Loading...
MILL/TURN
Gibbs and Associates
323 Science Drive
Moorpark, CA 93021
(805) 523-0004
March, 1999
M i l l / T u r n M a n u a l |
G F K - 1 7 1 1 |
|
|
Proprietary Notice
This document contains propriety information of Gibbs and Associates and is to be used only pursuant to and in conjunction with the license granted to the licensee with respect to the accompanying Gibbs and Associates licensed software. Except as expressly permitted in the license, no part of this document may be reproduced, transmitted, transcribed, stored in a retrieval system, or translated into any language or computer language, in any form or by any means, electronic, magnetic, optical, chemical, manual or otherwise, without the prior expressed written permission from Gibbs and Associates or a duly authorized representative thereof.
It is strongly advised that users carefully review the license in order to understand the rights and obligations related to this licensed software and the accompanying documentation.
Use of the computer software and the user documentation has been provided pursuant to a Gibbs and Associates licensing agreement.
© Copyright 1998 Gibbs and Associates, Inc.
All Rights Reserved
Acknowledgements:
Written by: Shannon McConville and Wil Gaffga
Thanks to Bill Gibbs, Alvaro Martins, Jeff Castanon, Bart Ehlers, Jeff Myers, Gary Esser, Michael Kelley Charles Haden and Israel Klain for their input and assistance.
Special Thanks to Louise Burns for supplying the Clutch Basket tutorial part.
Trademarks:
Windows NT and Windows 95 are trademarks of Microsoft Corporation
Macintosh is a trademark of Apple Computers, Inc.
Printed in the United States of America
G F K - 1 7 1 1 |
T a b l e o f C o n t e n t s |
Table of Contents
MILL TURN |
II |
Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . ii Preferences . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 2 Interface . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 2
PART SETUP |
4 |
Machine Definition Documents. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 4
Coordinate Systems . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 5
Geometry Creation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16
Tool Orientation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16
MACHINING OPERATIONS |
19 |
Machining. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . |
. . 19 |
Y-axis & C-axis Interpolation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . |
. . 21 |
ROTARY MILLING & WRAPPING |
23 |
MILL/TURN EXERCISES |
26 |
Exercise 1 : Clutch Basket . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 26
Exercise 2 : Coupling . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 41
i
M i l l / T u r n M a n u a l |
G F K - 1 7 1 1 |
|
|
I N T R O D U C T I O N
The system provides for Mill/Turn capabilities when both the Mill module and Lathe module of the software are present. When this is the case, the system will have an option to designate the machine type as Mill/Turn, and the user can now apply any of the system's available milling machining processes to a lathe part. All milling and turning functions are available for Mill/Turn parts. Additional modules are available that increase the capabilities of Mill/Turn, most importantly the Rotary Milling option which provides the ability to wrap any shape or toolpath around the C axis using rotary axis interpolation.
The Mill/Turn functionality of the software provides capabilities for programming single spindle, single turret lathes that have the capability of driving live tooling. The turret positions can drive live tools such as endmills and drills which can be oriented along the Z axis, toward the chuck (face machining), or along the X axis, toward the turret (OD machining). In order to perform milling operations, the spindle must be changed from its normal function of spinning the part into a third programmable axis, usually designated as the C axis. The Mill/Turn functionality allows users to position the part by specifying angular rotations of the C axis.
Note: This symbol is used periodically in this manual to signify Mill/Turn functions that AM are enhanced by the Advanced Mill module.
The following image is intended to clarify differences between different system modules and functions.
Mill/Turn allows the user to use a live mill tool with simple angle positions of the C-axis on the OD or face of the part.
Rotary Mill allows the user to wrap geometry about the C-axis and allows continuous C-Axis rotation when programming milling operations.
If the user’s machine has Y-axis capabilities any mill operation may be performed at any C-axis position
TERMINOLOGY
Live Tool: When a live tool is used the lathe spindle stops rotating and engages C-axis rotary motion. A milling tool is set to spin at a specified RPM.
Wrapped Geometry: A standard term for geometry that is drawn flat and wrapped or rotated around the rotary axis.
ii
G F K - 1 7 1 1 |
M i l l / T u r n |
Lathe module |
Mill/Turn capability |
Rotary Mill |
Rotary Mill with Y-Axis capability |
Figure 1: A comparison of capabilities in system modules.
