WARRANTY

Control Solutions, Inc. warrants this product to be free from defects in material and workmanship for a period of ninety days from the date of shipment. If the product is found to be defective during the warranty period, the product will either be repaired or replaced at our option without charge.

LIMITATION OF WARRANTY

This warranty does not apply to defects resulting from modification or misuse of any product or part, or failures caused by accidents, acts of God, or other causes beyond the control of Control Solutions, Inc. (i.e., lightning, power surges, etc.). Any product or part manufactured by others and merely installed by Control Solutions, Inc., such as electric motors, etc., is specifically not warranted by us and it is agreed that such product or part shall only carry the warranty, if any, supplied by the manufacture.

Under no circumstance shall Control Solutions, Inc. or any of its affiliates have any liability whatsoever for claims or damages arising out of the loss of use of any product or part sold to you.

While Control Solutions, Inc. products will general recognize and inform the user of programming syntax errors, Control Solutions, Inc. does not warranty the performance of the system when it is issued commands that contain invalid syntax.

This warranty is in lieu of all other warranties, expressed or implied, including any implied warranty of merchantability or fitness for a particular use. Control Solutions, Inc. shall not be liable for any direct, indirect, special or consequential damages, You agree in accepting our product or part to save us harmless from any and all such claims or damages that may be initiated against us by third parties.

RETURNING A PRODUCT

Before returning a product, obtain a return authorization number from the factory. The product should be shipped in the original packing carton or one that will provide equal protection. Shipping damage is not covered by this warranty. Send the product, transportation prepaid to the factory, referencing the return authorization number. Repairs will be made and the product returned, transportation prepaid. Repairs are warranted for the remainder of the original warranty or for 90 days, whichever is greater.

CLAIMS FOR SHIPPING DAMAGE

Upon receipt of the product, inspect it immediately for any damage. If the product is damaged, file a claim with the carrier. The factory will supply you with a quotation for estimated costs of repair. You must negotiate and settle with the carrier for the amount of the damage.

The Shadow CNC

The Shadow CNC can be installed on various kinds of motion apparatus. The Shadow provides high productivity, reliability, and quality performance.

The user or programmer is the central party responsible for instructing the Shadow and thus accomplishing the desired result. Like any other computer, the Shadow CNC does no more and no less than the programmer tells it to do. This CNC will rough a part out and then finish it to tolerances of +/-0.0001 inches. The total performance capabilities of the Shadow are in the hands of the programmer.

Axes movement is assumed standard in milling operations and thereby familiar to the programmer. The tool moves to the right relative to the work piece with an X+ move, thus the table (with work piece) moves to the left. The saddle (with work piece) moves toward the operator with a Y+ and away from him with a Y- move. The Quill (with cutting tool) moves up with a Z+ move and down with a Z- move.

General Notes on Operation

Powering the system down will not cause loss of:

the current program stored in program memory,

programs stored in external ram, or

the permanently saved machine set-up constants.

If you were working in 'SET-UP', 'JOG', OR 'MDI' the control will power-up in the last mode in which you were working before power down. If you were working in 'EXT', 'AUTO-S', or 'AUTO-C' mode upon power down, the control will power-up in MDI mode.

Running Indicator

A [R] will appear on the upper status line whenever a program is running or a command is being executed in MDI, AUTO-S OR AUTO-C.

START KEY

The 'START' key is used to start motion on the control. Depressing the start key during motion will have no effect upon the control. The 'START' key is also used throughout the set-up menus.

SLIDE HOLD

The 'SLIDE HOLD' key is used to stop motion on the control. Once motion has been started with the 'START' key, pressing the 'SLIDE HOLD' key will cause the motion to stop at the current position. Pressing the 'START' key will cause the motion to resume where it left off when the 'SLIDE HOLD' key was pressed. If the 'SHIFT' key is pressed and then the 'SLIDE HOLD' key is pressed, the move will be aborted and the control will go into MDI mode. When the external slide hold switch has been activated it is not necessary to press the 'START' key, just release the external slide hold switch and motion will continue. When the control is in slide hold an 'S' will appear on the upper status line indicating this mode. If a move is attempted while the control is in slide hold an error message will appear.

JOG MODE

Pressing the 'JOG' key will place the control in jog mode. This mode is normally used to correctly position the work piece or jig under the tool. Axis movement is caused by pressing keys on the front panel or using the handwheel.

