resulting frame.

First, select area A1 (large rectangle) to be subtracted from and click the [A] OK button. Next, select two smaller rectangles A2 and A3, and click the [A] OK button. A new area A4 is created with two upper corners cut off. Proceeding in the same way, areas should be cut off from the main rectangle to create the fin shown in Fig. 6.87.

From the ANSYS Main Menu, select Preprocessor → Modelling → Create → Areas → Rectangle → By Dimensions. Fig. 6.97 shows the frame in which appropriate inputs should be made.

To create area A1, input the following: [A] X1 = − 145; [B] X2 = − 125; [C] Y1 = 40; [D] Y2 = 85. In order to create area A2, input the following: [A] X1 = 125; [B] X2 = 145; [C] Y1 = 40; [D] Y2 = 85. In order to create area A3, input the following: [A] X1 = − 105; [B] X2 = − 95; [C] Y1 = 25; [D] Y2 = 100. In order to create area A5, input the following: [A] X1 = 95; [B] X2 = 105; [C] Y1 = 25; [D] Y2 = 100.

From the ANSYS Main Menu, select Preprocessor → Modelling → Operate → Booleans → Subtract → Areas. The frame shown in Fig. 6.96 appears. Select the first area A4 (large rectangle) and click the [A] OK button. Next, select areas A1, A2, A3 and A5, and click the [A] OK button. Area A6 with appropriate cut-outs is created, and is shown in Fig. 6.98.

To finish construction of the fin's model, use the frame shown in Fig. 6.97 and make the following inputs: [A] X1 = − 85; [B] X2 = − 75; [C] Y1 = 25; [D] Y2 = 100. Area A1 is created. Next, input [A] X1 = − 65; [B] X2 = − 55; [C] Y1 = 25; [D] Y2 = 100 to create area A2. Then input [A] X1 = − 45; [B] X2 = − 35; [C] Y1 = 25; [D] Y2 = 100 to create area A3. Appropriate inputs should be made to create areas, to be cut out later, on the right-hand side of the fin. Thus input [A] X1 = 85; [B] X2 = 75; [C] Y1 = 25; [D] Y2 = 100 to create area A4. Input [A] X1 = 65; [B] X2 = 55; [C] Y1 = 25; [D] Y2 = 100 to create area A5. Input [A] X1 = 45; [B] X2 = 35; [C] Y1 = 25; [D] Y2 = 100 to create area A7. Next, from the ANSYS Main Menu, select Preprocessor → Modelling → Operate → Booleans → Subtract → Areas. The frame shown in Fig. 6.96 appears. First select area A6 and click the [A] OK button. Then select areas A1, A2, A3, A4, A5, and A7. Clicking the [A] OK button implements the command and a new area A8 with appropriate cut-outs is created. To finalise the construction of the model, make the following inputs to the frame shown in Fig. 6.97 to create area A1: [A] X1 = − 25; [B] X2 = − 15; [C] Y1 = 50; [D] Y2 = 100. Input [A] X1 = − 5; [B] X2 = 5; [C] Y1 = 50; [D] Y2 = 100 to create area A2. Finally, input [A] X1 = 15; [B] X2 = 25; [C] Y1 = 50; [D] Y2 = 100 to create area A3. Again, from the ANSYS Main Menu, select Preprocessor → Modelling → Operate → Booleans → Subtract → Areas. The frame shown in Fig. 6.96 appears. Select first area A8 and click the [A] OK button. Next, select areas A1, A2 and A3. Clicking the [A] OK button produces area A4, as shown in Fig. 6.99.

Fig. 6.99 shows the final shape of the fin with dimensions as specified in Fig. 6.87. It is, however, a two-dimensional model. The width of the fin is 100 mm and this dimension can be used to create a three-dimensional model.

From the ANSYS Main Menu, select Preprocessor → Modelling → Operate → Extrude → Areas → Along Normal. Select Area 4 (to be extruded in the direction normal to the screen, i.e. Z-axis) and click the OK button. In response, a frame shown in Fig. 6.100 appears.

Input [A] Length of extrusion = 100 mm and click the [B] OK button. A three-dimensional model of the fin is created, as shown in Fig. 6.101.

The fin is shown in isometric view without area numbers. To deselect numbering of areas, refer to Fig. 6.93, in which box Area numbers should be unchecked.

From the ANSYS Main Menu, select Preprocessor → Meshing → Mesh Attributes → Picked Volumes. The frame shown in Fig. 6.102 is created.

Select [A] Pick All and the next frame, shown in Fig. 6.103, appears.

Material Number 1 and element type SOLID87 are as specified at the beginning of the analysis; to accept that, click the [A] OK button.

