U.S. Department j of Commerce

National Bureau

of Standards Technology Program

A11101 73DDEE

4</»fAU O*

NBSIR 80-2073.2

Guidelines for Exchangeable APT Data Packages

APT Part Programmer's Manual

Bradford M. Smith

June 1980

|

I

i

RATIONAL bureau

OF STANDARDS

L1BHART

SEP 1 9 1980

Automation Technology Program

So--Den

IMBSIR 80-2073.2

GUIDELINES FOR EXCHANGEABLE APT DATA PACKAGES

APT Part Programmer's Manual

Bradford M. Smith

June 1980

Prepared for the

Air Force Logistics Command

Sacramento Air Logistics Center

PRAM Office

U.S. DEPARTMENT OF COMMERCE, Philip M. Klutznick, Secretary

Luther H. Hodges, Jr., Deputy Secretary

Jordan J. Baruch, Assistant Secretary for Productivity. Technology, and Innovation

NATIONAL BUREAU OF STANDARDS, Ernest Ambler, Director
vA'i *
INTRODUCTION

A joint effort between the National Bureau of Standards and the

Air Force Logistics Command ( AFLC ) has developed a method of

APT part programming and postprocessor design which allows a part

program to be processed for any one of a variety of NC machines

with no changes needed in the part program. The concept produces

savings in terms of labor content, leadtime and cost of NC part

programming. Additionally, it gives shops greater flexibility in

scheduling NC facilities and responding to high priority work.

Details of this project are given in three companion documents.

Guidelines for Exchangeable APT Data Packages

Final Report - NBSIR 80-2073.1

APT Postprocessor Specifications - NBSIR 80-2073.3

Postprocessor Software Guide - NBSIR 80-2073.4

The approach was successfully demonstrated in production at Sacramento Air Logistics Center by processing a single APT data

package on three different machine tools. Only the MACHIN selection statement and the part ORIGIN statement had to be changed.

This exchangeability of part manufacturing data was made possible

by modifying the postprocessor software so that each APT statement is processed in the same manner for all machine tools. Thus

the original intent of the part programmer was satisfied on all

three machine tools.

This Part Programmer's Manual describes the APT Postprocessor

language used. For each language statement, it defines the proper order and arrangement of modifiers and scalar values. Furthermore, it defines the machining function which will result from

the use of each statement. Usually these functions are performed

automatically through tape controlled features on the machine

tool or controller. However, the manual also specifies default

conditions under which the postprocessor and machine tool operator accomplish the desired function in the absence of the automatic feature.

The work described was done at the National Bureau of Standards

for the Air Force Logistics Command under Military Interdepartmental Purchase Request FD 2040 78 60013 from the Producibility

,

Reliability, Attainability and Maintenance Office at Sacramento

Air Logistics Center. The Project Manager at Sacramento was Mr.

Cleon Binyon, and software modifications were under the direction

of Mr. Malcolm Allen at Ogden Air Logistics Center.

- 1 -
' ‘
BACKGROUND

The following pages of this manual describe the APT postprocessor

language chosen for this project. The syntax comes directly from

the American National Standards Institute document X3.37 - 1980

on APT. However, the document contains only a subset of the APT

language since lathe language is excluded.

The notation for each language statement uses square brackets to

denote that one of the included words must appear. Further, it

uses parentheses to denote a word that may optionally appear. An

example will illustrate:

SPINDL / n , / CLW \ , ^ CCLW/

The parentheses show that both the direction specification and

the entire range couplet are optional. The square brackets show

that if the range couplet is used, one of the four modifiers must

appear. The small letters "n" and "m" represent numerical

values.

- 3 -
'

- .
AIR /

This statement controls the operation of air jets used for chip

removal or as a coolant. Control is normally effected through

the use of miscellaneous function codes on the postprocessor NC

output

.