1
M i l l / T u r n M a n u a l |
G F K - 1 7 1 1 |
|
|
P R E F E R E N C E S
Graphics preference: The Graphics Preference which is accessed from the Preferences submenu under the File menu contains an item called Grid Brightness. This affects the contrast and brightness of the CS grid drawn on
the screen. The brightness can be adjusted by moving the slider. Clicking on the Apply Button in the Graphics Preference Dialog will apply the changes.
I N T E R FA C E
The system has three different levels of functionality, Level 0, Level 1 and Level 2, providing more advanced features as the level number is increased. All levels are available to users regardless of the specific options that are installed with the system, however certain items may not be accessible depending on the options installed. In order to use the Mill/Turn functions the user must be working with the Level 2 interface.
Each level makes slight changes to the interface. The Level 1 interface contains a 7 button Top level palette, while the Level 2 interface is characterized by a 14 button Top Level palette and a taskbar. The interface level is specified in the Interface Preferences accessed from the Preferences submenu under the File menu.
TASKBAR
When working with the Level 2 interface, there is a taskbar located along the top of the drawing window, directly below the menu bar. The taskbar contains a series of buttons which affect the drawing and selection of items in the drawing window. Each of the buttons has two states, depressed (on) or raised (off). The taskbar also contains a progress bar and message display. The progress messages indicate the function the system is performing and the progress bar gives the status of the function. The Stop button can be depressed to stop the current function. The current workgroup and coordinate system are displayed next to the progress bar. Again, certain items may be unavailable depending on the options installed with the system. There are two taskbar buttons which are used specifically for Mill/Turn parts.
Show CS Grid Button: When it is turned on, (the button is depressed), the CS grid and axis markers for the current Coordinate System will be drawn on the screen.
2
G F K - 1 7 1 1 M i l l / T u r n
Stock Cutaway: This button affects the cut part rendering function only. When turned on, the stock used for the cut part rendering will have a quarter section cut out. This is useful when rendering lathe parts which contain ID operations. When turned off, the stock used for cut
part rendering will be a full cylinder. When rendering Mill/Turn parts, it is recommended that Stock Cutaway be turned off to ensure that OD milling operations are viewed in the cut part rendering process.
Wrap Geometry: This button affects geometry creation. It is only available when the Rotary Milling option is installed. The Rotary Milling function provides continuous C axis rotation on milling operations, also referred to as wrapping. When this button is turned on, geometry
can be created and viewed radially, wrapped around the OD of the part. Rather than creating "flat" geometry using XYZ coordinates, the system allows users to create radial geometry using XZC coordinates, where X designates the radius or diameter. The user can either create flat geometry and then wrap it or simply create geometry using radial values. Any geometry can be wrapped, including lines, closed shapes and text. In order to create and view geometry radially, this button must be depressed. Effectively, geometry will be wrapped on the OD of the part. In addition, the Rotary Milling checkbox in the WG Info dialog must be checked. This issue will be discussed further in the Rotary Milling section of this manual.
HOME VIEW
The Home View is an additional view available from the Trackball that is useful when working with different coordinate systems. When selected, the system rotates the view of the part to a view normal (3D perpendicular) to the current coordinate system. The Home View always displays the part with the positive depth axis projecting out of the screen, signified by the “+” at the center of the axis markers. Using the part model on the trackball in the center of the View Control Palette allows the user to get an idea of the positioning of the plane in 3D space relative to the overall part.
Home View
Figure 2: Home View
GEOMETRY COLOR SCHEME
The system uses colors to graphically differentiate between certain items drawn on the screen. Additional meaning is added to the color scheme when working with multiple coordinate systems.
Blue and Yellow: Geometry drawn on the screen in either blue or yellow indicates that it is contained in the current workgroup and based on the current coordinate system. The current coordinate system is the coordinate system that is being worked in and is highlighted in the CS List Dialog.
Magenta: This color is added when working with multiple coordinate systems. Geometry drawn in magenta indicates that the geometry is not based on the current coordinate system. Magenta geome-
3
M i l l / T u r n M a n u a l |
G F K - 1 7 1 1 |
|
|
try can be selected, modified and used for machining operations. The color change merely indicates that the geometry was not created while working in the current coordinate system.
Gray: Geometry drawn in grey is contained in a background workgroup. It may or may not be based on the current CS. Geometry in a background workgroup cannot be selected or modified.
