About Geometry Using SmartPick

Reference Geometry

SmartPick finds out geometrical specifications according to geometrical elements that already exist in a sketch.

You will only detect geometrical specifications according to the current sketch elements that are visible in the 3D window in which the cursor is positioned. You will not need to perform any interaction and you will be returned a visual feedback as shown below in a non exhaustive way:

• Parallel (two lines)
  
  
• Tangent (a line and a circle)
  
  
• Perpendicular (two lines)
  
  
• Tangent (two circles)
  
  
• Concentric (a circle and an arc)
  
  
• Parallel (two lines)
  
  

As you will see when using SmartPick, snapping ambiguities currently occur. Besides, the dimensional specifications of a part often depend on technological specifications.

These dimensional specifications are defined as the part is being designed, they depend on the current application area and are, as a result, very hard to guess for the SmartPick tool.

In order to solve these ambiguities, SmartPick classifies possible snapping according to the geometric constraints that are associated to these snapping. As such, a given cursor positioning will be only assigned one snapping. Unfortunately, this classification cannot be modified. It is provided in the table below.

Moreover, to remove ambiguity during the creation of elements, the three options which are parallelism, perpendicular and tangency can be activated independently from each other. See SmartPick options in the Customizing section of this guide.

In addition to this classification, when several snappings are possible for a given type of geometric constraints, SmartPick takes into account the distance between the snapped cursor and the geometrical element according to which the snapping is possible. In this case, SmartPick snaps to the nearest element.

Nevertheless, there are some cases when SmartPick does not allow dimensioning as desired without additional interactions. This is why SmartPick manages two means for applying a particular snapping relatively to the geometrical elements.

Forcing the Snapping

SmartPick allows forcing the snapping on a given geometrical element using either:

• the contextual menu or
• the Ctrl key

SmartPick allows forcing the snapping on a given geometrical element using the contextual menu. You will avoid ambiguities linked to the automatic detection of elements in the current 3D viewpoint by forcing:

• snapping detected at a distance: parallel, perpendicular, concentric, tangency and curve (line/circle) that goes through a point.

  At a distance means that these constraints are detected even though the cursor is not positioned on the reference element.

• snapping at a given position that is relative to a geometrical element: line midpoint, circle center.

  At a given position means that both degrees of freedom are locked.

The contextual menu is therefore available when right-clicking most Sketcher geometrical elements. Of course, the contents of the contextual menu depends of the element that is being currently created. This contextual menu can be made of the below four sub-parts:

• Option that belongs to the Base Infrastructure product.
• Snapping the characteristic point that is being manipulated (see From scratch paragraph and table below).
• Snapping the geometrical element that is being created (see table below).
• Managing the parameters that are associated to the geometrical element that is being sketched.
  
  

Any snapping that is imposed via the contextual menu can be deactivated. To do this, right-click in the 3D window background and select Reset.

The table below lists the constraints that can be detected when snapping characteristic points which are being manipulated, relatively to existing geometrical elements, and thanks to the contextual menu.

The table below indicates the possible snapping for geometrical elements which are being created, relatively to existing geometry and thanks to the contextual menu.

	Element currently created
External Geometry =>		Point	Line	Ellipse
	Point
	Line	Midpoint Nearest end point
	Circle	Center Nearest end point
	Ellipse	Center Nearest end point		No
	Conic	No		No
	Spline	No		No

In the example below, you can see the various snapping possibilities for a line that is being created (dotted lines in the example) relatively to the existing spline: 3 tangency possibilities and 2 perpendicularity possibilities. The point you right-click to display the contextual menu is used to determine which option will be offered in the contextual menu. So depending on where you click, you will not be offered the same options.

Note that the software takes into account what has already been specified (in this example, the first point of the line) to offer the various snapping options. For this reason, depending on the first point of the geometrical element that is being created, there may be cases in which no solution can be found or in which the solution offered does not correspond to what you want. In such a case, try to right-click before and/or after the point you want the software to choose. If you try both ways, one solution at least should be found.

SmartPick also allows forcing the current snapping on an element using the Ctrl key:

• You can force SmartPick to remain snapped on an element whatever the position of the cursor. In order to do this, press the Ctrl key while the geometrical snapping you want to force is active (the element may be highlighted and symbols may appear). Keep the Ctrl key pressed.
• This functionality is efficient if once the Ctrl key is pressed you can still move the cursor. In other words, Ctrl has no effect if the current snapping inhibits both degrees of freedom. This is often the case when given snapping combinations are possible (for example at the intersection of two lines) or when the cursor is close to a given point (explicit or implicit as for example the midpoint of a segment).
• The Ctrl key is very useful when the sketch includes many geometrical elements because SmartPick takes into account the distance between the cursor and the geometrical element.
  
  
• This is the zone in which the line-circle tangency snapping (due to the circle proximity) has the first priority.
  
  Apart from this zone, either the tangency snapping is meaningless or it interferes with closest geometries or still with possible constraints that are assigned higher priorities (see table).

If SmartPick cannot solve an ambiguity and returns a snapping that you are not satisfied with, you can de-activate SmartPick assistant by pressing the Shift key.

Certain geometrical elements are assigned internal peculiar geometrical characteristics. For example and as shown below, this is the case for horizontal/vertical lines and for quarters of arcs of circles. When such an internal specification is found out by SmartPick, the color of the currently created geometrical element becomes blue.

Relation Between Parameters and Characteristic Points

There is a strong relation between the characteristic point of a geometrical element and some of the parameters it supports. In fact, if a parameter value is modified by moving the cursor, it means that the parameter is linked to the current characteristic point and consequently validating the point will modify the parameter status.

Indeed, as when valuated a characteristic point can no longer be modified, associated parameters get frozen which is echoed by a grayed entry in the Sketch tools toolbar.

As an example, in Arc Circle creation command, when the arc start point is defined (at the sketch origin on this picture) both Radius and Start Angle to H Axis get frozen. Indeed, as the arc center is necessarily previously defined, to impose arc start point leaves no ambiguity on the radius and the start angle of the sector.

Specific Parameters

Some parameters have a specific behavior. This behavior is common to all geometry creation commands that use these parameters. This is the case for Angle and Sector parameters.

This parameter is oriented so that no ambiguity is possible when defining an angular sector. In the standard units system, an angle range is from -360 to 360deg. Any other value is recomputed to this range. Positive values are for direct sectors (you go from the start direction to the end one the same way you go from H axis to V axis). Negative values are on the other end for reverse arcs (you go from the start direction to the end one the same way you go from V axis to H axis).

• A direct angular sector
  
  
  
  
• A reverse angular sector
  
  
  
  

The angle parameter is also oriented, its range is from 0 to 360 deg. As a consequence, a -10 deg value is identically equivalent to a 350 deg value and a 0 deg value is definitely not equal to a 180 deg value.

A fixed 30 deg angle value imposed to a line

By default, angle values are computed relatively to H Axis. This can be modified any time you want to define an angle value using the Parameters > Set as Angle Reference contextual command.

When an angle value is available in the Sketch tools toolbar, any line that is contained in the current sketch can be defined as the angle computation basis. To issue out orientation, a red arrow is displayed to show the reference line orientation. In this example, a 25 deg angle is set relatively to an existing line.

It is possible to copy some of the parameters values from any existing geometrical element that can be defined with the same parameters. The Copy functionality is available through the contextual menu Parameter section for length and radius parameters.

Length can be copied from a line while radius from a circle or an arc.