Dimensions in NX Sketches
Dimension Types
By clicking the dropdown arrow next to the dimensions button you can access several types of dimension. Usually, inferred dimension should serve your needs but if NX infers the wrong dimension type you may want to select one of the others.
Inferred Dimension: NX will guess at the appropriate dimension type based on the nature of the objects you select.
Horizontal/Vertical: Measures the distance horizontally/vertically between two points, two parallel lines or a point and a line. If you select an arc, it will snap to the center-point of the arc. This will be zero for intersecting features.
Parallel: Measures the straight line distance between two "points" on the sketch. If you select a line instead of a point but NX will snap to the nearest endpoint on the line. If you select an arc, it will snap to the center-point of the arc. This will be zero for intersecting features.
Perpendicular: Measures the distance from a line to a point along an imaginary line perpendicular to the sketch line. If you select two lines, NX will snap to the nearest endpoint of the second line you select. NX will not allow you to select two points or to select a curve. It will return zero for intersecting features.
Angular: Measures the angle between two straight lines. Note that you cannot use this to measure the angle covered by an arc. To do this you will need to create the appropriate tangent lines.
Diameter/Radius: Measures the diameter/radius of a single circle or circular arc.
Perimeter: Measures the sum of the lengths of the selected lines, arcs and other profiles. Note perimeter dimensions do not appear on your sketch! To view and change them you will have to go to the expression editor under the tools menu.
Dimension Modifiers
When you select the dimension button, a small menu like the one below will pop up. In order, they do the following:
- Dimension Dialog: Opens a small dialog on the screen that allows you to select the dimension type, define an expression for the dimension, change old expressions and change the appearance of the dimension.
- Reference Dimension: Selecting this mode creates a reference dimension. Much like a driven dimension in Solidworks, a reference dimension does not constrain the sketch.
- Alternate Angle: This option is only available in angular dimension mode. It simply flips which angle between the two lines is being measured.
Dimension Specification
Once you create a dimension, a small box like the one below will appear. This allows you to specify the name and value of the dimension in various ways.
Name: The first box is the name of the dimension. It is useful to name your dimensions if you will be referencing them in expressions.
Value: The value dropdown specifies the actual size of the dimension constraint in one of 5 ways.
- Measure: Defines the dimension in terms of another measurement in the sketch or on existing features. It seems like it would be better to do this with multiple dimensions and references.
- Formula: This is the most powerful dimensioning mode and the one you should probably use the most. It allows you to enter in a complete formula including references to other dimensions.
- Function: Provides an easy interface for defining a dimension in terms of a mathematical function. Once you enter the parameters, NX plugs the function into a formula. When you edit the dimension again, the formula dialog will appear.
- Reference: Sets this dimension equal to another dimension. To use, click on another feature in the sketch to see relevant dimension which can be referenced.
- Constant: This is the default mode in which you define the dimension as a numeric constant. Once you enter a different mode you may need to click "Make Constant" first in order to access the full list of modes.