Part Set-Up
MACHINE DEFINITION DOCUMENTS
Setting up a mill turn part is very similar to that of a standard lathe part. The stock is designated in the same manner and the options for designating clearance planes are identical to that for turning parts. With both the Mill and Lathe modules installed, additional Machine Definition Documents (MDD’s) will be available in the Machine Type pull-down menu in the Document Control Dialog. The Mill/Turn MDD's are similar to Lathe MDD's in that different shank sizes are available.
Figure 3: New Machine Definition Documents (MDD’s) for Mill/Turn
Selecting a Mill/Turn MDD signals the system that the part will contain both milling and turning operations. When the Mill/Turn MDD is selected, the system automatically creates four coordinate systems: the XZ plane which is used for turning operations, the YZ plane, which is used for OD milling operations, the XY plane which is used for face milling operations, and the HY backside plane which represents the back face of the part. Coordinate systems can be viewed and changed using the CS list dialog which is accessed from the Top Level palette.
The Document Control Dialog for lathe and mill/turn parts contains options for programming the part using radius values or diameter values. Either is a valid selection for Mill/Turn parts. However the diameter selection will only apply to geometry and machining processes used for turning operations as noted. The ZX plane is used for all turning operations. When working in this CS, if the part is being programmed in diameter, the user can enter diameter values. In all of the other coordinate systems, which are used to create milling operations, all values will be treated as radius values regardless of the selection made in the Document Control dialog. All text edit boxes, which require
4
G F K - 1 7 1 1 |
M i l l / T u r n |
input from the user, are labeled indicating the type of value that should be entered. The labels on all text edit boxes will read Xr (for radius) and Xd (for diameter) indicating the type of value to be entered. The user should make sure the label is appropriate for the value being entered.
All other information entered in the Document Control Dialog is used as it is when programming lathe parts. For more information about the information contained in this dialog, refer to the Lathe Module manual.
COORDINATE SYSTEMS
NOTE: The terms coordinate system, plane and CS are used interchangeably throughout this manual.
When a 3 axis lathe with C axis MDD is selected, four coordinate systems are automatically created. CS’s are used to create geometry and machining operations on different areas of the part. The first is the ZX plane which is used for turning operations. The second is the XY plane which is used for face machining. The third CS is the HY backside plane which is used for machining the back face with milling operations. The final CS is the YZ plane which is used for OD milling operations. These four coordinate systems can not be modified.
5
M i l l / T u r n M a n u a l |
G F K - 1 7 1 1 |
|
|
It should be noted that the system has an additional option referred to as the Advanced AM Milling option which allows users to create and modify coordinate systems into any pla-
nar orientation and program positioning moves for milling operations. For the mill/turn capabilities the Advanced Milling option provides the ability to create additional coordinate systems in any orientation and create milling operations which will use the non-stan- dard coordinate systems for the machining CS. The four base CS’s created by the system are not modifiable by Advanced Mill.
OVERVIEW
▲ A Coordinate System is a plane in space with an origin and three axes.
The origin is the point at which the axes intersect and serves as a zero reference point. The three axes are the horizontal, vertical and depth axes. In the standard XY Plane, the X axis is the horizontal axis, the Y axis is the vertical axis and the Z axis is the depth axis. The current coordinate system is the active coordinate system that is selected in the CS List Dialog. It refers to the CS that is currently being worked in.
▲ A Coordinate System is NOT a Workgroup.
Coordinate systems are completely independent of workgroups. Multiple coordinate systems can be used in one workgroup and the same coordinate system can be used in multiple workgroups. Often times it is helpful to have one coordinate system per workgroup, however that is only a convenience, not a rule.
▲ A coordinate system is an attribute of geometry elements (points, lines, circles, etc.).
Geometry is not contained in a coordinate system the way it can be said that geometry is contained in a workgroup. When geometry is created, dimensional information must be entered to indicate where the geometry should be located. When locational data is entered, there must be a referencing system that makes the dimensional data meaningful. This is the role a coordinate system plays in the creation of geometry. When using the Mill/Turn functionality, turning geometry is created in the ZX plane and milling geometry is created in the XY plane for face work and the YZ plane for OD work.
CS LIST
Coordinate System button: This button gives the user access to the CS List Pop-Up menu and the CS List dialog. It is found among the 14 buttons in the Top Level palette.
CS List Pop-Up menu: Holding down the mouse button while selecting CS Button will bring up a pop-up menu showing all of the coordinate systems contained in the part file. The user can change the current coordinate system by selecting one from the list and letting go of the mouse button. After a coordinate system has been selected, the list will disappear.