INCREMENTAL and CONTINUOUS JOG

In low jog, when a jog key is pressed, a movement of 0.001 inches occurs. If the key is released immediately, then only a single increment of motion will occur.

In high jog, when a jog key is pressed, an initial movement of 0.1 inches occurs. If the jog key is held and not released immediately, the axis pulses once, pauses, and then begins to run continuously at a feedrate of 100 inches per minute.

X AXIS JOG

A positive X direction jog is executed by pressing the '6' key.

A negative move on the X axis is accomplished by pressing the '4' key.

Y AXIS JOG

Press the '8' key for about six seconds, the saddle will move the work piece toward you. This movement causes the tool to move along the Y axis in positive direction.

A negative Y axis move is executed by pressing the '2' key. Do this for about six seconds and the saddle will move the work piece away from you. The tool will move toward you in respect to the workpiece.

Z AXIS JOG

The Z axis can be jogged by pressing the 'UP' key or the 'DN' key.

To jog the X, Y or Z axis press 'X', 'Y' or 'Z' and then turn the hand wheel.

U, V AND W JOGGING

To Jog the U, V or W axis, if present, press '/' 'STEP', then 'X' for U, 'Y' for V, or 'Z' for W and then turn the hand wheel.

U, V and W cannot be jogged with arrow keys.

Zeroing Axis in JOG MODE

Pressing the 'R' key in jog mode will zero all axes position displays and set the current absolute position at zero.

Entering '-' 'X' 'R' in JOG MODE will zero only the X-axis.

Entering '-' 'Y' 'R' in JOG MODE will zero only the Y-axis.

Entering '-' 'Z' 'R' in JOG MODE will zero only the Z-axis.

Axis U, V and W will work in a similar manner.

If the 'G' key is pressed in JOG MODE, all axes will move at rapid to the zero position or to the G92 offset position, if set.

TWO AXES SIMULTANEOUS JOG

Pressing the '9' key causes the tool to move to the right and away from you at a 45 degree angle to both the X and Y axes. This is a two axes, simultaneous move in the X positive direction and the Y positive direction. There are three other keys which produce 45 degree angle moves implementing the X and Y axes simultaneously. These are the '3' key, the '1' key, and the '7' key.

HIGH SPEED JOG

To shift the Shadow to high speed Jog, press the 'HI' key. The high speed jogging rate is either 100 inches per minute or the rapid rate (set internally when the Shadow CNC is installed), whichever is lower. When the Shadow is in the High Speed Jog, incremental movement is 0.1 inches. Press the 'LO' key for low jog.

JOG RATE CONTROL

Press the '2' key, continue pressing the key while simultaneously rotating the hand wheel counterclockwise. The tool is moving toward you and should be slowing as the feedrate percentage decreases from 100 percent. When the feedrate reads 5% on the LCD display, the axis creeps. Now rotate the hand wheel clockwise while still pressing the Jog key and notice that the tool resumes movement.

MDI MODE

Pressing the 'MDI' key will place the control in MDI mode.

MDI mode is most commonly used to enter commands into the control that make up a program to be executed later in Auto-continuous mode. Following are examples of commands that are executed immediately by pressing 'START'.

SINGLE AXIS MOVES IN MDI MODE

With the feedrate set at 10 IPM, (press: 'F' '1' '0' '.' 'START'), move the tool one inch to the right. Press, in order, the 'X' '1' '.' and 'START' keys. This move will be completed in six seconds. The X+ movement was demonstrated by the X axis display counting up to 1.0000 on the LCD screen. For a Z+ move press, in order, 'Z' '1' '.' and 'START'. The tool will ascend one inch in six seconds. For a Z- move press, in order, 'Z' '-' '1' '.' and 'START'. The tool will descend one inch. The Shadow assumes a positive entry is made unless the user enters a minus sign immediately after the axis indicator.

Continuing on, make the following entries:

X - 1 . START

Y - 1 . START

X 1 . START

Y 1 . START

These entries should have caused the tool to trace out a square with one inch sides. Now move the tool .5 inches to the left, press:

X - . 5 START

For repeated execution of a move in MDI mode press the 'START' button again, this saves re-entering the command.