Where the NC machine is not equipped with air jets under program

control, this function must be implemented manually by the

machine tool operator. The postprocessor brings the machine tool

to a halt by placing an OPSTOP code on the NC output. A warning

message is generated for the part programmer, and the operator is

advised through a message on the text output to control the function of the air jets manually.

BREAK

This statement is normally used where the NC output of the postprocessor is punched paper tape. The statement is used to segment the paper tape into convienent and manageable lengths.

BREAK causes the postprocessor to terminate the paper tape in an orderly fashion as with an END statement. A new length of paper

tape is then started with all functions such as the spindle and

coolant restored to the condition in which they were before the

break.

CLAMP / ON

OFF

Initiates or terminates a holding operation. Control is normally

effected through the use of miscellaneous function M Codes on the

postprocessor NC output.

Where the NC machine is not equipped with clamping devices under

program control, this function must be implemented manually by

the machine tool operator or the original statement changed by

the part programmer. No warning message is generated. If an axis move is programmed on a clamped axis, the unclaraping must be

done automatically by the postprocessor.

- 5 -
CLAMP / n,

Controls a holding operation on clamp number "n".

value is "ON" if the option is not specified.

The default

CLAMP /

A AX IS

“ LAXIS

CAXIS

X AXIS

YAXIS

Z AXIS

WAXIS

,TL AXIS_

Controls a clamping operation on one axis of the machine tool.

The default value is "ON" if the option is not specified.

CLAMP /

ALL

HE AD ,n CHUCK

COLLET

TABLE

PALLET

’ f°

N

) \offJ

Initiates a clamping operation on the device selected. The default value is "ON" if the option is not specified.

CLRSKF / n

The CLRSRF statement is used by the postprocessor to define a clearance level to be used in conjunction with subsequent RETRCT

statements. When a RETRCT is encountered, the postprocessor will

automatically retract the tool to the clearance level. The

scalar "n" defines the normal distance from the part reference

system origin, along the tool axis, to the clearance level.

- 6 -
CLRSRF /

Used to invoke or suspend a previously defined clearance surface

value.

COOLNT /

MIST

FLOOD

AIR

TAP

This statement is used to control the flow and the type of

coolant used. Use of the minor words FLOOD, MIST, and AIR alone

constitute a request for that type of coolant to be turned ON.

Control is normally effected through the use of miscellaneous

function M Codes on the postprocessor NC output.

Where the NC machine is not equipped with coolant under program

control, a warning message is generated. The operator is then

advised through a message on the text output to control the function of the coolant manually. Only the first occurrance of a COOLNT is noted as a warning message.

COOLNT /

The ON modifier is used to reinstate the coolant that was last

used by the programmer. Where none has been previously specified, the default option FLOOD is used. The OFF modifier will

turn off the last coolant specified to be on.

CUTCOM / n Specifies the cutter compensation register to be used in the NC

controller to adjust the programmed tool path for minor variations in cutter diameter and length from the nominal values used

in the part program. These variations are usually the result of

regrinding, wear, or inaccuracies of tool length adjustment.

Cutter compensation is controlled by M and G codes on the NC output. The exact amount of compensation to be applied is entered

by the operator into the NC controller. Where the NC machine

controller is not equipped with the cutter compensation feature,

this statement cannot be correctly processed. The postprocessor

must then flag the use of this statement with a warning diagnostic.

- 7 -
CUTCOM /

Turns cutter compensation ON or OFF.

CUTCOM / RIGHT

LEFT (

XYPLAN \

YZ PL AN I , (LENGTH , m

)

ZXPLAN I

Determines if compensation is applied to right or left side of

the cutter path. The optional scalar "n" can be used to specify

the cutter compensation register to be used in the NC controller.

The default register is governed by the postprocessor. The next

option selects the coordinate plane to be used for the cutter

compensation. Default value is the XY plane. Finally, cutter

length compensation can be optionally specified by the couplet ( LENGTH, m ). Default length compensation is zero.

CYCLE / BORE, - OPTIONS - ( options are specified on page 12 ) This statement specifies a boring operation consisting of a rapid

plunge, a feed-in motion and a feed-out motion. The depths for

these motions are specified by the couplets RaPTO and FEDTO.

