This section describes how to use the menus on the ANSYS GUI to perform the same steady-state thermal analysis described in Example of a Steady-State Thermal Analysis (Command or Batch Method). In this version of the sample analysis, instead of issuing commands, you select options from the GUI menus.
After you have started the ANSYS program and have entered the GUI, you need to begin the analysis by assigning a title to it. To do so, perform these tasks:
Choose . The Change Title dialog box appears.
Enter the text Steady-state thermal analysis of pipe junction.
Click on OK.
You need to specify units of measurement for the analysis. For this pipe junction example, measurements use the U. S. Customary system of units (based on inches). To specify this, type the command /UNITS,BIN in the ANSYS Input window and press ENTER.
The example analysis uses a thermal solid element. To define it, do the following:
Choose . The Element Types dialog box appears.
Click on Add. The Library of Element Types dialog box appears.
In the list on the left, scroll down and pick (highlight) "Thermal Solid." In the list on the right, pick "Brick20node 90."
Click on OK.
Click on Close to close the Element Types dialog box.
To define material properties for the analysis, perform these steps:
Choose . The Define Material Model Behavior dialog box appears.
In the Material Models Available window, double-click on the following options: Thermal, Density. A dialog box appears.
Enter .285 for DENS (Density), and click on OK. Material Model Number 1 appears in the Material Models Defined window on the left.
In the Material Models Available window, double-click on the following options: Conductivity, Isotropic. A dialog box appears.
Click on the Add Temperature button four times. Four columns are added.
In the T1 through T5 fields, enter the following temperature values: 70, 200, 300, 400, and 500. Select the row of temperatures by dragging the cursor across the text fields. Then copy the temperatures by pressing Ctrl+C.
In the KXX (Thermal Conductivity) fields, enter the following values, in order, for each of the temperatures, then click on OK. Note that to keep the units consistent, each of the given values of KXX must be divided by 12. You can just input the fractions and have ANSYS perform the calculations.
8.35/12 8.90/12 9.35/12 9.80/12 10.23/12
In the Material Models Available window, double-click on Specific Heat. A dialog box appears.
Click on the Add Temperature button four times. Four columns are added.
With the cursor positioned in the T1 field, paste the five temperatures by pressing Ctrl+V.
In the C (Specific Heat) fields, enter the following values, in order, for each of the temperatures, then click on OK.
.113 .117 .119 .122 .125
Choose menu path , then enter 2 for the new Material ID. Click on OK. Material Model Number 2 appears in the Material Models Defined window on the left.
In the Material Models Available window, double-click on Convection or Film Coef. A dialog box appears.
Click on the Add Temperature button four times. Four columns are added.
With the cursor positioned in the T1 field, paste the five temperatures by pressing Ctrl+V.
In the HF (Film Coefficient) fields, enter the following values, in order, for each of the temperatures. To keep the units consistent, each value of HF must be divided by 144. As in step 7, you can input the data as fractions and let ANSYS perform the calculations.
426/144 405/144 352/144 275/144 221/144
Click on the Graph button to view a graph of Film Coefficients vs. temperature, then click on OK.
Choose menu path to remove the Define Material Model Behavior dialog box.
Click on SAVE_DB on the ANSYS Toolbar.
Choose . The Scalar Parameters window appears.
In the window's Selection field, enter the values shown below. (Do not enter the text in parentheses.) Press ENTER after typing in each value. If you make a mistake, simply retype the line containing the error.
RI1=1.3 (Inside radius of the cylindrical tank) RO1=1.5 (Outside radius of the tank) Z1=2 (Length of the tank) RI2=.4 (Inside radius of the pipe) RO2=.5 (Outside radius of the pipe) Z2=2 (Length of the pipe)
Click on Close to close the window.
Choose . The Create Cylinder by Dimensions dialog box appears.
Set the "Outer radius" field to RO1, the "Optional inner radius" field to RI1, the "Z coordinates" fields to 0 and Z1 respectively, and the "Ending angle" field to 90.
