Profile Based Extrusions

Extrusions produce a 3D solid from a 2D profile by ‘sweeping’ a profile to a height or depth.

The profile to be extruded must be on the WorkplaneThe resulting shape of the extrusion can be set before using the Extrude options or the Properties page.The resulting shape of the extrusion can be modified after the extrusion using the Selection Info Palette.Some extrusion options are shown below.

SimpleExtrude

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.

A bi-directional extrusion can be created which creates an above and below Workplane extrusion, shown below right.

When an open profile is selected for extrusion, the resulting shape is a surface object.

2D profile on Workplane

Extrusion created perpendicular to Workplane

Bi-directional sweep creates an above and below Workplane extrusion 

Extrusion Shape

Ribbon : Draw | Draw 3D | Simple Extrude

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

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

(right click to display options or selection options from status bar at the base of the editor)

The shape of an extrusion can be modified by using a draft angle to produce a tapered extrusion.

Extrusion shapes are produced when using the Simple Extrude tool.

Worked Example

Set the view to Isometric South East. Draw a rectangle which measures approximately  50 x 100 in the workspace.

Select the Simple Extrude tool, then right click and select Properties.  In theExtrusion Shape field, input a draft angle of 30.

Select the rectangle and create an above-Workplane extrusion of approximately 50, shown below.

Select the solid, then open the Selection Info Palette and change the Draft Angle to -15.

By inputting a negative value into the draft angle field, the extrusion will taper inwards, shown below

Two Sided Extrusion

Ribbon : Draw | Draw 3D | Simple Extrude

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

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

(right click to display options or selection options from status bar at the base of the editor)

An above and below Workplane extrusion of a 2D profile can be produced.

The extrusion of the profile will be equal either side of the Workplane.

In the example, below, the total height of the extrusion is 50, therefore a height of 25 is given.

Extrusion Draft Angle

Ribbon : Draw | Draw 3D | Simple Extrude

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

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

(right click to display options or selection options from status bar at the base of the editor)

A draft angle can be applied to an extruded object to create an extrusion taper.

Draft angles can be applied to all extruded profiles, such as a cylinder, polygonal prism, etc.

Worked Example

Draw a circle to a radius of 45 on any layer

Select the Simple Extrude tool, then right click in the workspace and select Properties.

Select the Extrusion Shape page, then apply a draft angle of 5º, shown below.

TAB to the Height field and input a value of 150.  Press Enter.

 

 

Extrusion tapered by 5 degrees

Twisted Extrude

Ribbon : Draw | Draw 3D | Simple Extrude

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

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

(right click to display options or selection options from status bar at the base of the editor)

The Twisted Extrusion tool extrudes a profile perpendicular to the Workplane to create a solid object, allowing modeling features such as twisting and tapering to be created.

This extrusion tool can create a bi-directional above/below Workplane extrusion and modeling features such as a twist or taper can be applied at any position along the length of the extrusion.

The Selection Info Palette is used to modify the individual modeling features of the extrusion.

Worked Example

In this example, the view is set to Isometric South East. Right click in the workspace and select this option from the menu.

The Selection Info palette is activated and seated at the right edge of the workspace. Use Tools | Palettes | Selection Info to find this palette.

A 2D Polygon Draw | Draw 2D | Line | Polygon is drawn using the measurements shown below. The Polygon is set to Segment mode, see option below shown by the arrow.

Drawing a polygon in Segment mode

An initial extrusion height of 100 with a twist of 90º starting from the bottom of the extrusion and ending halfway up the extrusion will be produced, similar to the illustration, below.

Select the Twisted Extrude tool from the Draw | Draw 3D menu, then right click and select the Properties menu. Select the Twisted Extrude shape option from the left panel, then apply the following settings.

Close the Properties dialog box, select the polygon, then TAB to the Height field and input 100, press enter.

Next, a draft angle (extrusion taper) of 15º will be applied from the top of the twisted portion (50) to the top of the extrusion (100)

Select the extrusion, then select the Twisted Extrude options in the Selection Info palette shown by the arrow below.

Updating the extrusion shape using the Selection Info palette

Next, the Selection Info palette will be used to create an extruded rod with a twist midway up the extrusion.  The extrusion height will be changed to 90, with the twist starting at 30 and ending at 60.  The twist angle will be set to 90º, shown below.

The result is shown in the illustrations below.

