Creating Lines in Catiav5

Creating Lines


Path:
Insert | Profile | Line | Line
Insert | Profile | Line | Infinite Line
Insert | Profile | Line | Bi-Tangent Line
Insert | Profile | Line | Bisecting Line
Insert | Profile | Line | Line Normal to Curve
Located in a fly-out on the Profile toolbar.


Use this to ...
• Create lines in a sketch.

Prerequisites
• The Sketcher workbench must be active.
• The Sketch tools toolbar must be visible, and Dimensional and Geometrical Constraints active.
• All SmartPick options must be active.

Process: Creating a Line Using Coordinates

1. Select Insert | Profile | Line | Line.
2. In the Graphics window, pick the start point.
Or
On the Sketch tools toolbar, enter the H and V values for the start point and press TAB.
The text boxes change, allowing you to define the endpoint of the line.
3. In the Graphics window, pick the endpoint.
Or
On the Sketch tools toolbar, enter the H and V values for the endpoint and press TAB.
CATIA creates the line and adds dimensions from the sketch origin if you specify an H and V value.

Process: Creating a Line from Endpoints

1. Select Insert | Profile | Line | Line.
2. In the Graphics window, pick the start location of the line by picking an existing endpoint. CATIA displays a preview of the line as you move the mouse.
3. Pick the end location of the line by picking an existing endpoint. CATIA creates the line.

Process: Creating a Line from the Midpoint of a Line

1. Select Insert | Profile | Line | Line.
2. In the Graphics window, move the cursor over the line that contains the midpoint.


3. Right-click and select Midpoint from the pop-up menu. CATIA creates the first endpoint of the line and displays a preview.
4. Pick the endpoint of the line to create it.


Process: Creating a Parallel Line

1. Select Insert | Profile | Line | Line.
2. In the Graphics window, pick the start point of the line.
3. Move the cursor over the line that you want to be parallel. CATIA highlights the line.
4. Right-click and select Parallel from the pop-up menu. CATIA locks the previewed line parallel to the line you select.
5. Pick the endpoint of the line.

Process: Creating a Perpendicular Line

1. Select Insert | Profile | Line | Line.
2. In the Graphics window, pick the start point of the line. CATIA displays a preview of the line as you move the mouse.
3. Move the cursor over the line that you want to be perpendicular. CATIA highlights the line.
4. Right-click and select Perpendicular from the pop-up menu. CATIA locks the previewed line perpendicular to the line you select.
5. Pick the endpoint of the line.

Process: Creating Infinite Lines

1. Select Insert | Profile | Line | Infinite Line.
2. On the Sketch Tools toolbar, click either Horizontal Line or Vertical Line.
3. In the Graphics window, pick the point that the line passes through.
Or
On the Sketch tools toolbar, enter the H and V values for the point that the line passes through and press TAB.

CATIA creates the infinite line.

Process: Creating a Bi-Tangent Line

1. Select Insert | Profile | Line | Bi-Tangent Line.
2. In the Graphics window, pick the geometry that contains the first tangent point.
3. Pick the geometry that contains the second tangent point to create the line.

Process: Creating a Bisecting Line
1. Select Insert | Profile | Line | Bisecting Line.
2. In the Graphics window, pick the first line that you want to bisect.
3. Pick the second line that you want to bisect. CATIA creates an infinite line.

Process: Creating a Line Normal to a Curve

1. Select Insert | Profile | Line | Line Normal to Curve.
2. In the Graphics window, pick a point in space to define the first endpoint of the line.



3. Pick the curve that the new line will be normal to.


4. CATIA creates the line and a Perpendicular constraint.


Options
Infinite Line
Creates an infinite line in space. The three options available on the Sketch tools toolbar are Horizontal, Vertical, and Line through Two Points.

Horizontal Line
Creates an infinite horizontal line.
Vertical Line
Creates an infinite vertical line.
Infinite Line Through Two Points
Creates an infinite line through two points. This command is similar to the standard line creation.
Line Normal to Curve
Creates a line perpendicular to a selected curve.

Select a Curve Before
Reverses the selection order. This is located on the Sketch tools toolbar. Pick the curve first, then the opposite endpoint.