RATE CONTROL IN MDI MODE

To reduce the programmed feedrate in the MDI mode use the feedrate override. Observe this procedure by pressing:

X 3 . START

Now rotate the hand wheel counterclockwise while the tool is moving and notice the rate slowing. The LCD screen will show decreasing feedrate, until 0% is reached. When the hand wheel is rotated clockwise toward 100% the 3 inch move will be allowed to finish.

RAPID TRAVERSE IN THE MDI MODE

A much higher rate, rapid rate, is accomplished by pressing '/SHIFT' before the appropriate axis. For example:

/X 2 . START

Observe that the tool moved 2 inches to the right, but at an obviously higher rate.

The established feedrate is overridden when the '/SHIFT' command is implemented with an axis command. If another axis command is used without the '/SHIFT' then the axis will move at the established lower feedrate.

When a rapid move is in progress, the Shadow will not respond to feedrate override. Even if the hand wheel is rotated counterclockwise, the movement will not slow down. The user can press 'SLIDE HOLD' and interrupt the rapid move, but when 'START' is pressed the move continues as rapidly as before. If a rapid move is interrupted with 'SLIDE HOLD' and then the feedrate hand wheel is adjusted, the move will continue at the programmed feedrate when 'SLIDE HOLD' is canceled.

TWO and THREE AXIS SIMULTANEOUS MOVES

The Shadow allows two or three axes to move simultaneously. In order to accomplish a one inch move to the right and one inch away from the user at the same time press:

X Y 1 . START

To make the tool move at a 45 degree angle to each of the three axes simultaneously press:

X Y- Z 1 . START

This makes the tool move right one inch, toward you one inch, and up one inch. The (-) key is pressed immediately after the relative axis key. Therefore, in the previous data command displayed, the Y axis is moved in the negative direction and the X and Z axes are moved in the positive directions.

PROTECT or ENABLE MEMORY PROTECTION

To select Protect or Enable memory protection from MDI press '-' and then 'INSERT'. The Protect/Enable status will be displayed as a P or E, four characters to the left of the date.

SELECTING THE FOURTH FIFTH AND SIXTH AXES

To select axes U, V or W, if present, press '/' and then 'STEP'. All subsequent axis entries will be for U, V and W until the '/' 'STEP' combination is again entered. After the combination is entered the second time, X, Y and Z will be the active entry axes. A '*' will be displayed in the axis position area proceeding

the axis group which is active.

Execute the following key strokes to set a feedrate of 15 IPM:

F 1 5. START

Observe that the new feedrate is shown on the LCD display.

The decimal point is an essential part of any numerical entry, even if the entry is in whole numbers.

As each key is entered the LCD display will indicate that the key has been pressed. Since the feedrate was set at fifteen inches per minute (15 IPM), 15.0 appears on the LCD display.

If you incorrectly enter data, (press a wrong key), in the MDI mode and START has not yet been pressed you may backspace over the last character by pressing CE (clear entry), or you can clear the entire entry by pressing the DELETE key. Since this clears the entire entry, you will need to start completely over with your data entry for that line.

The decimal point is NOT used in the numerical portion of a N, G, M or S command, but should be used in other commands to avoid confusion. All parts of a multi- axis move or of a G code are entered on the same line, with 'STORE' or 'START' as the final key pressed for that line. On these multi-part entries the system will place a space between groups for readability.

LOADING, EDITING, and RUNNING A PROGRAM

This section will begin by demonstrating the procedure to store commands in the MDI mode. These can be executed immediately by pressing 'START' or later because they are stored in the Shadow CNC's memory.

LOADING A PROGRAM

Press: 'MDI' to put the control in appropriate mode.

Press: 'F' '1' '0' '.' to establish a feedrate of 10 IPM.

Press: 'Z' '1' '.' 'STORE' to cause a Z+ move.

Press: 'M' '2' 'STORE' to tell the control to stop program execution and go to line number one.

CHECKING A PROGRAM

The following format will be used throughout this manual whenever a sample program is demonstrated:

NO: ENTRY COMMENTS

NO: tells you the line number on which the Shadow CNC has the command stored. During the loading procedure, the cursor automatically drops to the next line number as soon as a command has been STORED.

ENTRY: refers to the actual data that is being stored into the Shadow's memory.

COMMENTS: column contains helpful information that will assist you in understanding the data entries.

The following series of commands will cause the Shadow to draw a rectangle.

NO: ENTRY COMMENTS

1: F20. STORE Establishes a feedrate of 20 IPM in memory.

