Defining a Point on a Face

Here are the methods you can use to define a point on a face (see also "Inserting a Datum Point onto a face of a solid").
 

• Point
  the feature is initially centered at the point you chose when you selected the face in which to create the feature.
  1. To move the feature, click on Point in the selection list and then click to select a new center point. You can also move the feature by dragging its center-point handle.

• From 2 lines
  the center of the feature is based on the distances from two (history based) lines which can be:
  • Edges, even not belonging to the same faces
  • Datum lines
  • Lines belonging to profiles.
  1. In the 1st Distance mini-dialog, specify the distance from the first line, or drag the feature center-point handle. To specify a different line as the first one, click on First Line in the selection list and then select the line.
  2. In the 2nd Distance mini-dialog, specify the distance from the second line, or drag the feature center-point handle. To specify a different line as the second one, click on Second Line in the selection list and then select the line.
  In the selection list the Reference Planar Face is displayed: the selection of a planar face is optional if the face is planar, mandatory if the face is not planar.

• From-along edge
  the center of the feature is based on the distance from one boundary edge of the face in which datum point is to be created or on the Reference Planar Face (see below) and the distance along that edge.
  1. In the first Distance mini-dialog, specify the distance along the selected edge to the center of the feature, or drag the feature center-point handle. To specify a different reference edge, click on Reference Edge in the selection list and then select a new edge.
  2. In the second Distance mini-dialog, specify the distance perpendicular from the selected edge to the center of the feature, or drag the feature center-point handle.

• Polar — the position of the center of the feature is based on its radius distance from a polar origin and the angle from a reference line.
  1. Origin — the origin is a mandatory selection element, whenever possible, the default origin will be automatically selected based on the face selection. You can change the origin by clicking on Origin and specifying another point.
  2. Reference Direction — you will have to specify the reference direction (as an existing line or the one identified by two points to be selected); whenever possible, the default reference direction will be automatically selected based on the face selection. You can change it by clicking on Reference Direction and specifying another direction.
  3. In the Radius mini-dialog, specify the radius from the origin to the position of the center of the feature, or drag the point handle.
  4. In the Angle mini-dialog, specify the angle from the reference line to position of the datum point, or drag the datum point handle.

     In the selection list the Reference Planar Face is displayed: the selection of a planar face is optional if the face is planar, mandatory if the face is not planar.

• Cartesian
  the center of the feature is defined through its X, Y coordinates measured starting from an origin and using a reference X-axis.
  • Origin — the origin is a mandatory selection element, whenever possible, the default origin will be automatically selected based on the face selection. You can change the origin by clicking on Origin and specifying another point.
  • Reference Direction — you will have to specify the reference direction (as an existing line or the one identified by two points to be selected); whenever possible, the default reference direction will be automatically selected based on the face selection. You can change it by clicking on Reference Direction and specifying another direction.
  • Reference Planar Face — the selection of a planar face is optional if the face is planar, mandatory if the face is not planar. You can change it by clicking on Reference Planar Face and specifying another face.
  • Delta X and Delta Y — are the distances (to be specified) of the point from the origin along the selected Reference Direction and in the direction orthogonal to it.

• Parameters
  the center of the feature is based on the u and v parameters of the face in which the feature is to be created.
  1. In the U mini-dialog, specify the U parameter, or drag the feature center-point handle.
  2. In the V mini-dialog, specify the V parameter, or drag the feature center-point handle.