6.0

Applying Dimension Constraints | 97
Mechanical Desktop recalculates the sketch and displays the constraints.
■ A fix constraint is added to the start point of the first line of the sketch.
This point is anchored and will not move when changes are made to the
sketch constraints.
■ Nearly horizontal and vertical lines have been assigned horizontal (H) and
vertical (V) constraints.
■ Nearly vertical lines are assumed to be parallel (P) to one another.
For this exercise, all of the assumed geometric constraints are correct and
none of them restrict the dimensioning scheme shown earlier.
Exit from Show Constraints, responding to the prompt as follows:
Enter an option [All/Select/Next/eXit] <eXit>: Press
ENTER
Adding Dimensions
The rough sketch is converted to a profile sketch, and default geometric
constraints are applied. Now you need to fully constrain the sketch by adding
four dimensions and two geometric constraints. Parts are resized as you
change parametric dimensions to refine your design, while all geometric
relationships are maintained.
Keep the following points in mind as you are adding dimensions:
■ Select the elements to dimension and choose where to place the dimension.
■ Dimension type depends on the element you choose and where you place
the dimension. The current size of the selected element is shown.
■ You can accept the calculated size or specify a new value.
■ The sketch element is resized according to the dimension value and the
dimension is placed at the location you chose.
It is good practice to accept the automatically calculated dimensions to
stabilize the sketch shape, particularly large outer dimensions. When you
later modify dimensions to exact sizes, the sketch shape is less likely to
become distorted.
In this exercise, you create horizontal and vertical dimensions. Then you
modify the sketch by appending geometry, and applying angular and radial
dimensions.