
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. May you want to select a curve, choose another type in the
combo list.
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. 




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





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, it is projected onto the
curve.

If no point is selected, the curve's extremity is used as reference. 

Select an option point to determine whether the new point
is to be created:
 at a given distance along the curve from the reference point
 a given ratio between the reference point and the curve's
extremity.



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).

The corresponding point is displayed. 


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 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.


It is not
possible to create a point with an euclidean distance if the distance
or the ratio value is defined outside the curve. 

Several options are available:
 Nearest extremity allows you to display the point at
the nearest extremity of the curve.
 Middle Point allows you 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. 
 Reverse Direction allows you to display:
 the point on the other side of the reference point (if a
point was selected originally)
 the point from the other extremity (if no point was
selected originally).

 Repeat object after OK lets you create equidistant
points on the curve, using the currently created point as the
reference, as described in Creating
Multiple Points and Planes.






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:
With N the normal to the selected plane (reference plane), H results
from the vectorial product of Z and N (H = Z^N).
If the norm of H is strictly positive then V results from the
vectorial product of N and H (V = N^H).
Otherwise, V = N^X and H = V^N. 
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. 





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.






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. 





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. 





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.


