This section describes how to perform a simple thermal analysis, using a 1D table to apply loads. This problem is shown twice, once done via commands, and then done interactively using the GUI.
Text preceded by an exclamation mark (!) is comment text.
/batch,list /show /title, Demonstration of position-varying film coefficient using Tabular BC's. /com /com * ------------------------------------------------------------------ /com * Table Support of boundary conditions /com * /com * Boundary Condition Type Primary Variables Independent Parameters /com * ----------------------- ----------------- ---------------------- /com * Convection:Film Coefficient X - /com * /com * Problem description /com * /com * A static Heat Transfer problem. A 2 x 1 rectangular plate is /com * subjected to temperature constraint at one of its end, while the /com * remaining perimeter of the plate is subjected to a convection boundary /com * condition. The film coefficient is a function of X-position and is described /com * by a parametric table 'cnvtab'. /com ** *dim,cnvtab,table,5,,,x ! table definition. cnvtab(1,0) = 0.0,0.50,1.0,1.50,2.0 ! Variable name, Var1 = 'X' cnvtab(1,1) = 20.0,30.0,50.0,80.0,120.0 /prep7 esize,0.5 et,1,55 rect,0,2,0,1 amesh,1 MP,KXX,,1.0 MP,DENS,,10.0 MP,C,,100.0 lsel,s,loc,x,0 dl,all,,temp,100 alls lsel,u,loc,x,0 nsll,s,1 sf,all,conv,%cnvtab%,20 alls /psf,conv,hcoef,2 ! show convection bc. /pnum,tabn,on ! show table names nplot fini /solu anty,static kbc,1 nsubst,1 time,60 tunif,50 outres,all,all solve finish /post1 set,last sflist,all ! Numerical values of convection bc's /pnum,tabn,off ! turn off table name /psf,conv,hcoef,2 ! show convection bc. /pnum,sval,1 ! show numerical values of table bc's eplot! convection at t=60 sec. plns,temp fini
The same problem is shown here using interactive menu selections on the GUI.
Step 1: Define a 1D table
Choose . The Array Parameters dialog box appears. Click Add...
The Add New Array Parameter dialog box appears. Type cnvtab in the "Parameter name" field.
Select "Table" for Parameter type.
Enter 5,1,1 as I,J,K values
Enter X as row variable.
Click OK.
In the Array Parameters dialog box, make sure cnvtab is highlighted and click Edit. The Table Array:CNVTAB=f(X) table editor dialog box appears. (See Tabular Input via Table Array Parameters in the Ansys Parametric Design Language Guide for details about table arrays.)
Two columns appear in the table editor dialog box. The first column is column 0; the second column is column 1. Column 0 contains six boxes. Do not do anything in the first (top) box. In the five other boxes, type 0.0, 0.5, 1.0, 1.5, and 2.0. These are row index values.
Column 1 also contains six boxes. You do not have to enter anything in the blue (top) box, because this table is one-dimensional. In the other five boxes, type 20, 30, 50, 80, and 120.
Choose .
Close the Array Parameters dialog box.
Step 2: Define your element type and material properties
Choose . The Element Types dialog box appears. Click Add.
The Library of Element Types dialog box appears. Select Thermal Solid from the list on the left, and select Quad 4node 55 from the list on the right.
Click OK.
Close the Element Types dialog box.
Choose . The Define Material Model Behavior dialog box appears.
In the Material Models Available window, double-click the following options: Thermal, Density. A dialog box appears.
Enter 10.0 for DENS (density). Click OK. Material Model Number 1 appears in the Material Models Defined window on the left.
In the Material Models Available window, double-click the following options: Conductivity, Isotropic. A dialog box appears.
Enter 1.0 for KXX (Thermal conductivity). Click OK.
In the Material Models Available window, double-click Specific Heat. A dialog box appears.
Enter 100.0 for C (Specific Heat). Click OK.
Choose menu path to remove the Define Material Model Behavior dialog box.
Step 3: Build and mesh your model
Choose . The Create Rectangle by Dimensions dialog box appears.
Enter 0, 2 for X1,X2 coordinates.
Enter 0, 1 for Y1, Y2 coordinates.
Click OK. A rectangular area appears on the screen.
Choose .
Under the Size Controls section of the Mesh Tool, click Globl,Set. The Global Element Sizes dialog box appears.
Set the "Element endge length" field to 0.5 and click OK.
In the Mesh area of the Mesh Tool, choose Areas and Map and verify that Quad and 3/4 sided are selected.
Click MESH. The Mesh Areas picking menu appears.
Click Pick All. The mesh appears in the Graphics window.
Close the MeshTool dialog box.
Click SAVE_DB on the Mechanical APDL Toolbar.
Step 4: Apply Tabular Boundary Conditions
Choose .
Choose . The Apply TEMP on Lines picking menu appears.
In the Graphics window, select the vertical line at x=0 (on the far left of the model). Click OK.
The Apply TEMP on lines dialog box appears.
Enter 100 for VALUE. Click OK.
Choose . The Apply CONV on Lines picking menu appears.
In the Graphics window, select all lines except the line at x = 0.
Click OK. The Apply CONV on lines dialog box appears.
In the drop-down selection box for "Apply Film Coef on lines," select "Existing table."
Remove any value in the VALI field.
Enter 20 in the "VAL2I Bulk temperature" field. Click OK.
A second Apply CONV on lines dialog box appears. Verify that the selection box for "Existing table" shows CNVTAB. Click OK. The Graphics Window displays arrows on all lines except the line at x = 0.
Choose . The Uniform Temperature dialog box appears.
Enter 50 as the uniform temperature. Click OK.
Step 5: Show the applied loads to verify
Choose . The Symbols dialog box appears.
Select "Convect FilmCoef" in the "Surface Load Symbols" drop-down selection box.
Select "Arrows" in the "Show pres and convect as" drop-down selection box.
Click OK.
Choose . The Plot Numbering Controls dialog box appears.
Click Table Names on. Click OK. The table name CNVTAB appears on the arrows on the right side of the Graphics window.
Click SAVE_DB on the Mechanical APDL Toolbar.
Step 6: Set Analysis Options and Solve
Choose . The New Analysis dialog box appears.
Verify that "Steady-State" is selected and click OK.
Choose . The Time and Substep Options dialog box appears.
Enter 60 as "Time at end of load step."
Enter 1 as "Number of substeps."
Choose Stepped. Click OK.
Choose . The Controls for Database and Results File Writing dialog appears. Verify that the "Item to be controlled" field shows "All items."
Select "Every substep" for "File write frequency" field. Click OK.
Choose . Review the /STATUS Command dialog box. If OK, click Close.
In the Solve Current Load Step dialog box, click OK to begin the solve. When the solution is done, click Close in the "Solution is done!" information box.
Step 7: Postprocess
Choose .
Choose . The SFLIST Command dialog box appears. Review the results and click Close.
Choose . The Plot Numbering Controls dialog box appears.
Click Table Names display off.
Click Numeric contour values on. Click OK.
Choose . The Symbols dialog box appears.
In the "Surface Load Symbols" drop-down selection box, select "Convect FilmCoef."
In the "Show pres and convect as" drop-down selection box, select "Arrows." Click OK.
Choose . Observe the numbers over the arrows on the model.
Choose . The Contour Nodal Solution Data dialog box appears.
Verify that DOF Solution is selected in the list on the left, and Temperature is selected in the list on the right. Click OK. Observe the resulting display.
Step 8: Finish
You are now finished with this sample problem. Click in the Mechanical APDL Toolbar. Choose a save option and click .