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The analysis feature is a very powerful tool of Pro/ENGINEER that can be used in different ways to automate the design process. With the following example, I will explain how to use it effectively.
Consider the simple protrusion in Figure 1. Now consider Figure 2, where the top corner has been rounded. We know the height of the protrusion before applying round. But we have to measure it again after rounding because the height is not equal to total height minus the radius value. Since the design may change several times, it will be very time-consuming to measure the height repeatedly. Creating the analysis feature will do it for you.
Figure 1
Figure 2
Figure 3
1. Create a plane tangent to the round as shown in Figure 4.
Figure 4
2. Now click on the Analysis feature icon to invoke the dialog box. Note the name of feature and set Type to Measure (Figure 5).
Figure 5
3. Click Next. In the Measure dialog box, set the Type to Distance and measure the distance between dtm 1 and the base surface (Figure 6).
Figure 6
4. Pro/ENGINEER will automatically create a parameter and assign it the value of the measurement. Click Done and the feature will be completed. Make sure that Create option is set to Yes (Figure 7).
Figure 7
All the measurements taken by the analysis feature are regenerated as the model is regenerated, providing up-to-date information. We can display this useful information either as a note or as a separate column in the model tree.
But to do so, we have to write the following simple relation:
Dd=distance:fid_analysis1
Where:
analysis1 is the name of the analysis feature
distance is the parameter name created by it
dd is the name of the parameter the system will create to store the value of measurement taken by analysis feature.
Now we can use dd parameter for different purposes. Using the intermediate parameter ‘DD’ is not required for use in notes or relations. It may, however, be required to get the value shown in the model tree.
Relations can directly reference analysis features like this:
D5= distance:fid_analysis1
And Notes can directly reference analysis features like this:
&distance:fid_analysis1
Figure 8. Relations dialog box.
Now that we have created the dd parameter, we can display its value as a note. First create a note and in the text box write “&dd” (where & indicates that dd is a parameter). When we place the note instead of showing text “&dd”, it will display the value of the parameter
Figure 9
The note will appear as shown in Figure 10.
Figure 10
To add a column to model tree that displays the value of the parameter DD, go to Settings, Tree Columns. The dialog box shown in Figure 11 appears.
Figure 11
Change the Type to Model Params and add DD to the Displayed box. Click OK and the DD parameter will display in the column tree (Figure 12).
Figure 12
Suppose we want the radius of the above protrusion to change such as to limit the height within the range (135 to 135.05). To accomplish this, write the following relations:
IF DD<135
d6=D6-.05
ENDIF
IF DD>135.05
d6=D6+.05
ENDIF
Here D6 is the dimension symbol for radius, and DD is the total height of the protrusion after applying the round.
Figure 13
Pro/ENGINEER always evaluates parameters and relations at the start of regeneration. We therefore have to regenerate the model several times to get exact results. Otherwise, the system will display the following error message:
This happens because the analysis feature measures the correct value after regeneration, but the relation has been evaluated before regeneration. 
Asim Rashid is a Design Engineer at Wahid Industries Limited in Gujrat, Pakistan. He can be reached by email at aaasimm@hotmail.com.
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