Move/Copy part entities in a linear direction at a specified distance.  This command can be used to rotate entities (Distance = 0).  All sketch copies will be locked using this command (see CAD Tips & Techniques for more about copying sketches).  Use the Copies option to make more than one copy at a time.     

 

 

Required Inputs

 

• Entity - Select the entities to move.

• Direction - Select the move direction.  You can select an edge to indicate the direction or right-click to select from the Input Options Menu.

• Distance - Enter the distance (positive or negative) along the move direction or drag the entities to the desired location.

• Angle - Enter the rotation angle about the move direction.

 

 

Optional Inputs (Copy Only)

 

• Copies - Make additional equally spaced copies.  Enter the total number of copies.

 

 

 

Move/Copy part entities from one point to another.  All sketch copies will be locked using this command (see CAD Tips & Techniques for more about copying sketches).  Use the Vector options to modify the alignment of the new copy(s).
 

 

Required Inputs

 

• Entity - Select the entities to move.

• From point - Select a reference point to move from.

• To point - Select a destination point to move to.

 

 

Optional Inputs

 

• 1st vector, 2nd vector - Modify the alignment while moving or copying. Reference and destination vectors are used to define the alignment. Select the reference vectors.

• Group  connected faces - When moving faces, check this box to group (i.e., sew) all connected faces (that are moved) into a single shell. Otherwise, the moved faces will be disconnected.

 

 

 

Move/Copy part entities by aligning one reference frame (datum plane or planar part face) with another.  All sketch copies will be locked using this command (see CAD Tips & Techniques for more about copying sketches).

 

 

Required Inputs

 

• Entity - Select the entities to move.

• From frame - Select a reference frame (datum plane or planar part face) to move/copy from.

• To frame - Select a destination frame to move/copy to.

 

 

 

Move/Copy part entities along a curve path.  All sketch copies will be locked using this command (see CAD Tips & Techniques for more about copying sketches).  The command options can be used to orient the entities during the move/copy or to apply a linear or variable scale or twist factors.

 

Required Inputs

 

• Entity - Select the entities to move or copy.

• Path - Select a point near the starting end of the sweep path.  The path can be a sketch, curve, edge or a curve list.  Refer to the Notes section below.  Remember that the move or copy starts at the end of the path nearest where it is selected.  Refer to the preview echo to see the results.

• To points - Select the destination points along the sweep path to move or copy to.

 

 

Options Tab (Frame)

 

Frame

This option defines the reference frame used during the move or copy.  The reference frame can be a datum plane or a part face.  The direction of the X and Z axes of the reference frame are controlled during the move or copy by the X-Orient and Z-Spine options respectively (see below).

 

• Natural - The default reference frame of the profile or entity is used to control the move or copy along the curve. It begins at the start of the curve path.

• At Path - The frame is built at the start of the sweep path.

• Selected - You are prompted to select a datum plane or part face whose default reference frame will be used to control the move or copy.  The reference frame and the entities are theoretically joined as a rigid body.  The reference frame is then moved or copied to the start of the curve path.

 

Frame

If the Selected method (see above) is used, pick the Define icon and select the datum plane or part face whose reference frame to use.

 

 

Options Tab (Z-Spine)

 

Z-Spine

Use this option to control the Z axis direction of the reference frame during the move or copy.

 

• Natural - A straight line is used if all of the profiles are in parallel planes.  If not, a simple spine perpendicular to each of the profile planes through the centroid of the profile is used.  No additional inputs are required.

• Spine - The Z axis remains tangent to a spine curve.  The spine curve can be any existing curve or face edge.  Use the Curve option below to select the spine curve or face edge.

• Parallel - The Z axis remains perpendicular to an existing plane.  This forces the profile plane to remain parallel with the existing plane.  Use the Plane option below to select the normal vector of the parallel plane.

 

Curve

Select the spine curve or face edge. This option is use with the Z-Spine / Spine option above.

 

Plane

Select the normal vector of the parallel plane.  This option is use with the Z-Spine / Parallel option above.

 

 

Options Tab (X-Orient)

 

X-Orient

Use this option to control the orientation of the X axis of the reference frame during the move or copy.

 

• Natural - The X axis is constrained to minimum rotation. No additional input is required.

• Guide Plane - The X axis stays "in" an existing plane. It is perpendicular to the plane normal.  Use the Plane option below to select the normal vector that defines the direction of the guide plane.

• X-axis Curve - The X axis is projected and follows the intersection of an existing curve or face edge.  Use the Curve option below to select the X axis curve or face edge.

 

Plane

This option is only used with the X-Orient / Guide Plane option above.  Select the normal vector that defines the direction of the guide plane.

 

Curve

This option is only used with the X-Orient / X-axis Curve option above.  Select the X axis curve or face edge.

 

 

Advanced Tab (Scale/Twist)

 

Scale/Twist

Use these options to apply scale and/or twist to the entities as they are moved or copied along the path.  Each is applied in a similar manner.

 

• None - No scale or twist is applied.

• Linear - The scale or twist factor is applied as a linear uniform function starting and ending at the values you specify on this tab.  Scale is an absolute value.  Twist is measured in degrees.  Positive values will twist counterclockwise.

• Variable - The scale or twist factor is applied non-uniformly based on attributes attached to the drive curve (see above) using the Add, Modify, and Delete buttons discussed below. The scale or twist factor will match the attribute value at that point on the drive curve and blend smoothly between attributes.
  
  If only one attribute is placed on the drive curve, the entire move or copy will be scaled or twisted to that value.

 

Add

Add a scale or twist attribute to the drive curve. This option is used with the Variable option above.