CYCLE / BORE, DEEP, (STEP, m, n, p, etc.) - OPTIONS -

This statement specifies a boring operation consisting of a rapid

plunge, a series of feed motions, and a rapid retraction. The

initial plunge depth is controlled by the RAPTO couplet. The

feed motions are in "woodpecker" fashion; feed to depth, retract

to initial plunge depth, plunge back to the previous feeddepth,

feed down again, etc. The ultimate feed depth is under control

of the FEEDTO modifier. Depths for the intermediate positions

are under control of the STEP modifier.

- 8 -
CYCLE / BORE, DRAG, OPTIONS

This statement specifies a boring operation where the spindle is

brought to a halt at the end of the cut and then withdrawn at rapid feedrate whereapon the spindle is restarted. Otherwise the

parameters and operation are the same as for CYCLE / BORE.

CYCLE / BORE, NODRAG, (ORIENT, n), - OPTIONS -

This statement is similar to the DRAG option except at the end of

the feed motion the spindle is stopped in a known orientation and

a move is made in X or Y to back the cutter away from the work

before the cutter is retracted. Where the spindle orientation

capability is not available, this statement defaults to a CYCLE /

BORE, MANOP.

CYCLE / BORE, MANOP, - OPTIONS - This statement allows for a manual retraction of the tool once

the feed motion has terminated. The machine tool spindle is

turned off automatically.

CYCLE / BORE, RAPOUT, - OPTIONS - This statement specifies a boring operation followed by a rapid

withdrawal with spindle still in motion. Otherwise the parameters and operation are the same as for CYCLE / BORE.

CYCLE / DRILL, - OPTIONS - This statement specifies a drilling operation consisting of a rapid plunge, a feed motion, and a rapid retraction. Depths for

these motions are contained in the modifier couplets RAPTO and

FEDTO.

- 9 -
CYCLE / DRILL, DEEP, (STEP, ml, m2 - ran), OPTIONS

This statement specifies a drilling operation consisting of a rapid plunge, a series of feed motions, and a rapid retraction.

The initial plunge depth is controlled by the RAPTO couplet. The

feed motions are in "woodpecker" fashion; feed to depth, retract

to initial plunge depth, plunge back to the previous feed depth,

feed down again, etc. The final feed depth is controlled by the

FEEDTO couplet. Depths for the intermediate positions are under

the control of the STEP couplet.

CYCLE / CSINK , DIAMTR, m, - OPTIONS -

This statement specifies a countersinKing operation consisting of

a rapid plunge, a feed motion, and a rapid retraction. The feed

depth is computed by the postprocessor from the scalar values of

"m", the desired countersink diameter, and the tool tip angle

given in the previous LOAD/TOOL statement.

CYCLE / TAP, - OPTIONS -

This statement specifies a fixed cycle of tapping operations consisting of a rapid plunge, forward spindle, feed to depth, reverse spindle, feed-out to the feed start position, and a rapid

retraction .

CYCLE / MANUAL

A manually controlled operation is to be performed at each X Y

point. The machine operator will restart the machine after each

operation .

CYCLE / MILL, - OPTIONS -

This statement specifies a milling operation consisting of a rapid plunge, a feed motion into the workpiece, a milling sequence

to successive GOTO points, and a rapid retraction after the last

point. Milling feedrate is specified by a normal FEDRAT/ command. The CYCLE feedrate couplet controls only the tool axis

feed motion. The milling sequence is cancelled by any other CYCLE command
CYCLE / OFF

This statement terminates a previously defined cycle operation

sequence.

CYCLE /ON, - OPTIONS -

This statement reinstates the last defined cycle operation sequence. Options may be appended to modify any aspect of the sequence desired .

For all CYCLE operations the following couplets can be used as

options : RAPTO, m The tool will plunge at rapid feedrate to

the position defined by the delta distance

"m". A positive value is measured from the

point back along the spindle center line. A

negative value is measured from the point in

the opposite direction.

