tool_compensation.lyx

CNC 的开放码,EMC2 V2.2.8版

#LyX 1.3 created this file. For more info see http://www.lyx.org/
\lyxformat 221
\textclass book
\language english
\inputencoding default
\fontscheme bookman
\graphics default
\float_placement h
\paperfontsize 10
\spacing single 
\papersize Default
\paperpackage a4wide
\use_geometry 0
\use_amsmath 0
\use_natbib 0
\use_numerical_citations 0
\paperorientation portrait
\secnumdepth 5
\tocdepth 5
\paragraph_separation skip
\defskip smallskip
\quotes_language english
\quotes_times 2
\papercolumns 1
\papersides 2
\paperpagestyle default

\layout Chapter

Tool File and Compensation
\layout Section

Tool File
\layout Standard

Tool length and diameter may come from the tool file (see section 
\begin_inset LatexCommand \ref{sub:Tool-File}

\end_inset 

) or from a word specified when tool compensation is enabled.
\layout Section

Tool Compensation
\layout Standard

Tool compensation can cause problems for the best of nc code programmers.
 But it can be a powerful aid when used to help an operator get a part to
 size.
 By setting and reseting length and diameter of tools in a single tool table,
 offsets can be made durring a production run that allow for variation in
 tool size, or for minor deviation from the programmed distances and size.
 And these changes can be made without the operator having to search through
 and change numbers in a program file.
\layout Standard

Throughout this unit you will find ocasional references to cannonical functions
 where these are necessary for the reader to understand how a tool offset
 works in a specific situation.
 These references are intended to give the reader a sense of sequence rather
 than requiring the reader to understand the way that cannonical functions
 themselves work within the EMC.
\layout Section

Tool Length Offsets
\layout Standard

Tool length offsets are given as positive numbers in the tool table.
 A tool length offset is programmed using G43 Hn, where n is the desired
 table index.
 It is expected that all entries in the tool table will be positive.
 The H number is checked for being a non-negative integer when it is read.
 The interpreter behaves as follows.
\layout Standard

1.
 If G43 Hn is programmed, A USE_TOOL_LENGTH_OFFSET(length) function call
 is made (where length is the value of the tool length offset entry in the
 tool table whose index is n), tool_length_offset is reset in the machine
 settings model, and the value of current_z in the model is adjusted.
 Note that n does not have to be the same as the slot number of the tool
 currently in the spindle.
\layout Standard

2.
 If G49 is programmed, USE_TOOL_LENGTH_OFFSET(0.0) is called, tool_length_offset
 is reset to 0.0 in the machine settings model, and the value of current_z
 in the model is adjusted.
 The effect of tool length compensation is illustrated in the screen shot
 below.
 Notice that the length of the tool is subtracted from the z setting so
 that the tool tip appears at the programmed setting.
 You should note that the effect of tool length compensation is immediate
 when you view the z position as a relative coordinate but it does affect
 actual machine position until you program a z move.
\layout Standard


\begin_inset Minipage
position 1
inner_position 0
height "0pt"
width "50col%"
collapsed false

\layout Standard

Test tool length program.
 
\layout Standard

Tool #1 is 1 inch long.
\layout Standard


\family typewriter 
N01 G1 F15 X0 Y0 Z0
\newline 
N02 G43 H1 Z0 X1
\newline 
N03 G49 X0 Z0
\newline 
N04 G0 X2
\newline 
N05 G1 G43 H1 G4 P10 Z0 X3
\newline 
N06 G49 X2 Z0
\newline 
N07 G0 X0
\end_inset 


\hfill 

\begin_inset Minipage
position 1
inner_position 0
height "0pt"
width "50col%"
collapsed false

\layout Standard
\added_space_top 0.3cm \added_space_bottom 0.3cm \align center 

\begin_inset Graphics
	filename length1.png
	width 2in
	subcaptionText "Length Offset"

\end_inset 


\end_inset 


\layout Standard

The effect of this is that in most cases the machine will pick up the offset
 as a ramp during the next xyz move after the g43 word.
\layout Section

Cutter Radius Compensation
\begin_inset LatexCommand \label{sec:Cutter-Radius-Compensation}

\end_inset 


\layout Comment

By Jon Elson
\layout Standard

Cutter Diameter Compensation (also called Cutter Radius Compensation) is
 something that was obviously added onto the RS-274D specification at the
 demand of users, as it is VERY useful, but the implementation was poorly
 thought out.
 The purpose of this feature is to allow the programmer of the tool path
 program to 'virtualize' the tool path, so that the control can, at run
 time, determine the correct offset from the surface to be cut, based on
 the tools available.
 If you resharpen the side cutting edges of end mills, then they will end
 up smaller than the standard diameters.
\layout Standard

