4.1.1.3 Complex sketch

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

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

Make sure, that this function  alt (Create Inferred Constraints) is active in sketch mode. Otherwise, your sketch may not be fully constrained later on.
If you can not 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.

Firstly, create the I with a rectangle alt. Adjust the left side to the vertical axis with alt. You can find the measurements for the rectangle in the picutre on the right. (figure "I measurements").

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I measurements

 

Next, you should create the D. Use alt, to create an arc like shown in the figure on the right. (figure "D measurements")

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D measurements

 

Important:
  • Make sure, that you create the arc somewhere within your sketch so that the midpoint is not located on the horizontal axis. That ensures that you recognize every constraint that is still missing.

Create a second arc.

Apply constraints in a way that the second arc is concentric alt to the first one.

Connect the endpoints of the arcs with lines alt, so that they form a D. The lines should be aligned vertically alt.

Eventually you have to make both vertical lines colinear alt. (figure "D finished")

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D finished

 

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:

  1. Display every previously applied constraint by clicking Display Sketch Constraints alt , or
  2. Go to Show/Remove Constraints alt.

All in Active Sketch shows you every constraint that is applied. You can select every single constraint, change their order with the small arrows or remove constraints with Remove Highlighted. (figure "Show/Remove Constraints")

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Show/Remove Constraints

 

Now, create the contour of the K. Make sure, that the horizontal line of the K is not colinear with the coordinate axis, but at a distance of 1mm to it. The other letters should also end on the same Y-Coordinate. The function Perpendicular alt and Parallel alt are useful to create perpendicular or parallel lines. (figure "K dimensioned")

 

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K dimensioned

Draw a horizontal line that crosses the D as well as the I. It should be placed 1mm above the horizontal axis.

Mirror this line across the horizontal axis Insert -> Sketch Curve -> Mirror Curve... alt. Firstly, select the newly created line (for "Select Curve") and subsequently select the horizontal axis as Centerline ("Select Centerline"). (figure "Mirror Curve")

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Mirror Curve

 

Confirm by clicking  OK.

Now you should have two parallel lines. Trim any unnecessary sections with the function Quick Trim alt .

Delete all unnecessary sections so that your sketch resembles the sketch shown in figure "DIK trim".

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DIK trim

 

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 "DIK finished")

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DIK finished

 

Save your Model.

NX's sketch mode has defined color coding. Dimensions are displayed in different colors, depending on their necessity. If they are unnecessary, the dialog 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) alt
Line draw single lines alt
Arc draw arcs alt
Circle draw circles alt
Quick Trim trims sections of lines alt
Fillet round off edges alt
Rectangle draw rectangle alt
Make Corner connects the ends of two lines to a corner alt
Mirror Curve mirrors elements across a center line
Offset Curve creates a scaled version of selected elements
Tool (for references) Function Icon
Inferred Dimension add measurements/dimensions to your sketch alt
Constraints add constraints alt
Display Sketch Constraints Show all constraints in the sketch alt
Show/Remove Constraints Dialog used for displaying and removing constraints alt
Inferred Constraints and Dimensions configure constraints alt
Other important  functions  Function Icon
Finish Sketch Close sketch mode alt
Orient View to Sketch Adjust your view to the drawing plane alt