- slide 1 of 2
Pro engineer is highly parametric software, means if you edit any dimension to see the change in the model. Due to the parametric nature of pro engineer, relations could be added between different dimensions and parameters. Relations are basically some user written equations. Relations help modification of different dimensions and parameters in a predetermined proportion.
The relations equations may be some sort of simple equation or may be some comparison statement.
You can even use simultaneous equations and logical statement as part of relations.
Operators used in relations: The operators (and their purpose shown between parenthesis) you can use in pro engineer relations are as below:
+ (addition), - (subtraction), *(multiplication), ^ (exponentiation),/ (division),()(parenthesis).
= (equal to)
When a TRUE/FALSE kind of value is expected from a statement, then comparison operator is used. For example, if you want to know whether d32 is less than d33 or not, you can use the statement like below:
If d32<= d33
Functions used in relations: Apart from almost all mathematical and trigonometric functions, you can use graph evaluation function for controlling dimension through a graph.
How to add relation in pro engineer model: For adding relations, please follow tools>relations and you will get relation dialogue box. You have to type the relation in the box. For writing relations between different dimensions, you need to find the dimensions names instead of dimensions text. So you will click info>switch dimensions to toggle the dimensions text to dimensions names.
Example: Suppose in a cylinder the diameter is represented by d32 and height by d33, then the simplest for of relation may be d32=d33, by doing so whenever you will change diameter height also will be changed to become equal with diameter. In this case of relation d33 is called driving dimension and d32 is called driven dimension. You cannot change driven dimension manually (like normal editing).
After adding a relation in relation dialog box you can check the correctness of the relation by clicking utilities>verify of relation dialog box.
- slide 2 of 2
Parameters are useful to provide information about the pro engineer model/assembly. Some of the parameters are system generated parameters and some are user defined parameters. We will discuss here about user defined parameters.
Lets take an example, Suppose you are modeling a plastic glass using pro engineer, you can add an additional user defined parameter like color , now after adding the parameter color, you can a create family table for different colored glasses. Going further by using relation you can vary the size of the glasses for different colors.
Click on tools>parameters to open parameter dialog box and then go to parameters>add parameters to add user defined parameters. It will add one more row to the parameter dialog box, you have to rename the parameter, define the type, value and access of the parameter.
How to use parameters in family table?
Go to tools>family table and then add a new column (item), it will open the item selection dialog box, there click on parameter and it will direct you to the parameter dialog box there you need to select the required parameter. Now the value of the parameter could be set from family table.
How to use parameters in relations?
As you already know how to create parameter and relation, so let’s answer this question win an example. Suppose you have a cylinder, whose diameter is represented by d45 and height by d46. Now if you want that the dimension d46 should be controlled by a user defined parameter say, DIA, then you have to follow the below mentioned steps:
- Create a parameter DIA.
- Put some value of the parameter (DIA), say, 15.
- Add a relation, d46=DIA
- Remember to regenerate to see the change.