2: Z-1. STORE Z -, 1 inch axis move.

3: X2.3 STORE X +, 2.3 inch axis move.

4: Y1.15 STORE Y+, 1.15 inch axis move.

5: X-2.3 STORE X-, 2.3 inch axis move.

6: Y-1.15 STORE Y-, 1.15 inch axis move.

7: Z1. STORE Z+, 1 inch axis move.

8: M2 STORE End of program command, terminates execution and rewinds program to line 1.

Notice the decimal point is not used with the M command. It isn't used in an N, G, M or S command, but should be used in other commands to avoid confusion.

Now that the program is loaded it can be checked for accuracy and edited, if necessary. In order to evaluate any individual entry in the program, press N followed by the line number of the command and then START. The LCD screen of the Shadow will display the line in question. Check the data displayed for mistakes.

To check the entire program, use the STEP key to evaluate each line, by pressing: N 1 START. When given this command the Shadow returns to line number 1, the first entry in your program. If the command on line 1 is incorrect, it can be corrected by simply reloading it in the proper manner. Whenever a command is stored at any line number, it automatically erases whatever command was previously loaded there.

Press: STEP. The STEP command causes the Shadow to advance to the next line number (in this case line 2). At this point corrections can be made before advancing to the next lines of data commands.

Press: STEP until all of the program has been previewed by the programmer, compare each line with the written program.

Press: - STEP. This feature of the Shadow enables the user to step backward through the program. You must press the minus (-) key prior to the STEP key for each sequential step backward. This program back-step feature of the Shadow can also be used during the loading procedure of the program. This allows you to check on earlier entries. The back-step procedure cannot be used if the entry is not stored. Any entries not stored will need to be cleared, using the clear entry key CE or the DELETE key.

The AUTO-S(ingle) MODE will allow you to watch as each move is executed individually. At this point you can also check your written programs for accuracy.

INSERT KEY

The Shadow allows the user to change a previously loaded program by inserting additional commands. The use of INSERT does not cause any commands to be erased. Instead, all entries are moved in memory to the next higher line numbers.

To prepare for the substitution of data, press 'MDI', 'N', and the line number on which to insert the data, then press 'START'. Now press the proper keys for the additional command, and INSERT. You may also press 'INSERT' to create a blank line at the cursor on which to 'STORE' an additional command.

DELETE KEY

As with the INSERT key, the DELETE key can be used to change or edit a program. The DELETE key allows the programmer to erase a command from memory and automatically moves each subsequent entry to the next lower line number. Memory locations of the remaining program after a delete is completed will be on the line number prior to the initial location. For example, if a program end command was on line number 51 before line 42 was deleted, it is now on line number 50.

PROGRAMMABLE PAUSE

Programmable Pause (or dwell) causes the CNC system to pause for a programmable period of time from .01 seconds to 60 seconds.

To program a Pause:

Press: MDI

Press: /SHIFT T (Any time in seconds)

Press: START or STORE example: a /T 5. would pause the control for 5 seconds.

LOADING and RUNNING a PROGRAM using SIMULTANEOUS X and Y AXES

The Shadow allows a program to start at any line number.

Press: MDI

Press: N 100 START this allows the programmer to begin the program on line number 100.

As an example load the following program:

NO: ENTRY COMMENTS

100: F10. STORE Feedrate is set at 10 IPM.

101: Z-1. STORE Lowers tool to work piece.

102: Y-2.75 STORE

103: X3.1 STORE

104: YX1.375 STORE

105: X-Y1.375 STORE

106: /T30. STORE 30 second pause in the program.

107: X-3.1 STORE

108: Z2. STORE Moves tool up.

109: M0 STORE Program stop command.

The program is now loaded, but should be checked for inaccuracies by using the STEP key in the MDI mode. Once any necessary editing is completed and the program is correct, change to the AUTO-S mode and check the program. Then run it in AUTO-C.

REPEATS and SUBROUTINES

The Shadow can be programmed to repeat an identical set of moves several times using a /G command, or by using a subroutine.

A subroutine in the program refers to a block of commands stored separately from the Main Program. This saves space in the Shadow CNC's memory and reduces the need for duplication of entries. A command such as /N 200 tells the Shadow that a subroutine is located at line number 200. The command causes the CNC to branch to that specific subroutine.

