Drawing Tools

Create centerlines using two points on your drawing, including the end points on another 2-point linear centerline.

1. Click .
2. Select two points to establish a centerline. Note that you are able to use snap points, but it is not required.

   

When aligning dimensions and annotations, you can hover over edges, midpoints, or other lines to activate red inference points. Use the inference points to snap the location of the entity when creating or dragging a dimension or annotation. Similarly, you can move the mouse vertically or horizontally over views, lines, dimensions, or annotations to activate pink vertical and horizontal inference lines. Use these inference lines to align the location of the entity vertically or horizontally from the desired referenced annotation.

Create centerlines using two edges, two concentric arcs, or a single cylindrical or conical silhouette edge on your drawing.

1. Click .
2. To establish the centerline, do one of the following:
   • Select a single cylindrical or conical silhouette edge.
   • While holding the Shift key, select two edges or concentric arcs.

   

Adjust the length of the centerlines by clicking and dragging the grip points at the end of the centerline.

Create a circular centerline for a bolt circle diameter.

1. Click .
2. Click each of 3 points (centers of the holes, end, mid, or quad points). The illustration shows the centerline in process (the plus signs represent the selected points):

   

   The illustration below shows the centerline selected; you can see which holes help define the centerline:

   

   The centerline can now be dimensioned.

When aligning dimensions and annotations, you can hover over edges, midpoints, or other lines to activate red inference points. Use the inference points to snap the location of the entity when creating or dragging a dimension or annotation.

Create a circular centerline using two points.

1. Click .
2. Click a point to mark the center of the centerline (this does not have to be an actual circle center, you can snap to any point like an end point or midpoint as well).
3. Click a point to mark the circumference of the centerline (like the center of a bolt hole).

   The first illustration shows the centerline in process (the orange highlighting represents the selected points):

   

   You are now able to dimension the centerline.

When aligning dimensions and annotations, you can hover over edges, midpoints, or other lines to activate red inference points. Use the inference points to snap the location of the entity when creating or dragging a dimension or annotation.

Add a centermark

Place a mark in the centers of circles and arcs for visibility when printing and as a reference point for dimensions.

1. Click .
2. Select Single, Circular, or Linear.

   

3. Click the edge of a circle or arc:

   

4. (Circular and Linear centermarks only) Select the type of mark(s) you want to see: 

   • Circular: Reference center

     

   • Circular: Bolt circle

     

   • Circular: Radial lines

     

   • Circular: Pattern centermark

     

   • Linear: Connecting lines

     

5. Click the checkmark to accept the centermark(s).

Align a centermark

To orient a centermark to a line or edge:

1. Right-click the centermark.
2. Click Align centermark from the context menu.

   

3. Click the line or edge to align the centermark to.

Delete a centermark

To delete a centermark, click to select and press the Delete key. See centermarks for more centermark editing options.

Centermarks can be manually added to round and elliptical faces/regions, even if they are not normal to the Drawing view. This can be helpful when working with elliptical or cylindrical parts that are off-axis.

Create a virtual sharp associated with two linear edges. Virtual sharps are fully associated with the geometry and update appropriately with changes to the geometry.

1. Click .
2. Select first linear edge.

3. Select second linear edge.

   

Dimensions are to the intersection of the cross only. To change the visual style of the virtual sharp from Centermark to Edge extension, open the Drawing properties panel:

Shortcut: L

Create lines in your drawing.

1. Click .
2. Click to begin the line.
3. Drag and click to define subsequent line segments.
4. Escape to end the line and exit the tool.

Note that horizontal and vertical inferencing lines appear as appropriate:

Each segment in a series of connected lines is a separate entity.

As you draw, snap points appear on existing objects to aid you in line placement. Click once the snap points appears to connect to it automatically.

Tips

• There is no need to click directly on the point once it is visible. While moving the mouse to place the line, you'll notice thin, dashed lines as the cursor passes near other entities. These are inferencing lines that you are able to align the line to; simply click when you see the line appear to align to that inferencing line.

• To format lines, see Sketch geometry styles.

Shortcut: c

Create a circle in your drawing starting with its center point.

1. Click the Center point circle tool to set the center point.

2. Click again to set the radius.

   

TIps

• When aligning dimensions and annotations, you can hover over edges, midpoints, or other lines to activate red inference points. Use the inference points to snap the location of the entity when creating or dragging a dimension or annotation. Similarly, you can move the mouse vertically or horizontally over views, lines, dimensions, or annotations to activate pink vertical and horizontal inference lines. Use these inference lines to align the location of the entity vertically or horizontally from the desired referenced annotation.

  

• To format circles, see Sketch geometry styles.

Create a circle in your drawing by defining three points along its circumference.

1. Click the 3 point circle tool to set the start point.

2. Click to set the second point.

3. Click the third point to set the diameter.

   

Tips

• When aligning dimensions and annotations, you can hover over edges, midpoints, or other lines to activate red inference points. Use the inference points to snap the location of the entity when creating or dragging a dimension or annotation. Similarly, you can move the mouse vertically or horizontally over views, lines, dimensions, or annotations to activate pink vertical and horizontal inference lines. Use these inference lines to align the location of the entity vertically or horizontally from the desired referenced annotation.