Now the meshing of the fin can be carried out. From the ANSYS Main Menu, select Preprocessor → Meshing → Mesh → Volumes → Free. The frame shown in Fig. 6.104 appears.

Select the [A] Pick All option, as shown in Fig. 6.104, to mesh the fin. Fig. 6.105 shows a meshed fin.

6.4.3 Solution

Prior to running the solution stage, boundary conditions must be applied properly. In the case considered here, the boundary conditions are expressed by the heat transfer coefficient, which is a quantitative measure of how efficiently heat is transferred from the fin surface to the surrounding air.

From the ANSYS Main Menu, select Solution → Define Loads → Apply → Thermal → Convection → On Areas. Fig. 6.106 shows the resulting frame.

Select all areas of the fin except the bottom area and click the [A] OK button. The frame created as a result of that action is shown in Fig. 6.107.

Input [A] Film coefficient = 40 W/m² K and [B] Bulk temperature = 293 K, and click the [C] OK button. Next, the heat flux of intensity 1000 W/m must be applied to the base of the fin. Therefore, from the ANSYS Main Menu, select Solution → Define Loads → Apply → Thermal → Heat Flux → On Areas. The resulting frame is shown in Fig. 6.108.

Select the bottom surface (base) of the fin and click the [A] OK button. A new frame appears (see Fig. 6.109) and the input made is as follows: [A] Load HFLUX value = 1000 W/m. Clicking the [B] OK button implements the input.

All required preparations have been made and the model is ready for its solution. From the ANSYS Main Menu, select Solution → Solve → Current LS. Two frames appear. One gives a summary of solution options. After checking the correctness of the options, this frame should be closed using the menu at the top of the frame. The other frame is shown in Fig. 6.110.

Clicking the [A] OK button starts the solution process.

6.4.4 Postprocessing

A successful solution is signalled by the message ‘Solution is done’. The postprocessing phase can now be initiated to view the results. The problem asks for temperature distribution within the developed area.

From the ANSYS Main Menu, select General Postproc → Plot Results → Contour Plot → Nodal Solution. The frame shown in Fig. 6.111 appears.

Select [A] Thermal Flux and [B] thermal flux vector sum, and click [C] OK to produce the graph shown in Fig. 6.112.

In order to observe how the temperature changes from the base surface to the top surface of the fin, a path along which the variations take place has to be determined. From the ANSYS Main Menu, select General Postproc → Path Operations → Define Path → On Working Plane. The resulting frame is shown in Fig. 6.113.

By activating the [A] Arbitrary path button and clicking the [B] OK button, another frame, shown in Fig. 6.114, is produced.

Two points should be picked: one that is on the bottom line at the middle of the fin and one, moving vertically upwards, on the top line of the fin. After that the [A] OK button should be clicked. A new frame appears and is shown in Fig. 6.115.

In the [A] Define Path Name box, write AB and click the [B] OK button.

From the ANSYS Main Menu, select General Postproc → Path Operations → Map onto Path. The frame shown in Fig. 6.116 appears.

Select [A] Flux & gradient and [B] TGSUM, and click the [C] OK button. Next, from the ANSYS Main Menu, select General Postproc → Path Operations → Plot Path Item → On Graph. Fig. 6.117 shows the resulting frame.

Select [A] TGSUM and click the [B] OK button to obtain a graph as shown in Fig. 6.118.

The graph shows temperature gradient variation as a function of distance from the base of the fin.

A block of material with thermal conductivity k = 10 W/m°C is assumed to be infinitely long. On three sides of it, the surrounding temperature is 100°C and at its top end, it is 500°C. Determine the temperature distribution in the block.

The block is schematically shown in Fig. 6.119. A steady-state (transient thermal) analysis is adopted. The problem will be solved using the main approach of GUI (graphic user interface). However, the command approach will also be given at the end of the solution procedure to illustrate the features of this methodology.

6.5.3 Solution stage

First, the analysis type must be defined. From the ANSYS Main Menu, select Solution → Analysis Type → New Analysis → Steady-State. The frame shown in Fig. 6.126 is created.

As always, the model must be constrained. For thermal problems, constraints can be in the form of temperature, heat flow, convection, heat flux, heat generation and radiation. In this particular example, all four sides of the block have fixed temperatures. Thus, from the ANSYS Main Menu, select Solution → Define Loads → Apply → Thermal → Temperature → On Nodes. The frame shown in Fig. 6.127 appears.

In the frame shown in Fig. 6.127, highlight the [A] Box button and draw a box around the nodes on the top line of the block (the surrounding temperature is 500°C). As a result of that action, the frame shown in Fig. 6.128 is generated.

