4.1.1.2 Simple sketch

Sketch

Create a new Sketch with the YZ-Plane as drawing plane and confirm with OK.

You should draw an L-Profile. You automatically entered the mode for drawing lines when entering sketch mode. Your NX screen should look like the one on the right. If not, click on profile  (figure "Drawing lines").

Draw an L, like displayed in the picture on the right. (figure "L created")

Sketch mode allows you to place points (e.g. endpoints of lines, midpoints of circles) directly by entering values.

Constraints

Your Drawing now has to be positioned respectively to the coordinate system. Click  to define Constraints.

Click Collinear . Select the lower horizontal line of the L, and as the second element the horizontal axis of the coordinate system.

The lower horizontal line of the L will now be aligned with the horizontal axis of the coordinate system. Do the same steps again to align the vertical line of the L. (figure "L aligned")

Highlight both short sides of the L. By clicking Equal Length they are adjusted to the same length.

The following constraints are used in this CAD course:

Icon	Name	Function
	Coincident	Connects two points to each other.
	Equal Radius	Equal radius for arcs or circles.
	Cocentric	Cocentric circles / arcs (same midpoint).
	Tangent	Adjusts lines/curves to be tangent to an arc/circle.
	Parallel	Parallel constraint for axes, lines, etc.
	Perpendicular	Adjusts two elements perpendicular.
	Equal Length	Equal length for lines
	Collinear	Parallel with distance = 0
	Horizontal	Alignes a line horizontally
	Vertical	Alignes a line vertically
	Point on Curve	An endpoint can be placed on a line or arc.
	Horizontal Alignment	Alignes two (or more) points horizontally
	Vertical Alignment	Alignes two (or more) points vertically

Furthermore the following list of geometric constraints exists in NX and can be used if needed (click for the list):

Icon	Name	Function
	Fixed	Constrains one or more curves to be fixed in position.
	Fully Fixed	Constrains one or more curves to be fixed in position AND orientation.
	Constant Angle	Constrains one ore more lines to be at a constant angle.
	Constant Length	Constrains one or more lines to have constant lenghts.
	Point on String	Constrains a point to be on a string of curves.
	Tangent to String	Constrains a curve to be tangent to a string of curves.
	Perpendicular to String	Constrains a Curve to be perpendicular to a astring of curves.
	Non-uniform Scale	Constrains a spline to scale proportionally along the spline length.
	Uniform Scale	Constrains a spline to scale in two directions maintaining the splines shape.
	Slope of Curves	Constrains the tangent direction of a spline to be parallel to a curve at a defining point.

Dimensioning

Click Rapid Dimensions , to create measurements.

Under the menu "Method" you can choose among different measurement types (horizontal, vertical, angular, asf.). for now leave it at Inferred .

Select the long vertical line of the L. As length, enter 100 mm.

Dimension your sketch as shown in the picture on the right. (figure "L dimensioned").

Make sure your sketch is fully constrained.

End sketch mode with  .

Save your model.

References

Especially with complex sketches, it can be convenient to work with references. These are datums that can be created from sketch elements. How to use them is illustrated in the following example:

The mount on the right should be created by extruding a sketch. The diameter of three cylinders is known. They are placed symmetrically around an imaginary circle in the middle, of which the diameter is known as well. To create the mount, 3 lines with an angle of 120° to eachother are created. The endpoints of those represent the midpoints for 3 circles with the diameter D=50mm. To fulfill the requirement, that the 3 small circles surround a bigger circle (diameter D=100mm), this circle is created in the point of origin. By using the Tangent constraint, the small circles are aligned around the big one. (refer figure "Sketch created"). Now you can create similar geometries, by only changing the diameters specified before.
To extrude the sketch properly, the big circle and the 3 lines have to be references. To convert those elements, click on them with RMB and choose Convert To/From Reference   (refer figure "Sketch with references"). References can be handled like normal sketch elements (constraints, dimensioning, etc.), at the same they'll be ignored outside of sketch mode. (refer figure "extruded properly").

You can convert references back to normal sketch elements by following the same steps.

This is a summary of the most important tools within sketch mode:

Tool	Function	Icon
Profile	draw profiles (can contain arcs)
Line	draw lines
Arc	draw arcs
Circle	draw circles
Quick Trim	trim sections of lines
Fillet	round off edges
Rectangle	draw rectangles
Make Corner	connect the ends of two lines to a corner