6
G F K - 1 7 1 1 |
M i l l / T u r n |
CS List dialog: Clicking on the CS Button will bring up the CS List Dialog on the screen. This dialog displays a list of all existing coordinate systems, highlighting the current coordinate system. It is strongly recommended that the CS List Dialog remain on the screen at all times when working with multiple coordinate systems.
The CS List Dialog contains eyeball icons next to each of the coordinate systems. Double-clicking a closed eyeball opens it, and vice-
versa. When open, the CS Frame Indicator for that coordinate system will be displayed on the screen. This action does not affect the current CS, which will remain highlighted in the CS List Dialog. The CS grid and axis markers will be based on the current CS.
Double-clicking on the name of a coordinate system in the CS List will open the CS Info Dialog for that coordinate system. This dialog allows the user to enter a comment for each coordinate system. The text entered in the Comment text box will appear in the CS List Dialog and as the title for the CS Palette. Because the system names all new coordinate systems, User coordinate system, it is strongly recommended to give each CS a unique name.
CS GRID AND AXIS MARKERS
The coordinate system (CS) grid and axis markers are very important tools when working with multiple coordinate systems. The CS grid graphically displays the planar orientation of the current coordinate system. The CS grid and axis markers will be drawn on the screen when the Show CS Button in the taskbar is turned on (button depressed). When creating multiple coordinate systems, the CS grid should be displayed on the screen at all times.
The axis markers will be placed at the origin of the current coordinate system. The axis marker arrows show the positive direction of the horizontal (H) and vertical (V) axes. When the horizontal and vertical axes align with one of the primary axes, the system labels the axis markers with X, Y and Z. This is the case with three of the four coordinate systems used with Mill/Turn parts, the ZX plane, the XY plane and the YZ plane. The other CS is labeled with HY because the X axis is flipped in the opposite direction. At the intersection of the axis marker arrows, there is either a plus “+” or minus “-”sign. This indicates the polarity (positive/negative direction) of the depth (D) axis with respect to the current view.
7
M i l l / T u r n M a n u a l |
G F K - 1 7 1 1 |
|
|
The grid is drawn in dark gray and shows the plane of the current coordinate system. Additional light gray lines will be drawn showing where the coordinate system intersects with the stock size.
ZX Plane CS |
XY Plane CS |
HY Backside CS |
YZ Plane CS |
USE OF COORDINATE SYSTEMS WITH MILL/TURN PARTS
For turning operations the designation of the machining coordinate system is set by the selection made in the Lathe process dialog for OD, ID or front face. The selection made for the approach type signifies the area of the part being machined and designates the appropriate machining coordinate system. However, with milling operations, the proper CS must be set by the user, usually through the tool orientation.
The machining CS is used to determine how the tool will approach the part. For turning operations, the Approach Type selection designates the axis along which the tool will approach and cut the part, while for milling operations the tool orientation typically designates the axis of tool approach.
Turning operations also require the tool orientation to be specified, however, this information is not used to determine the machining CS, however it is very important to designate the appropriate orientation in order to achieve the correct toolpath.
The various coordinate systems are primarily used for creating milling operations. As the following figures illustrate, the system does support Y axis moves for milling operations. Some mill/turn machines do not support the Y axis, and instead use the C axis to facilitate these type of moves. C axis continuous moves will be discussed in the Rotary Milling section. Users should know whether their mill/turn machines support the Y axis and program their parts accordingly. This issue is discussed further in the Machining and Rotary Milling sections of this manual.