Extrude to Face

Ribbon : Modify | Modify 3D | Extrude to Face

Default Menu : Modify | Modify 3D Object | Extrude to Face

Palette : 3D Model | 3D Object | Extrude to Face

(right click to display options or selection options from status bar at the base of the editor)

This extrusion tool allows selected faces of solids to be extruded so that they intersect the face of the selected body, either adding or subtracting material during the extrusion.

Two faces can be extruded bi-directionally by selecting 2 faces in the same plane.

Worked Example

In this example, a 3D Box to measurements 100 x 80 x 20 has been drawn, then shelled out by creating an inner wall thickness of 2.  The top and bottom faces were excluded from the shell function, shown below.

A smaller profile has been drawn and placed in the interior of the box and a simple extrusion of 2 has been provided for the smaller profile.

The illustrations below indicate clearly the position of the smaller solid in relation to the main solid body.

Top / World Plan View

Side View

Front View 

The Boolean Add function shown above is the default option for the Extrude to Face tool .

To extrude the profile shown below so that it intersects with the body of the box and combines (3D Adds) its volume with that of the primary solid, select the Extrude to Face tool from the 3D Object menu.  Select the indicated face, then select the box.

The result is shown below.

Extruding 2 Faces

Two faces in the same plane can be extruded bi-directionally to extrude opposing faces to the body of the solid.

In this example, both sides of the smaller extrusion were selected using the SHIFT tool.

Both faces were then extruded bi-directionally using the default Add option to combine the volumes of the shapes, shown below.

Using the Subtract option

In this example, the Subtract option was used to create an extrusion of the face shown below to the body of the primary solid.

The result is shown below.

Sweep

Ribbon | Draw | Draw 3D | Sweep

Default : Draw | 3D Object | 3D Profile Based | Sweep

Palette : 3D Model | 3D Object | Sweep

This extrusion tool sweeps an open or closed 2D profile along a predetermined path defined by another 2D profile.

The extruded profile can be tapered or twisted.

Worked Example

A 2D polygon was used to create the profile and a 2D polyline was used to create the path.

In the illustration, below left, the hexagonal profile lies in a perpendicular plane to the profile.

When using the Sweep tool, the path is moved to the profile and the profile is forced along the path.

Profile and path

Path moved to profile

Result

Rail Sweep

Ribbon | Draw | Draw 3D | Rail Sweep

Default : Draw | 3D Object | 3D Profile Based | Rail Sweep

Palette : 3D Model | 3D Object | Rail Sweep

Sweeps an open or closed 2D profile along a predetermined path defined by another 2D profile.

The profile and path do not have to lie in the same plane.

The extruded profile can be tapered or twisted.

Worked Example

In the illustration, below left, the hexagonal profile lies in a perpendicular plane to the profile.

When using the Rail Sweep tool, the profile is moved to the path and the profile is forced along the path.

Profile and Path

Profile moved to Path

Result 

Compound Profile Sweep

Ribbon | Draw | Draw 3D | Rail Sweep

Default : Draw | 3D Object | 3D Profile Based | Rail Sweep

Palette : 3D Model | 3D Object | Rail Sweep

Sweeps a connected 2D profile or a closed profile with interior regions along a predetermined path defined by another 2D profile.

When a compound profile consists of an outer profile with an inner region, the volume of the inner region will automatically be subtracted from the volume of the sweep extrusion.

The extruded profile can be tapered or twisted and the corners of a bended extrusion can be crimped or blended.

The Selection Info Palette can be used to adjust any properties of the resulting extrusion.

Worked Example

Draw a similar sketch to the illustration below, adjusting the Workplane accordingly.

Select the Sweep tool from the 3D Objects toolbar, then select the Use Compound Profile option, shown top.

Select the rectangle, then hold down the SHIFT key and select the inner circle.

Select the polyline as the sweep path.  The result is shown below.

Use the Selection Info Palette to adjust the properties of the extrusion shape.  An example is shown below.

Wire Wrapping

Ribbon | Draw | Wire Wrap

Default : Modify | Wire Wrap

Palette : 3D Model | 3D Object | Rail Sweep

The Wire Wrap tool allows a 2D sketch object to be wrapped around a 3D solid object by defining the target face, shown below left and a wrap direction (axis) A start and end point can be given on the target face.

