Pro/ENGINEER - Defining Relations

In this mini-tutorial, we will 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. In the first relation, 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.

Adding relations

Simple relations can be added a couple of ways. One way is to create them one at a time with the add command:

Choose part>relations>add
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.

Other relations menu options

When you first enter the relations menu, you are given an option to choose features to show the variable names (rather than the value) of the dimensional constraints. If you would like to switch the display of the dimensional constraints between variable names and values, choose switch dim.
Add param allows you to create and set the value for parameter variables without entering a relation equation. The disadvantage to this approach is that the parameter is not accessible in the relations table. I would discourage you from using this method. The only way to modify such a parameter is to delete it using del param and re-entering it.

Setting the relations table editor

The relations table editor is set, by default, to the default editor for the computer OS. On NTs, the default editor is typically Notepad. This will be adequate for most users. If you want a more spreadsheet type environment or are working under Unix, you may want to set the editor to the internal Pro/E editor, Pro/Table. You would do this by editing (or creating) your config.pro file in the directory where you start Pro/E to include the line:

relation_file_editor    protab

Changing variable names

If you would like to have more meaningful names for dimensional constraints, you can change them with part>modify>dim cosmetics>symbol. This modify option, rather than changing the value of the variable, changes its name. This new name is what you would use in the relations. If you have already used the old name of the variable in a relation, it will automatically be changed. If the variable name you have entered is already in use, you will be prompted to enter a different name.

Entering relations in an assembly

Relations can also be set up between parts in an assembly. These relations would be defined in assembly, rather than part, mode using an identical relations menu. The main difference between part and assembly level relations is that assembly level relations have to indicate which part a variable belongs to. Each assembly component (e.g., a part) is assigned an ID number when it is brought in, usually even numbers starting with 0. You can see what number has been assigned to a part by going to the relations menu and selecting a feature on a part. You might see a dimensional constraint variable appear which looks like:
d1:4
The d1 is the dimensional constraint assigned when the part was created in part mode. This will stay the same no matter what assembly the part is brought into. The 4 is the component ID assigned inassembly mode. This number will vary with what assembly the part is brought into or may vary due to modifications in the assembly. Always confirm this number before writing relations.
If you went back and modified the dimension name (symbol) in part mode to len, then the dimensional constraint would appear as len:4 in the assembly mode. All part level relations and parameters are inherited by the assembly and will hold true in the assembly. Parameters can also be declared in assembly mode. These will not need a component ID after them.
The assembly-level relations table will have additional comment lines, called the coding table, added to the beginning of the file. After entering one or more relations, lines are added which list both thecomponent ID of parts referenced in the relations and the file name of the component.

Example relations table file

An assembly-level relations table file might look something like:

/* CODING TABLE CODING SYMBOL  MODEL NAME
/* CODING TABLE  0    BASE.PRT
/* CODING TABLE  2    PIN.PRT
/* CODING TABLE  4    SLEEVE.PRT
/* CODING TABLE

/* general tolerance
TOL = .002

/* fit sleeve outer dia to base counterbore
D5:4 = D3:0 - TOL

/* fit pin length to sleeve outer dia
D10:2 = D5:4 + .5

Notice that:

Comments were added to each relation. This makes it much easier for you (or someone else) to debug it at some later time.
An assembly-level parameter, TOL, was declared.
The dimensional constraint for the outer dia of the sleeve, D5:4, was used both on the left side of one relation and the right side of another. The relations are processed in order and the relation with D5:4 on the left (driven variable) should always appear first in the relations table.
All of the variables are in upper-case. To the best of my knowledge, Pro/E is not case-sensitive for naming variables. If you enter them in lower-case, the next time the relations table is open, they'll be in upper case.