4.1.1.2 Simple sketch

 

Sketch

Click Sketch in Task Environment  . You can find this icon within the tab Modeling.

Now you have to define a drawing plane. Select the YZ-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   (figure "Drawing lines").

Draw a 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.

Attention:

Sketches always have to be fully constrained. Auto-constraints are only basic help by NX - your modeling strategy is not reflected by this. This is why you have to replace auto-constraints with your own constraints / dimensioning.

Hint:

If you made a mistake when drawing, deactivate the profile-tool by clicking  again. Now you can select specific lines or your whole sketch by dragging a rectangle around it with your mouse. The highlighted elements can be deleted by pressing Del / Entf.

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")

Hint:

The Dialog on the lower egde of your screen says: "Sketch is fully constrained with auto dimensions". After you constrained and dimensioned your sketch on your own, it'll change to: "Sketch is fully constrained".

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

When constraints are missing in your Sketch, NX marks the missing degrees of freedom with red arrows next to the respective points. To see the marks, you need to either open the Sketch Relations Browser (will be explained in chapter 4.1.1.3) or the Geometric Constraints window. Two degrees of freedom are still present in the picture on the right. The vertical line on the left can still be moved horizontally, so you can see horizontal arrows on its endpoints. The upper horizontal line can still be moved vertically, so the arrows are displayed vertically. (figure "degrees of freedom")

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 alignment	Specifies two points to be horizontally aligned
	Vertical alignment	Specifies two points to be vertically aligned
	Midpoint	Alignes a point with a midpoint
	Horizontal	Horizontal alignment
	Vertical	Vertical alignment
	Point on Curve	An endpoint can be placed on a line or arc.

Furthermore the following list of geometric constraints exists in NX and could be used if so wished (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.

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").

Hint:

If you accidentally rotated your sketch with CMB, you can adjust your view back to your sketch by clicking  View -> Orient View to Sketch . This function can also be accessed via the context menu (refer chapter 3.7.2 "Navigating with the mouse").

Make sure your sketch is fully constrained.

End sketch mode with  .

Save your model.

Hint:

If you want to edit a sketch later on, RMB-click on it within the part navigator and choose  Edit...

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 a 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 whith 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 "Properly extruded").

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