Target face shown on solid object, left; 2D object (line) wrapped around object from top to bottom

Quick Pull

Ribbon : Modify | 3D Modifications | Quick Pull

Default : Modify | Modify 3D Objects | Quick Pull

Palette : 3D Model | 3D Object | Quick Pull

This tool allows for the planar extrusion of a face of a solid, either as a quick modeling function, or by a specific extrusion height/depth.

The integrity of the original object can be maintained by selecting the Always Create Solid option from the status bar at the bottom left of the workspace.

Modeling features such as draft angle, fillet blends and chamfers can be applied to the new extruded face.

The Part Tree Activated using Options | ACIS | Create Editing History, then displayed in the Selection Info palette after the object is selected. records all extrusions created using Quick Pull tool as an Imprint and allows future modifications to be done using the relevant Part information in the Selection Info Palette.

This tool allows for dynamic switching between Quick Pull and Imprint modes.

Worked Example

Display the Workplane and set the view to Isometric South East. These options are activated by right clicking in the workspace.

Draw a Box Draw | Draw 3D | Box to measurements100 x 80 x 50, shown below.  The face shown shaded will be extruded to an additional outward distance  of 40.

From the Modify | 3D Modifications menu select the Quick Pull tool, then right click in the workspace and select the Properties page. Set the draft angle to 0 degrees in the Simple Extrude shape options, shown below.

Click Ok to exit the Properties sheet, then select the indicated face, shown below. The Workplane will automatically align to the selected face.

TAB to the height field and input a value of 40.

Next, a tapered extrusion of 15º will be applied to the face indicated below, with a new extrusion distance of 40.

Select the Quick Pull tool, right click and apply a draft angle of 15º in the Extrude Shape options.

Select the face shown above and extrude to a new outward distance of 40 so that the result is similar to the illustration, below.

New extruded face showing a draft angle of 15° 

 Using thePart Tree to modify a Solid

In the illustration below, the part has been selected and the information presented in the Selection Info Palette as Part Tree components.  In this example, the tapered extrusion is shown  selected and highlighted as point 1 in the illustration below.

Using the Part Tree in the Selection Info palette to modify the part

A Fillet with a radius of 15 can be applied to the top edge of the new tapered extrusion by modifying the data in the Selection Info Palette, shown by point 2 in the illustration above. See below the illustration for rendering information.

Part rendered with ACIS Degenerative Faceting Options | ACIC | Degenerative Faceting activated.

Rendering done using Quality Render with Foreground Wireframe Right click in the workspace. Right click on the Quality Render tool. Activate Foreground Wireframe ‘non-renderable’ and ‘renderable objects’ options. set to ‘non-renderable objects’ and ‘renderable objects’

Lofting and Prism tools

These profile-based tools create a solid shape when uniquely shaped profiles on different elevations are connected by their vertices to form a solid object.

The resulting shape will be drawn on the currently activated layer, irrespective of the layer of the profiles.

Prism

Ribbon : Draw | Draw 3D | Prism

Draw | 3D Objects | 3D Profile Based| Prism

Palette : 3D Model | 3D Object | Prism

This tool creates a lofted shape from 2 profiles in different planes.

In the illustration below left, 2 profiles line in a parallel plane. When the Prism tool is used, both profiles are connected by their vertex points.

Prism tool connects objects in a parallel plane by their vertex points

Lofting

Ribbon : Draw | Draw 3D | Loft

Default : Draw | Profile-based | Loft

A solid shape is created when uniquely shaped profiles on different elevations are connected to form a solid object. This is referred to as a Loft.  The resulting shape will be drawn on the currently activated layer, irrespective of the layer of the profiles.

The 2D profiles are connected using NURB calculations – Non-Uniform Rational B-Spline and the resulting shape can be altered after lofting by modifying the individual profiles.

A perpendicular, straight edgedloft is created when connecting 2 profiles. When connecting 3 or more profiles, a curved loft is produced.

Different solids are produced by selecting the profiles in different sequences.

Lofted profiles always produce a 3D Solid. Boolean functions, including the Round Fillet Edges and Shell feature can be performed on Lofts but the properties cannot be changed from Solid to Surfaces.

The construction profiles of Lofts can be edited using the Edit tool, but not individual nodes of the resulting surface.

Unlike the Prism tool, Lofting can be performed on open or closed Polylines.

Example

When creating a loft, 3 profiles, similar to those shown below, should be on different elevations. Draw the profiles, then turn the view to Front and move the profiles to different elevations in the workspace.

When selecting the loft sequence from bottom to top, the resulting shape, shown below is produced.

