Creating and Exploring Sketch Mode

Creating and Exploring Sketch Mode

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Objectives

  Create a new sketch and explore the action bar in Sketch mode.

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Creating And Exploring Sketch Mode

Key Points

  It is important to fully understand how positioned and non-positioned sketches work so that you can properly use them.

  You cannot create an empty sketch. If you exit a sketch that contains no geometry, the sketch will not be created in the Specification Tree.

  A Non-Positioned or Sliding Sketch can be converted to a positioned sketch and vice versa.

Process of Creating a Sliding Sketch (Non-Positioned Sketch)

Step 1:

When creating a new 3D part, the Sliding or Non-Positioned sketch a proper way to begin. Select the Model section of the Action Bar and click the Positioned Sketch icon.

 

Step 2:

The Sketch Positioning Dialog appears.

Step 3:

In the Graphics Window or the Specification Tree, pick the YZ plane as Reference and select Type as Sliding under Support.

Note that the Sketch origin and orientation are the same as that of the 3D part.

Step 4:

Select OK CATIA activates the Sketcher workbench and takes you into the 2D Sketcher workspace.

 

Step 5:

On the Workbench toolbar, click Exit App to leave the 2D sketch work space and return to the 3D Graphics Window. Since nothing was was created in the sketch it will not show anything in the Specification Tree. When a sketch is created a sketch feature will be noted in the Specification Tree.

 

Process of Creating a Positioned Sketch

Step 1:

When creating a new 3D part from an existing sketch or solid model the Positioned Sketch is the proper way to begin. Select the Model section of the Action Bar and click the Positioned Sketch icon.

Step 2:

The Sketch Positioning Dialog appears.

In the Graphics Window or the Specification Tree, pick the YZ plane as Reference and select Type as Positioned under Support.

 

Step 3:

In the Origin Type list, set the type to your specific origin.

 

In the Graphics Window or the Specification Tree, pick the geometry that will define the origin point of the sketch.The sketch origin is now set to be at that point.

Step : 4

In the Orientation Type list, set the orientation method in the drop down menu.

In the Graphics Window or the Specification Tree, pick the geometry that will define the direction of the sketch axis.

Select the Horizontal or Vertical options to specify the direction of the sketch.

Step 5:

In the Graphics Window or the Specification Tree, pick the YZ plane as the planar support. CATIA activates the Sketcher workbench and takes you into the 2D Sketcher workspace. Note that the Sketch origin and axis orientation are different from that of the 3d part.

Step 6:

On the Workbench toolbar, click Exit App to leave the 2D sketch workspace and return to the 3D Graphics Window.

 

Options :

Planar Support

Defines the planar sketch support on which the sketch will be placed.    

 

Origin

These options define the methods for positioning the origin of the sketch.

 

Implicit 
Defines the sketch origin as the default origin of the face or plane that is selected as the sketch support. Selecting two lines prior to selecting the Positioned Sketch Icon places the origin at the intersection of the two lines. The H axis direction is collinear with the first line.
Part Origin
Defines the sketch origin as the absolute origin of the part.

Projection Point
Defines an origin by projecting a point onto the sketch positioning face or plane.

Intersection 2 Lines
Defines the origin at the intersection of two lines.

Curve Intersection
Defines the origin at the intersection of two curves.

Middle Point
Defines the origin at the mid-point of a line or edge.

Barycenter
Defines the origin at the center of a face.   

Orientation

Defines the Horizontal and Vertical directions of the sketch axes. When defining the direction, you can control either the H or V direction. You also have the ability to reverse the direction of the H and V sketch axes or swap them.

 

Implicit
Defines the sketch directions as the default directions of the sketch support.

X Axis
Defines the active direction along the X-axis of the model.

Y Axis
Defines the active direction along the Y-axis of the model.

Z Axis
Defines the active direction along the Z-axis of the model.

Components
Defines the active direction by entering vector components.

Through Point
Defines the active direction as the vector through a point.

Parallel to Line
Defines the active direction as parallel to a selected line.

Intersection Plane
Defines the active direction as the line created by the intersection of two planes.

Normal to surface
Defines the active direction as the normal of a selected surface.

 

H Direction
Lets you define the H direction of the sketch.

V Direction
Lets you define the V direction of the sketch.

Reverse H
Reverses the H vector.

Reverse V
Reverses the V vector.

Swap
Swaps the H and V directions.  

   

Modification in CATIA V6 R2017x

  In CATIA V6 R2016x, if you want to change the planer support of sketch then first you have to create the sketch with default planar support and exit the sketcher app and then you can modify the planar support.

  In CATIA V6 R2017x, you can select the planar support before switching the sketcher app.