Tips
• Use SmartPicks to increase productivity.
• Look at the geometric symbols that appear when constructing geometry. By reviewing these symbols, you will know if you are creating unwanted geometric constraints.
• Hold SHIFT to deactivate SmartPick when creating geometry.
• Double-click the icon to use the same command continuously.

Creating Points

Creating Points



Path:
Insert | Profile | Point | Point
Insert | Profile | Point | Point...
Insert | Profile | Point | Equidistant Points
Insert | Profile | Point | Intersection Point
Insert | Profile | Point | Projection Point

Located in a fly-out on the Profile toolbar.

Use this to ...
• Create points.
• Create equidistant points.
• Create intersection points.
• Create projection points.

Prerequisites
• You should be in the Sketcher workbench.
• The Sketch tools toolbar must be visible, and Dimensional and Geometrical constraints active.
• All SmartPick options must be active.

Process: Creating a Point by Clicking
1. Select Insert | Profile | Point | Point.
2. In the Graphics window, pick the point.
Or
On the Sketch tools toolbar, enter the H and V values for the point and press TAB. CATIA creates the point and its associated dimensions if specified using the toolbar.

Process: Creating Points Using Coordinates
1. Select Insert | Profile | Point | Point… The Point Definition dialog displays.



2. Click Cartesian or Polar.
3. Enter the coordinates of the point.
4. Click OK to create the point and its associated dimensions.

Process: Creating Equidistant Points – Points and Length

1. Select Insert | Profile | Point | Equidistant Points.



2. In the Graphics window, pick the geometry on which you want to create equidistant points. The Equidistant Point Definition dialog displays.
3. In the New Points text box, enter the number of points.



4. Click OK to create the points.

Process: Creating Equidistant Points – Points and Spacing

1. Select Insert | Profile | Point | Equidistant Points.


2. In the Graphics window, pick the geometry on which you want to create equidistant points. The Equidistant Point Definition dialog displays.


3. Pick the origin point. The Equidistant Points Definition dialog text boxes become selectable.
4. In the New Points text box, enter the number of points.



5. In the Spacing text box, enter the spacing.
6. Click OK to create the points.

Process: Creating Equidistant Points – Spacing and Length

1. Select Insert | Profile | Point | Equidistant Points.


2. In the Graphics window, pick the geometry on which you want to create equidistant points. The Equidistant Points Definition dialog displays.
3. Pick the origin point. The Equidistant Points Definition dialog text boxes become active.



4. In the Parameter list, select Spacing and Length.



5. In the Spacing text box, enter the spacing.



6. In the Length text box, enter the length.
7. Click OK to create the points and dimensions.

Process: Creating Intersection Points

1. Select Insert | Profile | Point | Intersection Point.
2. In the Graphics window, pick the first element to intersect.
3. Pick the second element to intersect. CATIA creates the intersection point and geometric constraints.

Process: Creating Projection Points

1. In the Graphics window, pick the points for projection.
2. Select Insert | Profile | Point | Projection Point.
3. Pick the element for the points to project onto. CATIA creates the points and geometric constraints.

Options



Point Definition Using Cartesian Coordinates

Allows you to specify the point location using Cartesian coordinates. Cartesian coordinates define a point by specifying the horizontal and vertical position relative to a datum.





Point Definition Using Polar Coordinates

Allows you to specify the point location using Polar coordinates. Polar coordinates define a point by specifying a radius and an angle that the point lies on relative to a datum.


Equidistant Points – Parameters
Specifies how to create the specified points.



Points and Length
Creates a number of equidistant points along a specified length. This option is the default when the Equidistant Points Definition dialog displays.



Points and Spacing
Creates a number of points along a specified spacing. This option is only available after you pick a start point.


Spacing and Length
Creates a number of points along a specified spacing and length. This option is only available after you pick a start point.
Projection Point
When this option is active, two projection methods are available on the Sketch tools toolbar.

Orthogonal Projection
Projects the point in a direction that is perpendicular to the target curve object.
Along a Direction
Projects the point in a direction that you specify by entering H, V, and Angle data.