pro-e engineering 5.0 relations

can anyone please suggest me with using of relations in pro-e 5.0

Here is the solution for you. lets look at various ways of defining relations for constraint dimensions. To some degree, the design intent of a part or assembly can be embedded via the definition of features in a part and/or the constraining parts in an assembly (i.e., mating or aligning). Other design intentions, however, have to be embedded via relations. Relations are one or more parametric equations which either assign a constant to a variable or define a relationship between two or more variables. The relations are stored in a separate relations table. The variables can either be defined on the fly or represent dimensional constraints in the part/assembly.
For example,the dimension, d1, is assigned a constant, 76.:
d1 = 76
In this next relation, d2 is always 5 more than d3.
d2 = d3 + 5
In this next relation, d4 is always half of d5.
d4 = d5 / 2
It is important to note that trigonometric functions can also be used:
d7 = d8 * sin(d9)
In all of these equations the variables and/or constants on the right hand side of the equation determine the value of the variable on the left. Another way of representing this:
driven = driver
Driven dimensional constraints cannot be manipulated directly using commands such as modify. They have to set indirectly through the driver dimensional constraints or the constants defined in the relations table.
New variables, defined on the fly and not representing a dimensional constraint, are called parameters. For example:
drain = 20
vol = d3 * d2* d8 - drain
Both vol and drain are parameters. The drain parameter cannot be used on the right side of an equation until it has been defined on the left.

Simple relations can be added a couple of ways. One way is to create them one at a time with the add command:
• Enter the relation (e.g., d1 = d2 + 3) in the command window
• Enter another relation or hit enter again to stop entering relations
• Regenerate the part/assembly to make sure it behaves as expected
Editing relations
If you need to modify a relation or are going to enter numerous relations it is usually better to use edit relations:
• Choose part>relations>edit rel
• You will go into a text editor (more on this later). If you have already entered relations, you will see them, one per line, in the order you entered them.
• Edit/add/delete relations, one per line, as needed. Comments (text that won't be evaluated) can be added by beginning the line with a /*.
• Save changes under the file menu of the editor
• Exit from the editor
• If you have made an error in editing (i.e., illegal characters, undefined variables, etc.), you will be asked on the command line if you want to re-edit your file. Enter yes.
• Regenerate the part/assembly to make sure it behaves as expected
Showing the relations table
If you just want to see the relations associated with the part or assembly, choose part>relations>show rel. Click in the window showing the relations to activate the window. Press the space bar to scroll the relations and press q to quit. This can also be useful in debugging your relations since it also shows the current values for each driven variable.