Product help with community knowledge

Page statistics

0 views0 edit(s)0 characters(s) Page last modified 13:58, 14 Nov 2012 by AstroJohnPE

Water-Cooled Wall with Radiation, Convection, and Temperature

Version as of 13:23, 25 May 2013

to this version.

View current version

Given: The cross-section of a water-cooled, refractory wall in a furnace is subjected to the conditions shown in the following figure. Assume that the cold face (outside face of the wall) remains at 125°F and the inside face is subjected to 1200°F heat of the furnace.

Find: The heat gained by the water per foot of pipe.

Problem Geometry

Material Wall (Part1) Refractory (Part 2) Pipe (Part 3)

Conductivity (BTU/s in °F)

6.254E-4

1.1E-5

6.254E-4

Table 1: Material Properties

This example only covers setting up and performing the analysis. For instructions on building the model, see Water-Cooled Wall with Radiation, Convection and Temperature Model. If you have not built the model, you can open the wcwall_input.ach file in the Models subfolder of the Autodesk Simulation installation directory.

Assume that each cross section is identical. Due to symmetry, only the cross-section around a single pipe is modeled, as shown in the following figure.

1. The assumed wall temperature can be fixed with controlled temperatures, but first estimate what stiffness is appropriate for the controlled temperatures (and then confirm the results after the analysis). Generally, the stiffness is two to three orders of magnitude (100 to 1000 times) higher than the conductivity of the material to which they are attached. Therefore, a stiffness of 0.625 is acceptable.
2. Select the nodes on the outside of the wall using Selection Shape Rectangle. Draw a rectangle that encloses the nodes at the bottom of the wall (on the -Z side of the model).
3. Right-click in the display area and select Add Nodal Controlled Temperatures.
4. In the Magnitude field, type 125 and 0.625 in the Stiffness field and click OK. The controlled temperature symbol (T) appears on all the selected nodes. It keeps these nodes at 125°F.
5. Set the element type. In the tree view, click the heading for Part 1. Hold down the Ctrl key and click the heading for Part 2. Right-click the headings and select Edit Element Type 2-D.
6. With the headings still selected, right-click and select Edit Element Definition. Although the thickness of the part has no affect on the temperature distribution, it does affect the surface area and the total heat flow. Type 12 in the Thickness field. Click OK.
7. In the tree view, right-click the heading for Part 3 and select Edit Element Type 2-D. With the heading still selected, right-click and select Edit Element Definition. Type 12 in the Thickness field. To sum the heat flow through the inside face, select the Linear Based on BC option in the Heat Flow Calculation drop-down menu. It forces the heat flow output to be based on the convection boundary conditions instead of based on the temperature distribution in the elements. Click OK.
8. Set the material properties. In the tree view, click the heading for Part 1. Holding down the <Ctrl> key, click the heading for Part 3. right-click a heading and select Edit Material. Click the Edit Properties. Type 6.254e-4 in the Thermal conductivity field. The other values are not needed for steady-state analysis. click the OK twice.
9. Right-click the heading for Part 2 and select Edit Material. Click the Edit Properties. Type 1.1e-5 in the Thermal conductivity field. The other values are not needed for steady-state analysis. Click OK twice.
10. Add the radiation load on the inside face of the wall. Using Selection Shape Point or Rectangle and Selection Select Surfaces, click the surface of part 2 on the inside of the wall (on the +Z side of the model). Right-click in the display area and select Add Surface Radiation Load. Type 1200 in the Temperature field and type 0.7 in the Function field. click the OK.
11. Add the water cooling inside the pipe. Click to select the inner surface of the hole, right-click in the display area and select Add Surface Convection Load. Type 0.0012 in the Temperature Independent Convection Coefficient field and type 70 in the Temperature field click OK.
12. Right-click the Analysis Type heading in the tree view and select Edit Analysis Parameters.
13. Click the Options tab and type 1190 in the Default nodal temperature field. Although it is strictly not necessary in this model, we can guess that the hot face is around this temperature. By specifying an initial temperature, we will speed up the iterative process when radiation is included in the analysis. (A warning message says that the temperature value seems high. Click OK to close it).
14. Because a nonlinear effect is included in the analysis (radiation), the iteration controls must be set. Click the Advanced tab and perform the following steps:
1. Activate the Perform check box.
2. Select the Stop when corrective norm < E1 (case 1) option in the Criteria drop-down box.  It indicates that the solution has converged when the average temperature change at a node is smaller than the corrective tolerance. (Note: Other models require a difference convergence criteria.)
3. Type 20 in the Maximum number of iterations field. After the analysis is completed, check that the analysis did converge within 20 iterations.
4. Type 0.01 in the Corrective tolerance field. When the average temperature difference from one iteration to the next is less than this value, the solution is converged.
5. Type 0.95 in the Relaxation parameter field. (Any value around 0.5 to 1 works for this model. If the model is slow to converge, try a different value.)
15. Click OK to accept the input.
16. Select Analysis Analysis Run Simulation to perform the analysis.
17. When the analysis completes, the model is loaded in the Results environment. First we must go to the Report environment to verify that the solution has converged. Use Tools Environments Report. Click the Summary heading. Scroll near the bottom of the file and search for the text CONVERGED SOLUTION OBTAINED. It occurs on nonlinear iteration number 5. Thus, the model converged within the 20 iterations specified.