FEDTO, n The tool will plunge under feedrate control

to the position defined by the delta distance "n". Positive and negative values are

measured as for RAPTO.

IPM, f The tool will move at a feedrate "f" in units of inches per minute.

IPR , r The tool will move at a feedrate "r" in units of inches per revolution.

DWELL, s Commands a dwell of "s" seconds.
DELAY / n Causes a suspension of all machine operations for "n" seconds.

Used to halt the machine for a given length of time.

DELAY / REV, n Causes a suspension of all machine operations for "n" revolutions

of the spindle

Dwell times are usually initiated by an appropriate miscellaneous

function, M code, or by a preparatory function, G code. The

length of dwell is governed either by an associated motion register (X,Y,Z, etc.) or by activating a preset timer in the NC controller. In the case of a dwell for a specified number of revolutions, the postprocessor first calculates the time in seconds

from the known spindle speed and the given number of revolutions.

Kor controllers without a delay feature, the postprocessor should

either simulate a delay or generate a warning message indicating

a delay was requested but not executed. A delay can sometimes be

effected by placing leader characters on the NC output.

END

This statement indicates the logical completion of a section of

programming. An orderly termination of all postprocessor output

follows. Final messages are printed on the text output concerning tape length produced, machining time, number of processing

errors , etc .

FEDRAT / n

Specifies the feedrate in inches per minute. Range selection is

optional

- 12 -
FEDRAT /

Specifies the feedrate " n" in units of inches per minute or per

revolution. Range selection is optional. The postprocessor will

ordinarily calculate the proper F code ( feedrate number ) to be

placed on the NC output based upon data such as the commanded

feedrate, the length of tool motion being executed, and the spindle speed if IPR has been specified.

The feedrate may have to be reduced by the postprocessor as a result of acceleration - deceleration requirements of the

machine, surface feet per minute calculations, or tape reader

speed limitations. All feedrates are tested by the postprocessor

to lie within maximum and minimum bounds. The optional range

selection will normally result in a miscellaneous M code being

generated to shift gears of the spindle transmission along with a delay preparatory function G code to cause a dwell for the required length of time for gear changing.

For those NC machines without gear changing ability, the RANGE

option is ignored. If by chance the commanded feedrate exceeds

the capability of the machine tool, a warning message is placed

on the output text listing and the maximum feedrate is assigned.

If a feedrate command is encountered which cannot be executed

within given range, an automatic range change is made and a warning message is generated.

GOHOME

Commands all axes of the machine tool to move to the HOME position. The statement is often used for manually changing tools,

for part inspection, or for loading and unloading workpieces.

Rapid feedrate is used for this move.

The HOME position is normally specified as the X,Y,Z value in the

first FROM statement. The inclusion of a SET / HOMEPT, X, Y, 2

command in the part program will overide all previous specifications. If the HOME point is not defined in the part program, the

postprocessor will assign a default value for that particular

machine. However, this may not be possible with controllers

offering a full floating zero capability.

- 13 -
INSERT $

Characters occurring after INSERT are inserted directly into the

output control information. No check is made for validity of

data. Imbedded blank characters are inserted in the same manner.

Character string must be terminated with a $.

LEADER / n Specifies the amount of leader to be produced in units set by the

postprocessor, commonly inches.

LINTOL / n Controls the linearization function. The value "n" specifies the

acceptable deviation of the tool tip from the desired cutter

pa th .

LINTOL /

Commands that the linearization function in the postprocessor be

on or off. The postprocessor linearization function forces the

machine tool to stay within a specified tolerance of a straight

line connecting two successive cutter location points. Intermediate points are calculated to fulfill this purpose. Linearization is performed only for non-rapid movements when started by

a LINTOL statement.

