This task shows the various methods for creating points: 





Open the Points3D1.CATPart document. 

A new lock button is available besides the Point type to prevent an automatic change of the type while selecting the geometry. Simply click it so that the lock turns red .
For instance, if you choose the Coordinates type, you are not able to select a curve. If you want to select a curve, choose another type in the combo list. The status of this button is stored as the default value: therefore, if it is red and you
launch the same command again or another command owning this button, the button will be red too.
This capability is not available in objectaction mode and is not retained at edition. 

If the input is selected automatically, when we change the type, the input will not be transferred to the new type. For example, if we select On Curve in Point type, and a closed curve is selected as input, an extremum feature is created automatically. This extremum feature would not be transferred, if we change point type to coordinates. 

Coordinates


 Click Point .
The Point Definition dialog box appears. 
 Select the Coordinates point type.
 Enter the X, Y, Z coordinates in the current axissystem.
 Optionally, select a Reference Point.
When the command is launched at creation, the initial value in the Axis System field is the current local axis system. If no local axis system is current, the field is set to Default.
Whenever you select a local axis system, the point’s coordinates are changed with respect to the selected axis system so that the location of the point is not changed. This is not the case with points valuated by formulas: if you select an axis system, the defined formula remains unchanged. 


 If you create a point using the coordinates method and an axis system is already defined and set as current, the point’s coordinates are defined according to current the axis system.
 The current local axis system must be different from the absolute axis.

 Click Compass Location. If the compass is lying on the geometry, the X, Y, and Z coordinates of the point are modified according to the location of the compass. However, if the compass is not lying on the geometry, i.e. it is at default location, clicking this button would display an error message, and the point would be created using existing specified coordinates.

The Compass Location button is disabled when any of the X, Y, or Z coordinate is specified using a formula. 
 Click OK to create the point.
The point (identified as Point.xxx) is added to the specification tree. 


On curve


 Click Point .
The Point Definition dialog box appears. 
 Select the On curve point type.
 Select a curve.
 Optionally, select a reference point.
If this point is not on the curve, the minimum distance between the point and the curve is
computed. 
If no point is selected, the curve’s extremity is used as reference. 
 Select an option point to determine where the new point is to be created:
 Distance on curve: Point is created at a given distance along the curve from the reference point. A distance value needs to be specified.
 Distance along direction: Point is created along a specified direction and at an offset distance from the reference point. Direction and offset values need to be specified.
 Ratio of curve length: Point is created at a given ratio between the reference point and the curve’s extremity.
A ratio value needs to be specified.


 Enter the distance or ratio value.
If a distance is specified, it can be:
 a Geodesic distance: the distance is measured along the curve.
 an Euclidean distance: the distance is measured in relation to the reference point (absolute value). Therefore, Distance on curve and Ratio of curve length are unavailable.

The corresponding point is displayed. 

 It is not possible to create a point with an euclidean distance if the distance or the ratio value is defined outside the curve.
 These options are available only with Distance on curve and Ratio of curve length options.


 You can select either Nearest extremity to display the point at the nearest extremity of the curve or Middle point to display the midpoint of the curve.

 Be careful that the arrow is orientated towards the inside of the curve (providing the curve is not closed)
when using the Middle Point option.
 These options are available only with Distance on curve and Ratio of curve length options.

 Click Reverse Direction to display either the point on the other side of the reference point (if a point was selected originally) or the point from the other extremity (if no point was selected originally).
 Select the Repeat object after OK option to create equidistant points on the curve, using the currently created point
as the reference, as described in Creating Multiple Points and Planes.

This option is available with Distance on curve and Ratio of curve length options. 
 Click OK to create the point.
The point (identified as Point.xxx) is added to the specification tree. 

 If the curve is infinite and no reference point is explicitly given, by default, the reference point is the
projection of the model’s origin
 If the curve is a closed curve, either the system detects a vertex on the curve that can be used as a reference point, or it creates an extremum point, and highlights it (you can then select another one if you wish) or the system prompts you to manually select a reference point.
Extremum points created on a closed curve are aggregated under their parent command and put in no show in the specification tree.




 If the input point is selected automatically and you change the type, it is not retained to the new type. For instance, an extremum feature would not be retained if you change its type from On curve to Coordinates.
 If the input for the curve is a feature, and an extremum point exits on this curve, this point is used as reference point.
 If the input for the curve is a part of a geometric feature (here an edge), and even though an extremum point already exists on this geometric feature, a new extremum is created.