8
G F K - 1 7 1 1 |
M i l l / T u r n |
X axis
Lathe Tool
Z axis
Figure 4: XZ Plane: Turning
9
M i l l / T u r n M a n u a l |
G F K - 1 7 1 1 |
|
|
X axis
Y axis
Z axis
Mill Tool
Figure 5: YZ Plane: OD Milling with Y axis moves
10
G F K - 1 7 1 1 |
M i l l / T u r n |
X axis
Z axis
Mill Tool
C axis
Figure 6: YZ plane, OD Milling with C axis moves
11
M i l l / T u r n M a n u a l |
G F K - 1 7 1 1 |
|
|
X axis
Y axis
Mill Tool
Z axis
Figure 7: XY Plane, Front Face Milling with Y axis moves
12
G F K - 1 7 1 1 |
M i l l / T u r n |
C axis
X axis
Mill Tool
Z axis
Figure 8: XY Plane, Front Face milling with C axis moves
13
M i l l / T u r n M a n u a l |
G F K - 1 7 1 1 |
|
|
X axis
Y axis
Mill Tool
Z axis
Figure 9: HY Plane: Back Face Milling with Y axis moves
14
G F K - 1 7 1 1 |
M i l l / T u r n |
X axis
Mill Tool
Z axis
C axis
Figure 10: HY Plane: Back Face Milling with C axis moves
At first glance CS2: XY Plane and CS3: HY Backside plane may appear identical when seen from an isometric view. The user may wonder why there are two CS’s in the same location. A close examination of the two CS’s shows the difference between them. The difference between the XY plane and the HY backside plane is the axis markers.
The XY plane, which represents the front face has a "+" sign at the intersection of the markers indicating that the positive direction of the depth axis is projecting outward. The Back face plane (labeled as HY) has a “–” sign on the axis markers, indicating that the view is from the negative depth axis. The positive depth axis projects out from the backside of the part. Essentially the difference between the XY plane and the HY backside plane involves the depth axis along which the tool will approach the part.
When machining either the front face or the back face, the tool must approach the part along the Z axis. The question is whether it will approach along the positive Z axis (front face) or the negative Z axis (back face). The way the system is set up, a tool must approach the part along the positive Z axis.
Therefore in order for the tool to approach the part to machine the back face, the machining coordi-
15
M i l l / T u r n M a n u a l |
G F K - 1 7 1 1 |
|
|
nate system must be flipped so that the positive direction of the Z axis is projecting outward from the backside of the part. This is the reason that two coordinate systems are created to facilitate face machining.
G E O M E T RY C R E AT I O N
Geometry can be created in any coordinate system. The CS the geometry is assigned to does not have any bearing on the machining CS. Typically, the machining CS is designated by the tool orientation. If geometry is not created in the appropriate CS for the type of operation that is being created, it is very likely that the resulting toolpath will not produce the desired results. The toolpath will be created based on the machining CS, regardless of the CS of the geometry. Geometry will be machined as it is viewed from the machining CS.
Geometry should be created in the appropriate coordinate system for the type of machining operation to be created. Geometry that defines the cut shape for OD machining operations should be created in the YZ plane. Likewise, geometry for front face operations should be created in the XY plane and geometry for back face operations should be created in the HY backside plane. It may be helpful when creating geometry to be machined on the back face to force the depth of the geometry so that when viewed on the screen, it appears in the correct location. This is recommended for visualization purposes only, as the machining operation and depths of cut will be calculated from the information entered in the machining process dialogs not the location of the selected geometry.
All geometry for OD milling operations must be created in the YZ plane. Geometry is created in a position as if it were to be machined in the C0 position. The rotation is accomplished when the toolpath is created by entering an angle value in the machining process dialog. The position C0 is along the positive direction of the X axis in the standard YZ plane. The system allows the user to designate a start angle when positioning the C axis. All geometry for OD operations must be created in the standard YZ plane, regardless of the start angle. As a result, often times geometry will not be created in the exact planar location in which it will be machined. For example, if a flat slot is created on the OD to be machined at a start angle C90, the geometry would be created at C0 and when the toolpath is created it will be rotated into position.
Geometry can also be created and viewed radially or wrapped when the Rotary Milling option is installed. Refer to the Rotary Milling section at the end of this manual for more information.
T O O L O R I E N TAT I O N
The Mill tool creation dialog contains an orientation diagram when creating a Mill/Turn part. Setting the proper tool orientation is very important because the tool orientation determines the machining coordinate system for the process. The system uses the designated machining CS in order to properly rotate the part. The system rotates the part so that the tool will approach normal to the cutting plane of the machining coordinate system. In other words the tool will approach and cut along the positive depth axis of the machining coordinate system.
16
G F K - 1 7 1 1 |
M i l l / T u r n |
If the Advanced Milling option is installed users are able to explicitly set the appropriate AM machining coordinate system. However, if the advanced Milling option is not installed,
the machining CS will be set by the orientation of the tool.
TOOL ORIENTATION DIAGRAM
Setting the proper tool orientation is very important as it determines the axis along which the tool will approach and machine the part. There are two basic axes along which the tool will travel, the X axis, for OD operations, and the Z axis for face operations. To select the tool orientation, click on one of the four positions on the diagram so that it becomes highlighted.