The problem is to describe to the control whether the tool is going to be
 cutting on the outside of an imaginary path, or on the inside.
 Since these paths are not necessarily closed paths (although they can be),
 it is essentially impossible for the control to know which side of the
 line it is supposed to offset to.
 It was decided that there would only be two choices, tool 'left' of path,
 and tool 'right' of path.
 This is to be interpreted as left or right 'when facing the direction of
 cutter motion'.
 The interpretation is as if you were standing on the part, walking behind
 the tool as it progresses across the part.
\layout Subsection

Cutter Radius Compensation Detail
\layout Comment

By Tom Kramer and Fred Proctor
\layout Standard

The cutter radius compensation capabilities of the interpreter enable the
 programmer to specify that a cutter should travel to the right or left
 of an open or closed contour in the XY-plane composed of arcs of circles
 and straight line segments.
 The contour may be the outline of material not to be machined away, or
 it may be a tool path to be followed by an exactly sized tool.
 This figure shows two examples of the path of a tool cutting using cutter
 radius compensation so that it leaves a triangle of material remaining.
\layout Standard


\begin_inset Minipage
position 1
inner_position 0
height "0pt"
width "50col%"
collapsed false

\layout Standard

In both examples, the shaded triangle represents material which should remain
 after cutting, and the line outside the shaded triangle represents the
 path of the tip of a cutting tool.
 Both paths will leave the shaded triangle uncut.
 The one on the left (with rounded corners) is the path the interpreter
 will generate.
 In the method on the right (the one not used), the tool does not stay in
 contact with the shaded triangle at sharp corners.
 
\end_inset 


\hfill 

\begin_inset Minipage
position 1
inner_position 0
height "0pt"
width "50col%"
collapsed false

\layout Standard
\added_space_top 0.3cm \added_space_bottom 0.3cm \align center 

\begin_inset Graphics
	filename radius_comp.png
	width 2.5in

\end_inset 


\end_inset 


\layout Standard

Z axis motion may take place while the contour is being followed in the
 XY plane.
 Portions of the contour may be skipped by retracting the Z axis above the
 part, following the contour to the next point at which machining should
 be done, and re-extending the Z-axis.
 These skip motions may be performed at feed rate (G1) or at traverse rate
 (G0).
 Inverse time feed rate (G93) or units per minute feed rate (G94) may be
 used with cutter radius compensation.
 Under G94, the feed rate will apply to the actual path of the cutter tip,
 not to the programmed contour.
\layout Standard


\begin_inset Note
collapsed false

\layout Standard

where is figure 7
\end_inset 


\layout Subsubsection*

Programming Instructions
\layout Itemize

To start cutter radius compensation, program either G41 (for keeping the
 tool to the left of the contour) or G42 (for keeping the tool to the right
 of the contour).
 In Figure 7, for example, if G41 were programmed, the tool would stay left
 and move clockwise around the triangle, and if G42 were programmed, the
 tool would stay right and move counterclockwise around the triangle.
\layout Itemize

To stop cutter radius compensation, program G40.
\layout Itemize

If G40, G41, or G42 is programmed in the same block as tool motion, cutter
 compensation will be turned on or off before the motion is made.
 To make the motion come first, the motion must be programmed in a separate,
 previous block.
\layout Subsubsection*

D Number
\layout Standard

The current interpreter requires a D number on each line that has the G41
 or G42 word.
 The value specified with D must be a non-negative integer.
 It represents the slot number of the tool whose radius (half the diameter
 given in the tool table) will be used, or it may be zero (which is not
 a slot number).
 If it is zero, the value of the radius will also be zero.
 Any slot in the tool table may be selected this way.
 The D number does not have to be the same as the slot number of the tool
 in the spindle.
\layout Subsubsection*

Tool Table
\layout Standard

Cutter radius compensation uses data from the machining center's tool table.
 For each slot in the tool carrousel, the tool table contains the diameter
 of the tool in that slot (or the difference between the actual diameter
 of the tool in the slot and its nominal value).
 The tool table is indexed by slot number.
 How to put data into the table when using the stand-alone interpreter is
 discussed in the tool table page.
\layout Subsubsection*

Two Kinds of Contour
\layout Standard

The interpreter handles compensation for two types of contour:
\layout Itemize

The contour given in the NC code is the edge of material that is not to
 be machined away.
 We will call this type a "material edge contour".
 
\layout Itemize

The contour given in the NC code is the tool path that would be followed
 by a tool of exactly the correct radius.
 We will call this type a "tool path contour".
\layout Standard

The interpreter does not have any setting that determines which type of
 contour is used, but the description of the contour will differ (for the
 same part geometry) between the two types and the values for diameters
 in the tool table will be different for the two types.
\layout Subsubsection*

Material Edge Contour 
\layout Standard

When the contour is the edge of the material, the outline of the edge is
 described in the NC program.
 For a material edge contour, the value for the diameter in the tool table
 is the actual value of the diameter of the tool.
 The value in the table must be positive.
 The NC code for a material edge contour is the same regardless of the (actual
 or intended) diameter of the tool.