LOAD / TOOL, n, ( TLSET , m), (TLANGL, a), (MANUAL)

Controls the loading of a tool specified by the optional parameters or by a previous SELECT / TOOL statement. "n" is the tool

identification number, "m" is the set length, and "a" is the tool

tip angle. These are specified in optional couplets and can occur in any order. The inclusion of the MANUAL option will disable the automatic tool change sequence to allow for special situations .
The tool to be loaded by this command is specified by the value

" n " . Use of just the basic statement LOAD / TOOL with no other

data implies that the tool was previously specified by a SELECT /

TOOL statement. Control of the tool loading operation is normally effected through the use of miscellaneous function, M Codes,

preparatory function, G Codes, and tool function, T Codes, on the

postprocessor NC output.

Where the NC machine is not equipped with tool changing capability under program control, this function must be implemented manually by the machine tool operator. In this situation the postprocessor will move the machine tool to the manual tool change

position and will halt all machine operations by placing STOP and

SPINDL / OFF codes on the NC output. The operator is then advised to load the specified tool manually through a message on

the text output.

MCHTOL / n

This feature of a postprocessor checks the amount of overshoot or undershoot that will occur when a change in direction has been

programmed. If the deviation from the desired cutter path

exceeds the value "n", the postprocessor will compensate by inserting commands on the NC output. Dwell commands are used to

correct for excessive undershoot. The commanded feedrate is reduced to correct for overshoot.

OPSKIP / ON

OFF

This statement allows the machine tool operator to skip over optional sections of NC control information. All blocks of postprocessor NC output occurring after an OPSKIP/ON statement are

flagged with slashes to allow the NC controller to ignore them

whenever the machine operator uses the block delete function of

the controller. Where this command is used for controllers not

equipped with the block delete option, a warning message is generated.

- 15 -
OPSTOP

Optionally halts all machine motions under tape control and turns

off the coolant, spindle, and tape reader. This command is similar to the STOP command but is under the option of the machine

operator. Through a switch on the control panel he can enable or disable this feature. If the switch is off, the command is ignored . For a machine not equipped to recognize the OPSTOP miscellaneous

function M Code, the postprocessor should ignore the command and

generate a warning message.

ORIGIN / X, Y, (Z) , (A) , (B)(C)

This statement defines the machine origin in terms of the part

programming reference system. X, Y, and Z give the location of

the machine tool origin in the coordinate system used for the

part program. Likewise, A, B and C give the orientation of the

machine's rotary axes. The values for Z, A, B and C are optional. Their default values are zero.

P1V0TZ / n

This statement is used only by raultiaxis postprocessors to define

the relationship of the part programming origin to the pivot

plane of the machine tool. The pivot plane is the basic reference plane of the machine tool. It is generally a Z plane. All

machine slide dimensions are measured from the pivot plane. The

scalar value "n" specifies the distance from the part origin to

the pivot plane.

PPRINT -------

This statement is used to place comments in the postprocessor

text output. These are used to give messages to the part programmer or machine tool operator concerning part setup, tool

changes, or reasons for a programmed STOP or OPSTOP. The string

of characters are inserted into the printed output of the postprocessor .

- 16 -
RAPID

This statement specifies that the next programmed movement is to

be executed at the maximum possible feedrate. The RAPID command

applies only to the next movement. All subsequent moves are at

the previously defined feedrate.

The exact feedrate for Rapid motions is machine dependent but can

be set by the part programmer using a SET / RAPFED, f command.

RETRCT

This statement specifies a rapid traverse movement of the tool to

the clearance surface which has been previously defined by a CLRSRF statement. Motion is along the tool axis (Z axis). The

command is used on positioning and milling machines.

REWIND

This command repositions the control medium to the first rewind

stop code detected. The machine is brought to an orderly halt

with spindle, coolant, etc. turned off.

ROTATE / [HEAD"! , n [table]

Commands the rotation of a head or table in the positioning mode

only. Motion is not under feedrate control. The scalar "n"

specifies the absolute value of the angle of rotation and is

given in degrees.