Once the Shadow CNC has completed the subroutine, an end subroutine command is necessary. /N0 STORE is keyed in at the end of the subroutine to instruct the Shadow CNC to return to the main program.

To begin, press MDI and N 50 START. This tells the Shadow to go to line number 50. Begin by loading the main program:

NO: ENTRY COMMENTS

50: F15. STORE Sets feedrate at 15 IPM.

51: Z-2. STORE Z- move, lowers tool.

52: X5.9 STORE

53: Y2. STORE

54: X-1. STORE

55: Y.5 STORE

56: X-.75 STORE Line 55 and 56 make the first of five identical stair-steps.

57: /G5 STORE Repeat command, includes the number of times a series of moves is to be repeated, in this case 4 more times after the Shadow has completed the initial pass.

58: N55 STORE This is a branching command. The Shadow interprets this and executes the line number of the first move of the series to be repeated.

59: Y.5 STORE This line will only be executed after lines 55 through 57 have been executed a total of 5 times.

60: X-1.15 STORE

61: Y-5. STORE

62: Z2. STORE Raises the tool.

63: /X1. STORE X+ rapid move.

64: /Y4. STORE Y+ rapid move.

65: Z-2. STORE

66: /N200 STORE Subroutine call.

67: Z2. STORE

68: /X2.5 STORE

69: /Y-2. STORE

70: Z-2. STORE

71: /N200 STORE Subroutine call.

72: Z2. STORE

73: /Y-1.5 STORE

74: /X.5 STORE

75: Z-2. STORE

76: /N200 STORE Subroutine call.

77: Z2. STORE

78: /Y-.5 STORE

79: /X-4. STORE

80: M0 STORE Program stop command.

Line numbers 66, 71, 76 will cause the Shadow to branch to a subroutine beginning at line number 200. The following are the commands that will cause a rectangle to be drawn when the subroutine is executed:

NO: ENTRY COMMENTS

200: X.25 STORE

201: Y.19 STORE

202: X-.25 STORE

203: Y-.19 STORE

204: /N0 STORE Return from subroutine to main program.

The main program and its subroutine are now loaded. Use the following steps to check the accuracy of your programming:

Press: MDI

Press: N 50 START

Press: STEP (repeat through entire program and correct any errors)

Press: N 200 START

Press: STEP (step through the subroutine and correct any errors)

Press: N 50 START (returns cursor to line 50)

Press: AUTO-S (Repeatedly press START and check your entries for accuracy as you observe each command executed. If you find a mistake, Press MDI and make the corrections.)

NESTED SUBROUTINES

Subroutine nesting is a programming device the Shadow utilizes when the main program calls up a subroutine which then calls up a second subroutine, etc. The Shadow uses subroutines to perform the same functions at different points in the program.

A drilling pattern requires the main program to call up a subroutine that, in turn, calls up a second subroutine. This is termed nested two deep. The Shadow does not allow more than seven deep nesting. If the CNC encounters an eighth level of nesting, an error 15 (subroutine nesting) will be given.

The pattern is comprised of three identical groups of four identical holes each. The holes are to be peck drilled to a depth of .5". This means a hole is drilled in a series of small "pecks", instead of in one full-depth move. The drill is removed from the hole between pecks to permit drilling chips to escape.

The following program uses 0.1 inch pecks. The tip of the drill is assumed to be at a position of 0.1 inch above the surface of the material at the start of the program.

NO: ENTRY COMMENTS

1: G91 STORE Puts the shadow in incremental mode.

2: /X1.0 STORE

3: /N50 STORE Executes the initial subroutine.

4: /Y2.0 STORE

5: /N50 STORE Executes first subroutine a second time.

6: /X3.0 STORE

7: /N50 STORE Executes first subroutine the third time.

8: M2 STORE Program ends and returns to line one.

Lines 1 to 8 make up the main program, which positions the tool for the drilling of the first hole in each group. Lines 3, 5 and 7 call up subroutine one (commands 50-57) to move the tool from hole to hole within the group. The initial entry of subroutine one is to call up subroutine two (commands 100-110) to drill the holes. Subroutine two is nested within subroutine one.

Now, continue loading the program;

NO: ENTRY COMMENTS

50: /N100 STORE Calls up subroutine two to drill the first hole.

51: /X0.6 STORE Moves the drill into position for the second hole.

52: /N100 STORE Retrieves subroutine two the second time.

