Sketch Options
Sets the default system options for sketching.
To set the default sketching options:
Click Options
, Sketch or Tools, Options,
Sketch.
Select
from the following options, then click OK.
Use fully defined sketches. Requires
sketches to be fully
defined before they are used to create features.
Display arc centerpoints in
part/assembly sketches. Displays arc centerpoints in sketches.
Display entity points in
part/assembly sketches. Displays endpoints of sketch entities as
filled circles. The color of the circle indicates the status of the sketch
entity:
Black
= Fully defined
Blue = Under defined
Red = Over defined
Green = Selected
Over
defined and dangling points are always displayed, regardless of this
option.
Prompt to close sketch. Displays a dialog
box with the question, Close Sketch With
Model Edges? if you create a sketch with an open profile, then
click Extruded Boss/Base to create
a boss feature. Use
the model edges to close the sketch profile and select the direction in
which to close the sketch.
Create sketch on new part. Opens a new
part with an active sketch on the Front
Plane.
Override Dims on Drag/Move. Overrides
dimensions when you drag sketch entities or move the sketch entity in
the Move
or Copy PropertyManager. The dimension updates after the drag is complete.
This option is also available
in Tools, Sketch
Settings, Override Dims on Drag/Move.
If the display is slow due
to the shaded plane, it may be because of the Transparency
options. With some graphics cards, the display speed improves if
you use low transparency. To set a low transparency, click Tools,
Options, System
Options, Performance
and clear High quality for normal view
mode and High quality for dynamic
view mode.
Display virtual sharps. Creates a sketch
point at the virtual intersection point of two sketch entities. Dimensions
and relations to the virtual intersection point are retained even if the
actual intersection no longer exists, such as when a corner is removed
by a sketched fillet or a sketched chamfer. (To set the display options
for virtual sharps, click Tools,
Options, Document
Properties, Virtual
Sharps.)
Line length measured between virtual sharps
in 3d. Measures the line length from virtual sharps, as opposed
to end points in 3D sketches.
Enable spline tangency and curvature handles.
Displays spline
handles for tangency and curvature.
Show spline control polygon by default.
Displays a control
polygon to manipulate the shape of a spline.
Ghost image on drag. Displays a ghost
image of a sketch entities' original position while you drag a sketch.
Show Curvature Comb Bounding Curve.
Displays or hides the bounding
curve
used with curvature
combs.
Enable on screen numeric input on entity creation.
Displays numeric input fields to specify sizes when creating sketch entities.
Over defining dimensions:
Prompt to set driven state. Displays
a dialog box with the question, Make Dimension Driven?
when you add an over defining dimension to a sketch.
Set driven by default. Sets the dimension
to be driven
by default when you add an over defining dimension to a sketch.
Use Prompt
to set driven state alone or with Set
driven by default. Depending on your selections, one of four actions
occur when you add an over defining dimension to a sketch:
A
dialog box appears that defaults to driven.
A
dialog box appears that defaults to driving.
The
dimension is driven.
The
dimension is driving.