The ROTATE command normally results in A or b axis movements on

the postprocessor NC output. For machine tools not equipped for

these movements there can be no simple manual remedy. The postprocessor should flag this condition as being beyond the capability of the selected machine tool.
ROTATE / HEAD

TABLE

, IN CR , m

(

CLW \

CCL W /

( ROTREF)

The angular rotation from the present position is specified by

the couplet (INCR.m). It is an incremental movement of "m" degrees. Where the optional direction selector is not specified,

the rotation is governed by the sign of "m". Rotation is clockwise for positive "m" and counterclockwise for negative "m". Use

of ROTREF insures that after rotation the part coordinate system

and the machine coordinate system remain in alignment.

ROTATE / HEAD

TABLE

ATANGL, n , / CLW \

\ CCLW

/

, (ROTREF)

The couplet (ATANGL, n) commands a rotation to the angle "n" degrees. Direction of rotation is governed by the optional selector. Default direction is clockwise. As above, the option ROTREF will cause rotation of the part programming coordinate syst em

.

SELECT / HEAD,

n ALL

BOTH

LEFT

RIGHT

MAIN

HIGH

LOW

This statement identifies a particular head on the NC machine

which will be referenced by future statements. The scalar "n"

will select the head by number. Machines with a single head ignore this statement.

SELECT / TOOL, n, ( TLSET , m), (TLANGL, a), (MANUAL)

This statement controls the selection of a cutting tool to be

used by the next LOAD / TOOL statement. previous SELECT / TOOL

statement. The scalar "n" is the tool identification number, "m"

is the set length, and ,, a" is the tool tip angle. These are

specified in optional couplets and can occur in any order. The

inclusion of the MANUAL option will disable the automatic tool

change sequence to allow for special situations. The tool will

not be loaded into the active spindle until a LOAD/TOOL statement

is encountered at a later time. Control is normally effected

through the use of miscellaneous function, M codes, preparatory

- 18 -
function, G codes, and tool function, T codes, on the postprocessor NC output

.

Where the NC machine is not equipped with automatic tool changing

capability under program control, this function must be implemented manually by the machine tool operator when the LOAD/TOOL

statement is encountered. The postprocessor must simply store

the data given in the SELECT/TOOL statement for future use when

issuing a message to the operator for loading the tool.

SEQNO / n Specifies that the next output block will be assigned the sequence number "n". Only the next block will be affected. Normal

sequencing will then resume.

Starts and stops the sequence numbering function. The ON modifier is used to reinstate the sequence numbering that was last

used by the programmer. Where none has been previously specified, the default option is to number each block starting with

the number one and incrementing by one.

SEQNO / INCR, m, (r)

Specifies that the next output block will be assigned a sequence

number equal to the previous number (or zero if no previous

number was assigned) plus the scalar value "m" . Subsequent sequence numbers will be incremented by the value "m". If the

scalar value "r" is present, a sequence number will only be assigned once every " r" output blocks.

- 19 -
SEQNO / n, INCR, m, (r)

Specifies that the next output block will be assigned sequence

number "n" and that each following block will be incremented by

"m" and "r M as above.

SET / MODE

[

LINEAR

CIRCUL

PARAB 0

Specifies the particular mode of interpolation to be used, (when

ever possible) for all non-linear motions.

SET / RAPFED, f

Allows the specification of a feedrate for all RAPID moves including within the CYCLE commands. If "f" exceeds the normal RAPID for the machine, a default maximum value is selected.

SET / TLCHG , X, Y, (Z)

Selects the position to be used for all manual tool changes. The

values X, Y, and Z are in the part coordinate system. Z is optional with the default value in the fully retracted position except with controllers using a floating zero. On these controllers, if the Z position is not specified, the Z axis machine position remains unchanged.

SET / HOMEPT, X, Y, Z Selects the position for all GOHOME commands. The values X, Y,

and Z are in the part coordinate system.