Click on OK.
Choose . The Offset WP dialog box appears.
Set the "XY, YZ, ZX Angles" field to 0,-90.
Click on OK.
Choose . The Create Cylinder by Dimensions dialog box appears.
Set the "Outer radius" field to RO2, the "Optional inner radius" field to RI2, the "Z coordinates" fields to 0 and Z2 respectively. Set the "Starting angle" field to -90 and the "Ending Angle" to 0.
Click on OK.
Choose .
Choose . The Overlap Volumes picking menu appears.
Click on Pick All.
Before you continue with the analysis, quickly review your model. To do so, follow these steps:
Choose . The Plot Numbering Controls dialog box appears.
Click the Volume numbers radio button to On, then click on OK.
Choose . A dialog box appears.
Set the "Coords of view point" fields to (-3,-1,1), then click on OK.
Review the resulting model.
Click on SAVE_DB on the ANSYS Toolbar.
In this step, delete the overlapping edges of the tank and the lower portion of the pipe.
Choose . The Delete Volume and Below picking menu appears.
In the picking menu, type 3,4 and press the ENTER key. Then click on OK in the Delete Volume and Below picking menu.
In this step, you select the areas at the remote Y and Z edges of the tank and save them as a component called AREMOTE. To do so, perform these tasks:
Choose . The Select Entities dialog box appears.
In the top drop down menu, select Areas. In the second drop down menu, select By Location. Click on the Z Coordinates radio button.
Set the "Min,Max" field to Z1.
Click on Apply.
Click on the Y Coordinates and Also Sele radio buttons.
Set the "Min,Max" field to 0.
Click on OK.
Choose . The Create Component dialog box appears.
Set the "Component name" field to AREMOTE. In the "Component is made of" menu, select Areas.
Click on OK.
Do the following:
Choose . The Plot Numbering Controls dialog box appears.
Click the Area and Line number radio boxes to On and click on OK.
Choose .
Choose .
Set "Erase between Plots" radio button to Off.
Choose .
Choose .
Set "Erase between Plots" radio button to On.
In this step, you concatenate areas and lines at the remote edges of the tank for mapped meshing. To do so, follow these steps:
Choose . The Concatenate Areas picking menu appears.
Click on Pick All.
Choose . A picking menu appears.
Pick (click on) lines 12 and 7 (or enter in the picker).
Click on Apply.
Pick lines 10 and 5 (or enter in picker).
Click on OK.
Choose . The Element Size on Picked Lines picking menu appears.
Pick lines 6 and 20 (or enter in the picker) .
Click on OK. The Element Sizes on Picked Lines dialog box appears.
Set the "No. of element divisions" field to 4.
Click on OK.
Choose . A picking menu appears.
Pick line 40 (or enter in the picker).
Click on OK. The Element Sizes on Picked Lines dialog box appears.
Set the "No. of element divisions" field to 6.
Click on OK.
In this sequence of steps, you set the global element size, set mapped meshing, then mesh the volumes.
Choose .
Choose . The Global Element Sizes dialog box appears.
Set the "Element edge length" field to 0.4 and click on OK.
Choose . The Mesher Options dialog box appears.
Set the Mesher Type radio button to Mapped and click on OK. The Set Element Shape dialog box appears.
In the 2-D shape key drop down menu, select Quad and click on OK.
Click on the SAVE_DB button on the Toolbar.
Choose . The Mesh Volumes picking menu appears. Click on Pick All. In the Graphics window, ANSYS builds the meshed model. If a shape testing warning message appears, review it and click Close.
Choose . The Plot Numbering Controls dialog box appears.
Set the Line, Area, and Volume numbering radio buttons to Off.
Click on OK.
In this step, you tell ANSYS that you want a steady-state solution that uses a program-chosen Newton-Raphson option.
Choose . The New Analysis dialog box appears.