2D profiles, similar to those shown below left, which reside on different elevations can be lofted to produce a lofted shape, shown below right.

Branched Lofting

The Branched Lofting tool creates a solid object by creating transitional tubing between objects which form a trunk and a branch.

Worked Example

In the illustration below left, the central profiles form the trunk and the side profiles form the branches.

Profiles from Front/Side View

Slightly tilted view achieved by holding down the mouse wheel and moving the cursor

Isometric View

Trunk and branches lofted 

The trunk profiles were selected from bottom to top, then the branch profiles were included by selecting the smaller profile first.

The result is shown below.

Face2Face Lofting

Produces a transitional connection between the faces of 2 existing solids.

Example

In the illustration below left, the branch profiles were used to create the new profiles which were lofted in the illustration below middle.

The Face2Face lofting tool was used to connect the faces shown in bold, in the illustration, above middle.

The result is shown below.

Surface by set of polylines

Draw | Loft | Surface by Polylines

An option Surface by Polylines is available in the Loft toolset.

This tool creates a 3D mesh (surface) from a set of polylines, arcs, and curves. The starting point of the first profile connects to the nearest starting point of the next polyline, and so on. Optionally, a smooth surface can be created along the direction of the profiles.

In the example below, the smooth surface loft was created from the profiles.

 

Skinning with Sweep Path

A local menu option Select Sweep Path is available in the Lofting toolset.

Skinning with a Sweep Path interpolates a surface through a series of input profiles along the given sweep path curve.  The input profiles are given in the form of wire bodies.

Revolve

Ribbon : Draw | Draw 3D | Revolve

Default Menu : Draw | 3D Object | 3D Profile Based | Revolve

Palette : 3D Model | Revolve

A 2D polyline can be used to create a suitable profile which can be revolved about an axis to produce a solid.If the start and end point of the polylines are collinear, then the resulting solid will be a closed, filled area.After the revolve function has been completed, the profile can be modified using the Edit Tool.  A new solid shape will be produced after the profile has been modified.

Worked Example

A 2D polyline, shown in bold, in the illustration below was used as the profile.

This profile was revolved using the end vertex as the revolution axis, shown below.

The profile was revolved through 360º to produce the solid shape, shown below.

Revolve Spiral Pitch

A 2D profile can be revolved to produce a spiral or helical shape.

This takes place when a spiral pitch and a number of coils is given.

Example

Observe the illustration below.  The rectangle will be revolved about the quadrant points of the circle, shown by points 1 and 2.

Select the Revolve tool, then right click in the Workspace and select the Revolution Shape options fro the left panel. The Spiral Pitch of the Revolve Shape is set to 30 and the number of coils is set to 5, shown below.

Click Ok to exit the Properties sheet, then select the rectangle profile. Select the horizontal quadrant points of the outer circle to produce the result shown below.

Spiral pitch set to 30 with 5 coils

Shown from Isometric South West viewpoint

Spiral

By selecting the part, shown below and using either the Properties sheet or the Selection Information palette, a spiral can be produced by activating the Spiral option shown below.

Spiral created by activating ‘spiral’ option. 

3 Coils with a Spiral Pitch of 30.

See Also

Helix

Revolve with Compound Profile

A compound profile is created from a boundary profile with interior regions which are automatically subtracted from the volume of the revolved object.

The interior regions are selected by holding down the SHIFT key to include them into the selection of the boundary profile before creating the extrusion.

Worked Example

Draw a simple rectangle with 2 concentric circles of any size, similar to the illustration below.  In this example, 2 circles were inserted onto the midpoint of the right vertical edge of the rectangle, then the 2D Boolean Add tool was used to combine their surface areas.

The resulting outer boundary of this new region was formatted into a sketch profile usingFormat > Explode.

Select the Revolve tool, then select Use Compound Profile from the options menu at the bottom left of the workspace.

Turn the view to Isometric South East, then select the outer profile, then hold down the SHIFT key and select the inner region.

Select a convenient mirroring axis, similar to the position shown below.

The result is shown below.

IMPRINT PROFILE

A pattern which has been saved in the Blocks palette can be used to add or subtract volume as the shape is extruded through a solid object.

In the example below, a pattern will be used as the imprint profile to subtract its extruded volume from a cylinder. This example uses a constrained pattern Geomemtric constraints are applied to maintain design integrity when the sketch is modified..