- 20 -
SPINDL / n, / CLW \ , \ C CLW J

Commands the spindle to be turned on at the specified angular

velocity "n" revolutions per minute. The default of the optional

angular direction is clockwise. The default of the optional

range is determined by the postprocessor, and "m" specifies a range by number.

Control of spindle speed is accomplished by varying the speed of

the drive motor and by changing the gear ratio between the motor

and the spindle. The desired gear range can be specified by the

words HIGH, MEDIUM, and LOW or can be selected by number. m = 1 specifies the lowest range; m = 2 is the next higher range; m = 3

next, etc. For transmissions with three ranges, LOW, MEDIUM and

HIGH correspond to m =1, 2, 3. But for transmissions with only

two ranges, MEDIUM and HIGH both select the m = 2 range. Control

is accomplished through the use of appropriate miscellaneous

function, M Codes, and preparatory function, G Codes.

If a range selection is necessary but not specified, it shall be

accomplished by the postprocessor in the best way possible.

Where the NC machine is not equipped with spindle functions under

program control, this function must be implemented manually by

the machine tool operator The postprocesor brings the machine

tool to a halt be placing a STOP code on the NC output. The

operator is then advised through a message on the text output to

manually set the speed direction, and range of the spindle drive

system to the proper values.

Commands the spindle to be turned on. Previous spindle speed,

direction, and range are reinstated unless modified by the optional parameters. If SPINDL / ON appears as the first specification, a default spindle speed is assigned by the postprocessor.

21 -
SPINDL / OFF i. M

Turns off the spindle motop-and coolant.

. - i i 'O’ i -

. Cu^rsa oyx..’.o ?q/-

inoivC.o »ii i.c J

6

3ilO XJqc: d lo

?•* isne

•» .) ') l ' V

f.'i

!?. ;90O"I(j020q Of1 S¥TN CrL’ 'r

; N E U T R t

U

Places the spindle motor trans, mission in the neutral position

b 3 £i

s ? 0 3 Jj n ! v i

'• ' y <•< j -> A > o - ’»

' - /> > O O H •? 1 d * A' «.

.< «> S J {; £ f ) j) :t ?. ?*<i £-' m . i g tf "> u fj v r* t- {? 3 o r* t o a

<,T. 1 rid , ,-v > i d. i

?) )n Ii 1 i find 1 & *3' 0 H ft 0 1

0

*:• is 3 a

1 i ^ s; ,ii * r

i ll 3 ri 3 .i.'W ’? dua . o

i

i - 10 Sl 0,1 b •>:

.

,

, J. , « < . < a f fl *• * a •:* is J <i l s. » »•! t ** -3 1

}

f* ' SP Dir «/* ‘LOCK ‘

v ’ “

MUIQ 3 M . WO. f-e’mft*

II c - - u; s o q v

2 oos ') s X Xeoaifti e «'i is x i ct o "< c, q u

. « 9 fc> 0 C lo eso oi:x

1

0

r t

o

si i: ?. ipoJe

i

e q «• if hi f> , seoo

J

* * £> ^* ^ t iA v j-f *» i **—* — ft

• n

-h r fftfls ii , tjt i J. i c e o e don i«U v,is8890s»i e c a oi-.- !^P

d

IM'«q/ odi .1 •,o«.opn«oq «ri4

_ V . . istbnu gnoidono'i s> X b n i q » rt-Jxw bsqqiope

:)vn£i> aSm Vjf fiVUV** key.aoick position.

a iriosffl ert-j ggnlid ‘jo8eo0'»<l**iQ.<5 ar.i -x

niriosffl - . . d T . iuqdiJO Ofl odd no 9 boo HOT^ & &nio&Lq

o.1 SuqJuo ixei edd ao » tigwoidJ fc 5 B*-he

brjE , noidosi ib boeqv 5-

. H *>U j. fcV IfH:

9

S'Ptfto ErL

1 b/* WlfW, 1 c

( nf * ~ *

Causes the spindle to be oriented into an absolute angular position specified by the optional scalar "n" or in the absence of

