3D Modification

Imprint

Ribbon : Modify | 3D Modifications | Imprint

Default Menu : Draw | 3D Object | Imprint

Palette : 3D Model | 3D Object | Imprint

The Imprint- tool will sweep a 2D profile through a 3D object, combining or subtracting the volumes of the extrusion and the primary solid.

Example

Set the view to Isometric South East, then draw a 3D Box measuring approximately 80 x 100 x 50.

Use Workplane by Facet to place the workplane on the top face of the box.

Draw a rectangular profile on the top edge similar in size to that shown below from World Plan view, left image, and Isometric South East view, right image.

Select the Simple Extrude Draw | Draw 3D tool, then right click in the workspace and apply a draft angle of 15º from the Simple Extrude shape options.

The Imprint-Add function is used to extrude the profile through the box.  This will combine the volumes of the box and the extrusion, shown below right.    

 

Imprint – Add

Select Modify | Imprint, then select the top planar facet of the solid, shown below.

Box and 2D Profile drawn on top face

Select the Add option from the options menu at the bottom left of the workspace, then select the profile.

TAB to the Height field and input a value of -50 to extrude the profile below the Workplane. Press enter.

The volumes of the Box and the extruded profile will be combined, shown below.

2D Profile extruded downward by 50; volume of box and extruded profile combined. 

Imprint – Subtract

In the example below, this exercise is repeated, this time using the Subtract option. The volume of the extruded profile is subtracted from the Box.

Profile imprinted through the solid, subtracting the volume.

 

Imprint – Top-Bottom Options

The top and bottom edges of the extrusion can be blended, chamfered or created with a dimple sheet material. 

Imprint withBlock

A Block insertion can be used as the profile to imprint through a solid. The unexploded Block maintains an associativity with the solid through which it is imprinted, updating the solid when the Block is updated.

Example

In the example below, a cylinder is drawn as a solid primitive.

Cylinder drawn as solid primitive

A Block pattern will be inserted onto the bottom face of the cylinder, then imprinted through the solid, subtracting material during the imprint.

Take Note

When Blocks are inserted from the Blocks palette as imprint profiles, they can remain in the workspace as ‘unexploded’

In the example below, the unexploded Block is shown on the bottom face of the cylinder. This pattern was inserted into the workspace from the Blocks palette.

Profile inserted from the Blocks palette, unexploded.

Select Modify | Imprint, then select the bottom planar facet, shown below.

Selecting the planar facet

Select the Block insertion profile as the 2D entity to imprint through the cylinder.

From the options menu on the Status bar at the bottom left of the workspace, select the Subtract option, then extrude the Block profile through to the top of the cylinder, shown below.

Imprinting the Block through the solid

The result is shown below.

When an unexploded block is used as the imprint profile, the profile retains its associativity to the solid through which it is imprinted.

In the example below, the Block is edited using the Edit Content option in the Blocks palette and saved in its new configuration, shown below.

Block updated using Edit Content

When the Finish Edit Content option is selected, indicating that the newly modified Block should be updated, the solid through which the Block profile was imprinted is automatically updated, shown below.

Associativity retained between Block and cylinder

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.

Worked Example

In this example, a cylinder with a radius of 10 and a height of 50 is drawn, shown below.

Select the Thread tool from the 3D Modify menu and select the Simple option, shown in the menu above.

Input 3 into the Pitch field, then select the top face of the cylinder shown below left.

Next, select the cylindrical body of the cylinder shown above right.

Now use the cursor to indicate the approximate threaded length similar to the illustration below.  In this example, a threaded length of 30 was used.

The result is shown below.

In this example, a thread will be added to the interior of the cylinder shown below.

Turn the view to Isometric South East and display the Workplane. Both options are available by right clicking in the workspace.

