Thread

In this Task 

A plate will be drawn, then a simple thread will be added.

Associated Tasks 

Creating a compound profile extrusion.

Moving the position of the plate to the center base point of the door handle.

Using the Selection Info palette to change the radius of a circle.

Mirroring a circle to the opposite side of the plate.

Before you Start 

Turn the view to World Plan view. Workplane is set to Plane by World.

The plate will be drawn as a rectangle, then extruded to create a thickness of 5.

Make sure the Workplane is set to Plane by World and is seated on the base of the object, shown below. Use Workplane Origin or Workplane by Facet to do this.

Take Note

The rectangle will be drawn anywhere in the editor, then assembled onto the original construction circle center point.

The Form Building Edges display was removed for this task for illustrative clarity.

Menu options for the Default menu and workspace, the Ribbon and Palettes are provided directly under the Command Name heading.

 

Thread

Ribbon : Modify | 3D Modifications | Thread

Default Menu : Modify | Modify 3D Objects | Thread

Palette : 3D Model | 3D Object | Thread

This tool applies a thread to a cylindrical face of an object by defining the pitch and the length of the thread.Internal threads can be created when a cylindrical shape is subtracted from the body of a solid.The Part Tree retains the individual history of both the thread and the cylinder and can be modified by means of the Selection Info Palette.

Turn the View to World Plan view.

Somewhere in the workspace, draw a simple 2D sketch rectangle to 110 x 170, shown below.

Move this rectangle to the vertex of the original polyline, shown below.

Insert a Double Point Circle, using the midpoint of the edge of the rectangle and the vertex point at the edge of the circular door handle, shown below.

Select the new circle, then use the Selection Info Palette to change the radius of the newly drawn circle to 5.

Turn the view to Isometric South East.

Use the Mirror Copy tool to mirror the circle to the opposite side of the plate. Use the midpoint at the vertical (long) edge of the plate as the first point of the mirroring axis, shown below.

Use the midpoints at the edges of the rectangle as the mirror axis for the circle

Simple Extrude

Ribbon : Draw | Draw 3D | Simple Extrude

Default Menu : Draw | 3D Object | 3D Profile Based | Simple Extrude

Palette : 3D Model | 3D Object | Simple Extrude

This extrusion tool sweeps a 2D profile in a plane perpendicular to the workplane to create a 3D object.

 

Select the Simple Extrude tool and select the Compound Profile Extrusion option.

Select the rectangle, then hold down the SHIFT key and select the 2 interior circles, shown below. 

Extrude this to a depth of -5, shown below.

Thread

Ribbon : Modify | 3D Modifications | Thread

Default Menu : Modify | Modify 3D Objects | Thread

Palette : 3D Model | 3D Object | Thread

This tool applies a thread to a cylindrical face of an object by defining the pitch and the length of the thread.Internal threads can be created when a cylindrical shape is subtracted from the body of a solid.The Part Tree retains the individual history of both the thread and the cylinder and can be modified by means of the Selection Info Palette.

Select the Thread tool from the menu options above, then select the Simple Thread option from the bottom left of the editor.

Select the planar facet on the top side of the plate, shown below.

TAB to the Pitch field and input 1.5 then select either cylinder on which the thread should be created, shown below left.

Drag the cursor downwards to define the height of the thread, or TAB to the Length field and input 5.  The result is shown below right.

Repeat this by creating a thread on the opposite side of the plate so that the result is similar to the illustrations below. 

Inserting a Symbol from theLibrary Palette

Ribbon : Tools | Palettes | Library

Default Menu : Tools | Palettes | Library

A Symbol is a compound entity which can be inserted into any drawing from the Library Palette and is sourced from an external folder.The Symbol is inserted into the editor as a compound object (Block) and is required to be exploded if modifications to the symbol are required.

In the example below, the Screw_1 symbol was selected from the Library palette 3D Symbols Fasteners folder.

Inserting a symbol from the Library

The symbol was manipulated onto the correct face using Assemble by Facet, then assembled onto the profile to appear in a more accurate position. Assemble by 3 Points was used do this.

This part was then mirrored across the longitudinal axis of the plate to create a duplicate.

This part was inserted for illustrative reference only.