"n" in a position determined by the machine hardware or the postprocessor

STOP

/ s m , WOJ |

, 3 014 ill MU 1 Q 3 M

| HOXHI /

\ ^ * ' “ i

“• i b rr x q e * n o fc 9 ii *1 u ^ ^ ® u *

rid vd bertiboiTi aselnu bedBdanisi sie

Ha it S a-il^ a^h lrje njat i

c?o^

q

u^d e^; ta pje] qco.nt r o 1 and

' i^«^V<,3Voq V<6*

' turns off the

... r c _

- 22 -
TMARK

This command causes a rewind stop code to be placed on the postprocessor NC output. It is used by the N C controller to terminate the rewind sequence of the control tape and restart

machining from a known point in the program.

TRANS / X, Y, (Z)

Defines the translation parameters used to modify tool position

coordinates'. The X, Y and Z values are those to be added to the

part coordinates in order to obtain the machine tool coordinates.

Z is optional with the default value being zero.

- 23 -
NBS-114A (REV. 9-76)

U.S. DEPT. OF COMM. 1. PUBLICATION OR REPORT NO. BIBLIOGRAPHIC DATA

SHEET

NBSIR 80-2073.2

4. TITLE AND SUBTITLE

Air Force Logistics Command

Guidelines for Exchangeable APT Data

Packages

APT Part Programmer’s Manual

7. AUTHOR(S)

Mr. Bradford M. Smith

9. PERFORMING ORGANIZATION NAME AND ADDRESS

NATIONAL BUREAU OF STANDARDS

DEPARTMENT OF COMMERCE

WASHINGTON, DC 20234

5. Publication Date June 1980

8. Performing Organ. Report No.

11. Contract/Grant No.

12. SPONSORING ORGANIZATION NAME AND COMPLETE ADDRESS (Street, City, state, ZIP)

Air Force Logistics Center

McClennan Air Force Base

California 95652

13. Type of Report & Period Covered Final

Agency Code • *

r-<

ii m —— ——i— —— ———— ——————i ! i —

y

15. supplementary notes This is a companion document to Air Force Logistics Command

Guidelines for Exchangeable APT Data Packages, Final Report

I I Document describes a computer program; SF-185, FIPS Software Summary, is attached.

16. ABSTRACT (A 200-word or teas factual summary of moat significant information. If document includes a significant bibliography or

literature survey, mention it here.) A method of APT programming and postprocessor design has been developed which permits

more efficient data preparation for numerical control (NC) machine tools and then

allows this data to be quickly and easily exchanged among different NC machines. This

is accomplished through rigorous specification of the APT post-processor language

based upon new ANSI standards for APT plus a comprehensive definition of the machining

functions which should result from the use of each APT language statement. Individual

post-processors are modified to process each statement in the same manner. The concept was successfully demonstrated in production by processing a single APT data package on

three different milling-drilling type machine tools. A 23% increase in NC manufacturing efficiency is projected. This document describes the APT post-processor language

used, including the syntax and semantics of each statement. It also defines the defaul : conditions under which the post-processor and machine tool operator accomplish the

desired function in the absence of the automatic feature.

17. KEY WORDS (six to twelve entries ; alphabetical order; capitalize only the first letter of the first key word unless a proper name;

separated by semicolons)

APT; Automation; Computer aided manufacturing; NC machining; NC programming;

Numerical Control; Part programming

18. AVAILABILITY jX( Unlimited

I I For Official Distribution. Do Not Release to NTIS

Order From Sup. of Doc., U.S. Government Printing Office, Washington, DC

20402, SD Stock No. SN003-003-

fX~| Order From National Technical Information Service (NTIS), Springfield, va. 22161 U.S. Distribution Only

19. SECURITY CLASS

(THIS REPORT)

UNCLASSIFIED

20. SECURITY CLASS

(THIS PAGE)

UNCLASSIFIED

21. NO. OF

PRINTED PAGES

23

22. Price

$5.00

USCOMM-DC