Click on OK to choose the default analysis type (Steady-state).
Choose . The Static or Steady-State dialog box appears.
Click on OK to accept the default (“Program-chosen”) for "Newton-Raphson option."
In a thermal analysis, set a starting temperature.
Choose . A dialog box appears.
Enter 450 for "Uniform temperature." Click on OK.
This step applies convection loads to the nodes on the inner surface of the tank.
Choose .
Choose . The Select Entities dialog box appears.
Select Nodes and By Location, and click on the X Coordinates and From Full radio buttons.
Set the "Min,Max" field to RI1 and click on OK.
Choose . The Apply CONV on Nodes picking menu appears.
Click on Pick All. The Apply CONV on Nodes dialog box appears.
Set the "Film coefficient" field to 250/144.
Set the "Bulk temperature" field to 450.
Click on OK.
Choose . A dialog box appears.
Click on OK to select component AREMOTE.
Choose . The Select Entities dialog box appears.
Select Nodes and Attached To, and click on the Areas,All radio button. Click on OK.
Choose . The Apply TEMP on Nodes picking menu appears.
Click on Pick All. A dialog box appears.
Set the "Load TEMP value" field to 450.
Click on OK.
Click on SAVE_DB on the ANSYS Toolbar.
In this step, apply a temperature-dependent convection load on the inner surface of the pipe.
Choose . A dialog box appears.
Set the "XY,YZ,ZX Angles" field to 0,-90, then click on OK.
Choose . The Create Local CS at WP Origin dialog box appears.
On the "Type of coordinate system" menu, select "Cylindrical 1" and click on OK.
Choose . The Select Entities dialog box appears.
Select Nodes, and By Location, and click on the X Coordinates radio button.
Set the "Min,Max" field to RI2.
Click on OK.
Choose . The Apply CONV on Nodes picking menu appears.
Click on Pick All. A dialog box appears.
Set the "Film coefficient" field to -2.
Set the "Bulk temperature" field to 100.
Click on OK.
Choose .
Choose . The Symbols dialog box appears.
On the "Show pres and convect as" menu, select Arrows, then click on OK.
Choose . The display in the Graphics Window changes to show you a plot of nodes.
To reset the working plane and default Cartesian coordinate system, choose .
Choose .
For this example analysis, you need to specify 50 substeps with automatic time stepping.
Choose . The Time and Substep Options dialog box appears.
Set the "Number of substeps" field to 50.
Set "Automatic time stepping" radio button to On.
Click on OK.
Choose . The ANSYS program displays a summary of the solution options in a /STAT command window.
Review the summary.
Choose Close to close the /STAT command window.
Click on OK in the Solve Current Load Step dialog box.
Click Yes in the Verify message window.
The solution runs. When the Solution is done! window appears, click on Close.
Choose . The Edge Options dialog box appears.
Set the "Element outlines" field to "Edge only" for contour plots and click on OK.
Choose . The Contour Nodal Solution Data dialog box appears.
For "Item to be contoured," pick "DOF solution" from the list on the left, then pick "Temperature TEMP" from the list on the right.
Click on OK. The Graphics window displays a contour plot of the temperature results.
In this step, you plot the thermal flux vectors at the intersection of the pipe and tank.
Choose . A dialog box appears.
Set the "Coordinate system number" field to 11.
Click on OK.
Choose . The Select Entities dialog box appears.
Select Nodes and By Location, and click the X Coordinates radio button.
Set the "Min,Max" field to RO2.
Click on Apply.
Select Elements and Attached To, and click the Nodes radio button.
Click on Apply.
Select Nodes and Attached To, then click on OK.
Choose . A dialog box appears.
For "Vector item to be plotted," choose "Flux & gradient" from the list on the left and choose "Thermal flux TF" from the list on the right.
Click on OK. The Graphics Window displays a plot of thermal flux vectors.
To leave the ANSYS program, click on the QUIT button in the Toolbar. Choose an exit option and click on OK.