  

• To format circles, see Sketch geometry styles.

Shortcut: g

Create a rectangle in your drawing starting with a corner point.

1. Click the Corner rectangle tool to start a corner.

2. Click to end at the diagonal corner.

   

Tips

• When aligning dimensions and annotations, you can hover over edges, midpoints, or other lines to activate red inference points. Use the inference points to snap the location of the entity when creating or dragging a dimension or annotation. Similarly, you can move the mouse vertically or horizontally over views, lines, dimensions, or annotations to activate pink vertical and horizontal inference lines. Use these inference lines to align the location of the entity vertically or horizontally from the desired referenced annotation.

  

• To format rectangles, see Sketch geometry styles.

Shortcut: r

Create a rectangle in your drawing starting with its center point.

1. Click the center point rectangle tool to set the center point.

2. Click again to set a corner.

   

Tips

• When aligning dimensions and annotations, you can hover over edges, midpoints, or other lines to activate red inference points. Use the inference points to snap the location of the entity when creating or dragging a dimension or annotation. Similarly, you can move the mouse vertically or horizontally over views, lines, dimensions, or annotations to activate pink vertical and horizontal inference lines. Use these inference lines to align the location of the entity vertically or horizontally from the desired referenced annotation.

  

• To format rectangles, see Sketch geometry styles.

Create a spline through multiple points.

1. Click .
2. Click to begin the spline.
3. Click to select additional points for the spline to fit to in the view.
4. Double-click or press Escape to end the spline.

As you draw, snap points appear on existing objects to aid you in spline placement. Click once the snap points appears to connect to it automatically. As with any spline, you are able to drag the points to reshape the spline.

Tips

• When aligning dimensions and annotations, you can hover over edges, midpoints, or other lines to activate red inference points. Use the inference points to snap the location of the entity when creating or dragging a dimension or annotation. Similarly, you can move the mouse vertically or horizontally over views, lines, dimensions, or annotations to activate pink vertical and horizontal inference lines. Use these inference lines to align the location of the entity vertically or horizontally from the desired referenced annotation.

• To format splines, see Sketch geometry styles.

Add points along a spline.

1. Click .
2. Click along the spline to set additional points.
3. Drag and click to define subsequent line segments.
4. Press Escape to exit the tool.

Drag spline points to modify the spline.

As you draw, snap points appear on existing objects to aid you in point placement. Click once the snap points appears to connect to it automatically.

Add a hatch region to enclosed sketch profile area.

1. Click the Hatch region button . The Hatch region dialog opens:

   

2. Sketch a closed profile using the sketch tools at the top of the dialog, or select a closed sketch profile in the drawing.
3. Select a standard: ANSI, ISO, or General.
4. Select from the following hatch parameters:
   • Pattern - Hatch material design
   • Scale - Size of the hatch pattern; Automatic, or 1.0 to 10.0 times the size, in integer increments.
   • Angle - Angle of the hatch pattern; Automatic, or 0.0 to 180 degrees in 15 degree increments.
   • Color - Color of the hatch pattern. By default, with Drawing properties checked. the global drawing color property is used for this hatch region. Uncheck to use a custom color instead.

   If a custom color is used, it is only visible in the drawing after the hatch region is accepted (by clicking the checkmark).

5. Click the checkmark to accept the new hatch region.

A preview of the hatch region is displayed at the bottom of the dialog.

Example of a hatch region on a side view of a rectangular sketch profile in a drawing.

You might see a spinner while the hatch region is being created. Press the ESC key to cancel the hatch creation.

Editing a hatch region

To edit a hatch region after it is applied, select it, then right-click and select Edit hatch. This opens the hatch dialog where the hatch can be edited.

Deleting a hatch region

To delete a hatch region, select it and press the Delete key on your keyboard, or right-click and select Delete from the context menu:

Drawing views in which hatch regions can be applied/edited

The following table outlines the views in which hatch regions can be applied and edited:

View	Apply/edit hatch
Projected	✓
Auxiliary	✓
Section	✓*
Aligned section	✓*
Broken out section	✓*
Detail
Break
Crop	✓

*Hatch is automatically applied when view is created.

Hatch color highlights

Hatch regions drawn with the hatch drawing tools display their hatch color in orange, with a yellow highlight surrounding the region (left image below).

Hovering your mouse near the region edge switches the highlight so that the hatch color is yellow and the highlight surrounding the region (and accompanying nodes) is orange (middle image below).

In both cases, hovering over the region also highlights the view's bounding box yellow.

If a closed profile is selected for the hatch region, when hovering your mouse over the region, the hatch color is orange, and the profile is highlighted light blue (right image below).

Hovering anywhere else in the view (outside hatch regions) highlights the view bounding box orange, highlights the surrounding area of hatch regions drawn with drawing tools yellow, and highlights the closed profile hatch color yellow (the profile is not highlighted):