If the tool orientation is not set correctly, the toolpath that will be generated will not produce the desired results. Often times, the system will not be able to create a toolpath if the tool orientation is not set correctly. Always check the tool orientation diagram if the toolpath (or lack thereof) does not seem correct.
Figure 11 labels the tool orientation diagram according to the approach axis of the selection and also what section of the part should be cut given the selection. It should be noted that a tool approaching along the X axis, while typically used for OD work can also be applied to milling operations cutting the face.
17
M i l l / T u r n M a n u a l |
|
|
|
G F K - 1 7 1 1 |
||
|
|
|
|
|
||
|
|
|
|
|
|
|
|
Z Axis Approach |
|
Z Axis Approach |
|||
|
(Front Face) |
|
(Back Face) |
|||
|
|
|
|
|
|
|
X Axis Approach
(OD)
Figure 11: Tool Orientation Diagram
TURRET SHIFT
The tool creation dialog for milling tools contains a turret shift button when programming a Mill/Turn part. The turret shift for milling tools functions as it does for turning tools. Turret shift allows users to specify a distance from the preset point, the theoretical tip of the tool, to the center of the turret. This dialog can also be used to specify a different tool change position for individual tools.
Default Tool
Change Position
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
Preset Point |
|
|
|
Turret Shift |
|||
|
|
|
|||||
|
|
|
|
|
|
||
Figure 12: Mill Turret Shift |
|
|
|
||||
18
G F K - 1 7 1 1 |
M i l l / T u r n |
Machining Operations
M A C H I N I N G
When one of the Mill/Turn MDD's is selected, the machining palette can be used to create milling operations and turning operations. The available machining processes are the same as those contained in the standard Mill and Lathe modules. Either type of process can now be applied to a single part, a mill/turn part. Turning functions include contouring, roughing, threading and center line drilling. Milling functions include live tool drilling, contouring, roughing, surfacing and threadmilling. (The Surfacing process requires the SolidSurfacer option.) All of these processes operate in the same manner as they do when working on either mill only or lathe only parts. For more information on the specific processes, please refer to the appropriate machining module manual.
MACHINING PALETTE
When a Mill/Turn MDD is selected, the Machining Palette contains two buttons in the title bar which allow users to toggle between mill and lathe processes.
Mill Toggle |
|
|
|
Lathe Toggle |
|
|
|||
|
|
|
|
|
Figure 13: Mill/Turn Machining Palette
When toggling between the milling and turning processes, the Process List will be cleared of any existing Process Tiles. A Process Group (multiple process tiles in one process list) can not contain a combination of milling and turning processes. Milling and turning processes must be created in different process groups. Turning machining processes function as they do with the standard Lathe module. Milling functionality has been enhanced to provide specifically for milling operations on turning parts.
ROTATE TAB
Milling Process dialogs (Drilling, Contouring, Roughing, Surfacing and Threadmilling) contain a Rotate tab when a Mill/Turn MDD is selected. The Rotate tab allows the user to designate C axis rotation for the operation.
The Rotate tab in milling processes contains two selections for rotating the part, Position and Rotary Milling. The Rotary Milling selection will only be available if the Rotary Milling option is installed. Rotary Milling is discussed in the following section.
19
M i l l / T u r n M a n u a l |
G F K - 1 7 1 1 |
|
|
The Position selection allows the user to enter an angle of rotation for the C axis, which designates the position in which the toolpath will be created. When the toolpath is generated, the system will display it in the proper location based on the angle value entered. It is independent of the geometry selected.
Geometry created for face operations should be based on the XY plane and geometry for OD operations should be created in the YZ plane. All geometry for OD operations is created in the YZ plane in the C0 position. The position rotation is accomplished when the toolpath is created. The posted code will contain the appropriate C axis positioning moves.
The Duplicate function allows for subroutine repeats at equal angular intervals of the toolpath generated by the operation. The system will create the toolpath dictated by the Position information and duplicate that toolpath a specified number of times at the interval angle position entered in the C text box. The value entered in the times text box is the additional number of times the toolpath will be
repeated. For example, if you are creating a toolpath using Position at a specified C angle, the process will create the toolpath at that angle and then duplicate it the given number of times at the given angle intervals. Thus the Duplicate # is the total number of subroutines the operation is to be performed minus one for the original step.
20
Loading...