A 2D Rectangle Draw | Draw 2D | Line | Rectangle is drawn to size 30 x 20.  A Double Point circle Draw | Draw 2D | Circle/Ellipse | Double Point Circle was then inserted  using the midpoints of the edges of the rectangle.  The circle was changed to a radius of 5 using the Selection Info Palette Tools > Palettes > Selection Info

The Simple Extrude tool using the Compound Profile option was used to create an extrusion of 10, automatically subtracting the volume of the circle, shown below.

Simple Extrude using compound profile option to subtract the inner volume

Select the Thread Modify | Thread tool and activate the Simple Select option from the Status Bar at the lower left of the workspace. option.  Set the Pitch to 2 then select the top planar face of the combined solid, shown as point 1 below, then the exterior surface of the cylinder, shown as point 2 below.

Drag the cursor upwards to get a visual representation of the thread using the temporary measurement as a guide. In this example, a measurement of 6 is input into the Height field to produce the result shown below right.

The Selection Info palette is used to modify any component of the new thread.  For example, the compound solid has been selected, shown below and each component in the Part Tree retains its original design parameters.

Any value can now be updated in the Part Tree fields and such changes will automatically be reflected in each modified component.

In the example below, the part is selected and the Thread Length is modified.

Using the Selection Info Part Tree to modify the thread properties

Section

Ribbon : Insert | Section

Default Menu : Modify | Section

Palette : 3D Model | 3D Object | Section

A closed polyline or similar contour can be used to section a solid object.The profile of a revolved surface can be used to create a section through a solid.

Half Sectional View

A half sectional view, shown below right can be obtained from a 3D solid by removing the front quarter.

Original Box

Closed polyline creates the section

Half sectional view created 

 

Full Sectional View

A full sectional view is shown below.

Section by Closed Polyline

This 3D Modify feature creates a cut section through an object, in a similar manner to the Slice feature.

A closed polyline can be drawn to define the sectional plane.

 

Example

In the example below the closed polyline contour which was used to create a revolution to produce the solid shape, has been used to define the sectional plane of the solid.

The section shown below has been removed from the solid as a separate portion. 

Associative Sections

Two local menu options 2D section by closed polyline and Associative Section were added to the Section tool.

If the option Associative Section is enabled, then the section created will be associated with the section polyline and the 3D object. This is, with the changes made in the associated Polyline or the 3D object, the section created will also be updated.

 

EXAMPLE

In the example below a closed 2D Polyline, show in green is drawn as an intersecting plane through a box.

In the diagrams below, the box in sketch 1 is shown in a different perspective to show the cutting plane represented by the closed polyline.

In point 2, the Associative Section using the 3D Section by Closed Polyline is used to create

In point 3, the Associative Section using the 2D Closed Polyline is used.

TAKE NOTE

The plane, shown in point 3 above, is represented as a physical object which can be selected and updated independently.

 

Holes

Ribbon : Modify | 3D Modifications | Hole

Default Menu : Modify | Modify 3D Object | Holes

Palette : 3D Model | 3D Object | Add Holes

This tool allows the creation of a predefined hole which automatically adds or subtracts the hole material from a solid.A point is used to place a single or multiple hole.

Example

A shape similar to the illustration below was used, drawn from a 2D Polygon, then arcs were inserted onto the vertices.

Construction circles were used which were then used to position Points.

The sketch was extruded to a depth below the Workplane.

The Add Hole tool was used to create simple holes in the solid which subtracted the material from the solid, shown below.

The result is shown below.

The Selection Info Palette is used to select one hole for modification, shown  below.

In the example below, the diameter of the selected hole was reduced by half.

Selection Info palette used to modify size and properties of holes

Custom hole 

Modify | 3D Modifications | Add Holes

The option Custom is available as a Hole type in the property page of the Hole tool in the Selection Information palette.

The custom hole is based on a block. Block content is used as a body to create a hole or boss. The middle of the top or bottom of the block bounding box is used as an anchor point. If the “Use Block Reference” option is switched on, the block ref point is used as an anchor point.

See Also

Imprint with Block