 

1. Select a point on the drive curve to locate the attribute.

2. Enter the scale or twist factor.

3. Repeat steps 1 and 2 until all attributes are added and then middle-click to continue.
    

Modify

Modify a scale or twist attribute currently attached to the drive curve.  This option is used with the Variable option above.

 

1. Select the attribute to modify.

2. Enter a new value (scale factor or twist degree).

3. Repeat steps 1 and 2 until all scale attributes are modified as desired and then middle- click to continue.

 

Delete

Select the scale or twist attribute to delete.  This option is used with the Variable option above.

 

 

Additional Advanced Inputs

 

Scale Type
This option is only used with Scale attributes.  Specify the axes along which the scaling should occur. Select Uniform, X only, Y only or Z only.

Make scale (or twist) locally flat
Use this option to mix constant and variable scale or twist factors along the drive curve.  Place attributes with this option checked at the boundaries of the region that should have a flat constant scale or twist factor.  This is similar to the Radius locally flat option of the Edge Fillet command.

 

 

 

Copy a root sketch and insert it into the active part. A root sketch is one that resides at the root object level like a part or Drawing Packet. The new sketch is not parametrically dependent on the root sketch from which it is copied (i.e., if the root sketch is changed, the new sketch will not).
 

Required Inputs

 

• File/Part - Select the VX file and root sketch to insert. The active file is selected by default. The list shows the root objects in the selected file.

• Preview - Sets the preview mode (e.g., Off, Graphics or Attributes) similar to the Object Browser.

• Name - Enter a name for the sketch copy. If you don't enter a name one will be assigned for you.  

• Plane - Select the insertion plane to locate the sketch (datum or face).

• Up - Select the UP direction to orient the sketch or middle-click to accept the default direction.

 

Optional Inputs

 

• Origin - Specify the XY origin of a sketch plane at the time it is created. Select a point to define the XY origin of the sketch plane or middle-click to accept the default origin of the selected plane.

 

 

 

Use this command to copy an external part and then insert it into the active part as a shape.  Select a part using the Object Browser and then specify an insertion point.  The shape is associated with the part from which it is copied.  This is similar to inserting a component.  If the source part is modified, the shape is also modified the next time the active part is regenerated.

 

Required Inputs

 

• File/Part - Select the VX file and part to copy. The active file is selected by default. The list shows the root objects in the selected file.

• Preview - Sets the preview mode (e.g., Off, Graphics or Attributes) similar to the Object Browser.

• Location - Select an insertion point. If you right-click and select Critical as the input option, and then press F7, you can snap to critical points on existing components.

 

Optional Inputs

 

History - Use this option to determine how should the copied history of the external part should be handled.  Select from the following options.

 

• Sub-Part - Copy non-native data into the active part as a sub-part.  In the active part's history, the sub-part is followed by an operation that merges the sub-part data into the active part.
   

• Backup - Copy non-native data into the active part and automatically insert a "Backup" operation in the active part's history.
   

• Encapsulate - Copy non-native data into the active part and then automatically "encapsulate" the active part's history.  Regenerating the active part restores a static copy of the encapsulated data, followed by a step-by-step regeneration of history operations added after the history was encapsulated.
   

• Import - Copy non-native data into the active part and put a regenable "Import" operation in the active part's history.   The file is re-copied every time the history is regenerated.

 

 

 

Use this command to copy geometry from the active part to a destination part (new or existing). You can use the "Extract as component" option if you want the geometry instanced into the part as a component.

 

An "import" feature is logged in the destination part that "pulls" user-selected geometry from the active part. Future regenerations of the destination part will re-import the geometry. If the destination part is new, its default geometry tolerance is changed to match the geometry tolerance of the source part.

 

 

 

Required Inputs

 

• Geometry - Select the geometry to copy. The pick filters include shapes, faces, edges, curves and points.

• File/Part - Specify the existing or new destination part to receive the copied geometry. You can enter the part's "file/name" in the text input field or select it using the folder icon. If you don't select a part or enter a new part name, a new root object will be created and you'll be asked if you want to instance it back into the active part as a component.

• Preview - Allows you to preview a selected part's graphics or attributes similar to the Object Browser and Root Object Browser.

 

 

Optional Inputs

 

• Frame -  The geometry is positioned such that the reference frame is aligned/coincides with the destination part's world axis.  Select a datum plane, planar face or sketch in the active part.

• Destination - This option is applied to the history of the destination part after the specified geometry is imported into it. "Encapsulate" is the default option, which avoids a history link between the destination part and the parent part.  If you're a history-savvy user you can choose the "No Action" or "Backup" option if you want an associative link between the parts.
  
  The "Backup" option will include a Backup feature in the destination part, after the import feature. If regeneration of the geometry import feature fails, it can be suppressed and the original geometry can be recovered from the backup feature.
   

• Extract as component - Use this option if you want the geometry instanced into the part as a component.

 

 

 

When you have a component within an assembly activated for editing, you can use this command to copy other components into the active part as shape geometry.  You can only copy a component that is selectable within the active assembly.  The shape geometry will update if the source component is modified.  

 

Shapes, faces, edges, curves, and points (see the filter associated with the command) can also be copied from an assembly component into the active part, not just the entire component.  You cannot select a part external to the assembly.  Use the Copy External Part command (see above) to perform that function.

 

 

 

 

• About Copying Sketches (see CAD Tips & Techniques).

• Assigning Names to Features (see CAD Tips & Techniques).

• The total number of copies echoed will depend on the Accuracy/Speed setting of the Echo Attributes Form. Select Attributes > Echo to display this form.

• During Path input, you can right-click and select Make Curve List from the Input Options Menu. This will allow you to make a parametric list of existing curves to use as input for this command.