Please note that the DOF to be constrained is [A] temperature (highlighted in Fig. 6.128), and [B] VALUE Load TEMP = 500°C should be entered (also shown in Fig. 6.128).

Using the same approach, constraints (temperature) to the remaining three sides should be applied, ensuring that VALUE Load TEMP = 100°C in all three cases.

The last step in the solution stage is to solve the problem. Therefore, from the ANSYS Main Menu, select Solution → Solve → Current LS.

This solved example will outline a simple analysis of coupled thermal/structural problem.

A steel link, with no internal stresses, is pinned between two solid columns at a reference temperature of 0°C (273 K), as shown in Fig. 6.130. One of the columns is heated to a temperature of 75°C (348 K). As heat is transferred from the column into the link, the link will attempt to expand. However, since it is pinned, this cannot occur and stress is therefore created in the link. A steady-state solution of the resulting stress will be arrived at to simplify the analysis.

Loads will not be applied to the link, only a temperature change from 0°C to 75°C. The link is made of steel with a modulus of elasticity of 210 GPa, a thermal conductivity of 60.5 W/m°K and a thermal expansion coefficient of 12 × 10^− 6/K.

6.7.4 Solution stage

Firstly, the analysis type needs to be defined. From the ANSYS Main Menu, select Solution → Analysis Type → New Analysis. In the generated frame, shown in Fig. 6.146, activate the [A] Static button.

After this, the thermal settings have to be recalled into the analysis. From the ANSYS Main Menu, select Solution → Physics → Environment → Read. In the generated frame shown in Fig. 6.147, select [A] Thermal and then click the [B] OK button.

As usual, constraints to the model must be applied. Therefore, from the ANSYS Main Menu, select Solution → Define Loads → Apply → Thermal → Temperature → On Keypoints. In the resulting frame (Fig. 6.148), set the temperature of keypoint 1 (the left-most point) to [A] 348 K and click the [B] OK button.

Finally, from the ANSYS Main Menu, select Solution → Solve → Current LS. It is important to close the currently used environment and enable other environments (structural) to be opened without contamination, otherwise error messages might appear.

The thermal part of the solution has now been obtained. If the steady-state temperature within the link is plotted, then it can be seen as being a uniform 384 K as expected. This information is saved in a file named Jobname.rth, where rth is the thermal results file. An appropriate name for the project should be used, as assigned at the beginning of the project. Since the jobname was not changed at the beginning of the analysis, this data can be found at file.rth and will be used in determining the structural effects.

From the ANSYS Main Menu, select Solution → Physics → Environment → Read. In the generated frame shown in Fig. 6.149, select [A] Structural and click the [B] OK button.

Next, from the ANSYS Main Menu, select Solution → Define Loads → Apply → Structural → Displacement → On Keypoints. Constrain keypoint 1 in all [A] DOF (see Fig. 6.150) and keypoint 2 in the [B] UX direction as shown in Fig. 6.151.

Stresses in the link are created by thermal expansion; therefore thermal effect must be recalled into the solution.

From the ANSYS Main Menu, select Solution → Define Loads → Apply → Structural → Temperature → From Therm Analy. In the resulting frame shown in Fig. 6.152, enter the file name (given to the project) [A] file.rth and click the [B] OK button. This couples the results from the solution of the thermal settings to the information defining the structural settings.

From the ANSYS Main Menu, select Preprocessor → Loads → Define Loads → Settings → Reference Temp. In the created frame (Fig. 6.153), the reference temperature is set to [A] 273 K; click the [B] OK button to implement the selection.

Finally, from the ANSYS Main Menu, select Solution → Solve → Current LS.

6.7.5 Postprocessing stage

In order to view the results, postprocessing has to be carried out. Since the link is modelled as a single line, the stress cannot be listed in the usual way. Instead, an element table must be created first.

From the ANSYS Main Menu, select General Postproc → Element Table → Define Table. In the resulting frame, select Add. A new frame then opens (see Fig. 6.154), in which the following entries should be made: [A] EQV strain = 0, [B] Lab. = CompStr. From the results data, select [C] by sequence num and [D] LS in the adjacent pull-down menu, and ensure that the entry [E] LS, 1 is made.

To list stress data from the ANSYS Main Menu, select General Postproc → Element Table → List Elem Table. In the resulting frame (Fig. 6.155), select [A] COMPSTR and click the [B] OK button.

Because of this action, a frame containing a list of compressive stresses in the link's elements is displayed (see Fig. 6.156). As expected, the stress of compressive nature in each element is − 189 MPa.