Hole Making Operations
(CAM Manager) Operations 
2X
Mill (Part Level)
Hole making includes operations such as drilling,
boring, reaming and tapping. Hole
geometry can include arcs, circles and cylinders. In CAM Hole Feature
Sets, the hole depth is obtained from hole feature attributes.
The depth may also be over-ridden for individual operations. The top of each hole is obtained from the geometry used to define the hole feature. Both 3 and 5 axis hole making is supported.
These tool path operations use the following:
Frames and speeds
Optional collision checking
Selectable hole ordering methods
Dwell time and approach distance
Depth and depth reference at tool tip or tool shoulder (the centering operation depth reference is always the tool tip)
User definable cycles for output
Sample Hole Making Operation
How
to Define Hole Making Operations
In the CAM
Plan Manager, right-click on Operations,
select Insert and then select
the hole making operation from the form provided. The
operation will be added to the manager tree.
Select Parameters
under the operation you just added and set them using the definition form
provided. When
you're done pick Accept. Each
operation uses a unique definition form. They
are shown below for each operation type. See
Hole Making Operation Form Parameters for a definition
of each parameter.
Notice that (undefined) is
shown next to Features under the
hole making operation you just added. This
means that no hole features are yet defined for the operation.
Your CAM features (once you define
them) are listed under the Geometry
section of the manager tree. Under
Geometry, find the CAM component
(i.e., part : name)
and expand it (i.e., select 
to the left of the part)
to list the CAM features currently defined for that component and select
one. It
will now be listed under Features
for the hole making operation you just created. The (undefined)
flag will be removed.
To create a new CAM feature: Again, under Geometry
right-click on the CAM component, select Add
Feature and follow the forms and prompts. You
will be prompted to select geometry from the graphics window.
|
Based on the tools available to the active CAM plan, VX CAM will automatically calculate hole data from a part or cam surfaces if there are no CAM hole features referenced by the operation. If there are hole features referenced by the operation, only those holes will be machined. |
The center hole operation is used to provide starting holes for other drilling operations.
The drill operation is the primary hole making operation. It is used to drill basic holes.
The peck-drill operation is a deep drilling method. The drill withdraws to the approach plane after advancing a specified distance into the hole, facilitating chip removal.
With a chip-break operation, the drill withdraws a specified distance after advancing into the hole to prevent the binding of chips.
Use the bore operation to enlarge, finish and accurately locate holes.
With a fine bore operation, the boring bar enters the hole off-center, centers and bores from the bottom of the hole upward, avoiding drag marks along sides of the hole.
Use the ream operation for finishing by removing a small amount of material from a pre-drilled hole.
Use the tap operation to cut threads in a hole.
Use the counterbore operation to spot-face, making room for the heads of bolts or screws, or to enlarge holes.
Use the countersink operation to machine a cone shaped enlargement at the top of a hole.
The subtypes used for hole making
are "standard" and "access hole." The
selection of any other subtype (or none) will have the same result as
specifying "standard."
ALL
hole making operations can use the "access hole" subtype,
and use a reference operation for locating those holes. If a reference
operation is specified, the "access hole" subtype will
be assumed. If the operation is for access holes, the depth reference
is assumed to be "tip." The depth of access holes is
always obtained from the reference operation's tool path.
All part and stock geometry in
the feature list is always checked for potential collisions with the tool.
Gouging and collision with all geometry including clamps will be corrected
if the "Collision Check"
field on the operation definition form is set to yes.
The hole start point will be
adjusted automatically for stock in the feature list.
The following constraints are adhered to during hole making operations:
Threaded holes will not be machined whose
tool diameter is equal to or larger than the hole diameter.
Tapped holes will not be machined if the hole diameter is equal to or larger than the tapping tool or if the pitch of the tapping tool and the hole do not match.
