4.1.1.3 Complex sketch

Create a new model with the name plcm according to the naming convention.

Enter sketch mode and choose the XY-Plane as your drawing plane. Create the P, L, C and M in the same sketch. (For demonstrational purposes, the six-line rule for sketches is ignored here)

Make sure, that this function  (Create Inferred Constraints) is active in sketch mode. Otherwise, your sketch may not be fully constrained later on.
If you cannot find this function, enter "Create Inferred Constraints" into Command Finder and let NX show you where this function is located by hovering over it with your mouse in Command Finder.

Start by modeling the P using three rectangles , take the measurements shown in this figure (figure "P made of rectangles"). Align the leftmost line of the P to the vertical axis. Use the constraint .

Use , to create two arcs as shown (figure "P rounded").
It's important to use the exact corners of the rectangles for creation.

 

Next you will create the L. Again use rectangles, the measurements are in the following figure. (figure "L measurements")
Place the L right of the P in a 10mm distance and align the bottom line of the L to the horizontal axis.

 

Make sure that the message Sketch is fully constrained is displayed. It's displayed in the bar on the lower edge of your screen.

If there are problems with applying constraints, there are two options to help you:

Every sketch element, constraint-status (fully , partially , conflicting ) and, when fully expanded, the elements referenced by constraints are displayed here. (Figure "Sketch Constraints Browser").
Here you can now delete problematic objects and constraints by klicking on them with the RMB.

Attention:

The Sketch Constraints Browser does not always show the constraint status of components correctly. Sometimes, components that are actually fully constrained are displayed as partially constrained and vice-versa. Always look at the low center bar in Sketch mode to check if your finished sketch is fully constrained!

Now create the C. Start by creating two circles below the P one with a diameter of 80mm and the other one with a diameter of 40mm. Use the feature .

Place a constraint making both circles concentric. (figure "concentric circles")

Draw two lines coming from the center of the circles to the outer arc and use the constraint Perpendicular to create a right angle.
Afterwards use the dimensioning tool to set a 45 degree angle between the upper line and the horizontal axis. (figure "45 degree angle")

Start the M by drawing the profile of a slanted beam. Use the measurements from this figure (figure "slanted beam") and use the constraints Parallel and Equal Length .

In the next step you will mirror the beam. Choose the sketching feature Mirror Curve and first select the bottom vertikal line of the beam as mirror axis and afterwards the remaining lines of the beam (figure "mirrored beam").

To complete the M add a rectangle with a height of 80mm and a width of 20mm to the right (figure "M completed").

In the last step trim any unnecessary sections with the function Quick Trim .

Delete all unnecessary sections so that your sketch resembles the sketch shown in figure "PLCM completed" and group the letters in a distance of 10mm to each other.

 

Trimming unwanted sections of lines, could cause you to lose constraints sometimes. These may have to be added back in to make your sketch fully constrained.

The small yellow arrows show which references still have to be defined. Add measurements as shown in the picture on the right to fully constrain your sketch. (figure "PLCM measurements")

 

Save your Model.

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NX's sketch mode has defined color coding. Dimensions are displayed in different colors, depending on their necessity. If they are unnecessary, the dialogue bar indicates Sketch contains over constrained geometry.

The most important colors of sketch mode are:

Color	Meaning
Green	Color of curves if the sketch is deactivated. Default color for curves in the active Sketch.
Blue	Sketch dimensions (without conflicts) Curves that do not belong to any sketch are marked blue.
Red	Geometry and dimensions that are over constrained Arrows of present degrees of freedom
Pink	When adding constraints causes conflicts, dimensions related to this issue are shown pink.
Grey	Geometry and dimensions that are affected by Convert To/From Reference
Green	As soon as your sketch is fully constrained, it turns green.

The following list contains all important icons for working in sketch mode:

Tool	Function	Icon
Profile	draw curves/profiles (can contain arcs)
Line	draw single lines
Arc	draw arcs
Circle	draw circles
Quick Trim	trims sections of lines
Fillet	round off edges
Rectangle	draw rectangle
Make Corner	connects the ends of two lines to a corner
Mirror Curve	mirrors elements across a center line
Offset Curve	creates a scaled version of selected elements
Tool (for references)
Inferred Dimension	add measurements/dimensions to your sketch
Constraints	add constraints
Sketch Constraints	Show all constraints in the sketch
Show/Remove Constraints	Dialogue used for displaying and removing constraints
Inferred Constraints and Dimensions	configure constraints
Other important functions
Finish Sketch	Close sketch mode
Orient View to Sketch	Adjust your view to the drawing plane