On plane


 Click Point .
The Point Definition dialog box appears. 
 Select the On plane point type.
 Select a plane.
If you select one of the planes of any local axis system as the plane, the origin of this axis system is set as the reference point and featurized. If you modify the origin of the axis system, the reference point is modified accordingly. 
 You can select a point to define a reference for computing coordinates in the plane.
If no point is selected, the projection of the model’s origin on the plane is taken as reference. 
 Optionally, select a surface on which the point is projected normally to the plane.
The reference direction (H and V vectors) is computed as follows:
H and V are computed from the directions belonging to the geometrical plane. 
Would the plane move, during an update for example, the reference direction would then be projected on the plane. 
 Click in the plane to display a point.
 Click OK to create the point.
The point (identified as Point.xxx) is added to the specification tree. 


On surface


 Click Point .
The Point Definition dialog box appears. 
 Select the On surface point type.
 Select the surface where the point is to be created.
 Optionally, select a reference point. By default, the surface’s middle point is taken as reference.
 You can select an element to take its orientation as reference direction or a plane to take its normal as reference direction.
You can also use the contextual menu to specify the X, Y, Z components of the reference direction.
 Enter a distance along the reference direction to display a point.
 Choose the dynamic positioning of the point:
 Coarse (default behavior): the distance computed between the reference point and the mouse click is an euclidean distance. Therefore the created point may not be located at the location of the mouse click (see picture below).
The manipulator (symbolized by a red cross) is continually updated as you move the mouse over the surface.


 Fine: the distance computed between the reference point and the mouse click is a geodesic distance. Therefore, the created point is located precisely at the location of the mouse click.
The manipulator is not updated as you move the mouse over the surface, only when you click on the surface.


 Click OK to create the point.
The point (identified as Point.xxx) is added to the specification tree. 

 The dynamic positioning option is persistent but is not stored in the feature. Therefore, at edition, the dynamic positioning may not be the one you selected.


 Sometimes, the geodesic distance computation fails. In this case, an euclidean distance might be used and the created point might not be located at the location of the mouse click. This is the case with closed surfaces or surfaces with holes. We advise you to split these surfaces before creating the point.



Circle / Sphere / Ellipse center


 Click Point .
The Point Definition dialog box appears:

 Select the Circle / Sphere / Ellipse center point type.
 Select a circle, circular arc, ellipse, or elliptical arc, or
 Select a sphere or a portion of sphere.

A point is displayed at the center of the selected element. 

 Click OK to create the point.
The point (identified as Point.xxx) is added to the specification tree.


Tangent on curve


 Click Point .
The Point Definition dialog box appears. 
 Select the Tangent on curve point type.
 Select a planar curve and a direction line.
 Click OK to create the point.
The point (identified as Point.xxx) is added to the specification tree. 


Between


 Click Point .
The Point Definition dialog box appears. 
 Select the Between point type.
 Select any two points.
 Enter the ratio, that is the percentage of the distance from the first selected point, at which the new point is to be.
You can also click Middle Point to create a point at the exact midpoint (ratio = 0.5). 
Be careful that the arrow is orientated towards the inside of the curve (providing the curve is not closed) when using the Middle Point option.
If the curve is closed, the point is created along the orientation of the curve. 
 Select an optional Support. It can be a surface or a curve.
If a support is selected, the point is created between the two points measured along the support.
If the support is a curve, the distance along the curve is used. If the support is a surface, the created point lies on the computed geodesic curve between the two points on the surface. 

 If the ratio is less than 0 or greater than 1, the point is created along the extrapolated curve tangent to the support. In this case, the created point may not lie on the support.
 For a closed curve, the point is created along the orientation of curve. If you want to create the point along another part of the closed curve, the input points should be selected in reverse order.




 Points must lie on the support, otherwise an error message is issued.
 In some cases, it may not be possible to create a point on a surface with a hole or a closed surface (for instance, if the geodesic curve encounters a hole).

 Click Reverse direction to measure the ratio from the second selected point.

If the ratio value is greater than 1, the point is located on the virtual line beyond the selected points. 
 Click OK to create the point.
The point (identified as Point.xxx) is added to the specification tree. 





 Parameters can be edited in the 3D geometry. For more information, refer to Editing Parameters.
 You can isolate a point in order to cut the links it has with the geometry used to create it. To do so, use the Isolate contextual menu. For more information, refer to Isolating Geometric Elements.