53: /Y-0.6 STORE Moves drill to third hole.

54: /N100 STORE Retrieves subroutine two the third time.

55: /X-0.6 STORE Moves drill to fourth hole.

56: /N100 STORE Execute subroutine two the fourth time.

57: /N0 STORE Return from subroutine one.

SUBROUTINE FOR PECKING HOLES

NO: ENTRY COMMENTS

100: Z-0.2 STORE Lowers drill at feedrate.

101: /Z0.2 STORE Raises drill at rapid.

102: Z-0.3 STORE

103: /Z0.3 STORE

104: Z-0.4 STORE

105: /Z0.4 STORE

106: Z-0.5 STORE

107: /Z0.5 STORE

108: Z-0.6 STORE

109: /Z0.6 STORE

110: /N0 STORE Return from subroutine two.

Subroutine two was executed four times during each of the three executions of subroutine one. The use of subroutines enabled the programmer to avoid entering identical command sequences repeatedly. Without subroutines the total number of commands would have been 142, however, with subroutines only 27 memory locations were utilized.

UNITS OF RESOLUTION - OMITTING THE DECIMAL POINT

The decimal point is NOT used for N, G, M or S commands but can be used in other commands. X, Y, and Z commands, feedrate (F), and pause or dwell (/T) commands use decimal points when entering data. If the decimal point is omitted in an axis-movement command, the Shadow unit of resolution is 0.0001. So, an X axis move of 0.5463 can be entered as X 5463, which is 5463 x .0001 inches. However, if you want the X axis move to be 5.463 you must use the decimal when entering the command or enter X 54630 without a decimal point.

In fine resolution the Shadow defines the units of resolution as: axial (X,Y,Z) .0001 inches, feedrate (F) 0.1 inches per minute, and dwell units (/T) .01 seconds.

When using these units of resolution features, be careful to check the program and edit if necessary, because the possibility of errors increases when eliminating decimal points.

ARCS

When programming arcs in the Shadow, first give the endpoint of the arc with X, Y and/or Z dimensions and then give the center point of the arc with /X, /Y and/or /Z dimensions. Lastly press STORE. The Shadow will translate I, J and K to /X, /Y, and /Z respectively during download from a computer. The radius from the start-point to the center must match the radius of the end point to the center within .0001 inches. If the Shadow is to execute the arc in absolute mode, then all dimensions of the arc must be calculated from the zero point of the part. If the arc is to be executed in incremental mode, all dimensions must be calculated from the start point of the arc. First, two examples of an arc one inch in radius blended into two sides of a hexagon with two inch sides.

NO: ENTRY COMMENTS

1: G91 STORE Puts the Shadow in incremental mode.

2: Z-0.5 STORE Lowers tool into work-piece.

3: X1.2320 Y-0.7113 STORE A 30 degree angle move 1.7113 inches long.

4: X0.5 Y-0.866 /X-0.5 /Y-0.866 STORE Endpoint of arc is inch to the right and 0.866 inches in the -Y direction from the start-point of the arc. The center point is inch to the left and 0.866 inches in the -Y direction from the start point of the arc.

5: Y-1.7113 STORE Moves the tool 1.7113 inches toward the operator.

The next example completes the same set of moves in absolute mode.

NO: ENTRY COMMENTS

1: G90 STORE Puts the Shadow in absolute mode.

2: G92 STORE Sets all active axes to a current position of zero.

3: Z-0.5 STORE Lowers tool into work-piece.

5: X1.7320 Y-1.5773 /X0.7320 /Y-1.5773 STORE Endpoint of arc is 1.732 inches to the right and 1.5773 inches in the -Y direction from the zero-point set in line 2. The center point is 0.732 inches to the right and 1.5773 inches in the -Y direction from the zero-point set in line 2.

6: Y-3.2886 STORE Moves the tool to Y-3.2886.

If one axis must change direction during the arc, then two arcs must be programmed. This holds true for either incremental or absolute mode. In the following example two 45 degree moves are blended together with a 90 degree arc.

NO: ENTRY COMMENTS

1: G90 STORE Puts the Shadow in absolute mode.

41: X0.6464 Z-0.6464 STORE Cuts a 45 degree angle into the work-piece.

42: X1.0 Z0.7929 /X1.0 /Z-.02929 STORE Cuts part of the arc between the two 45 degree moves.

43: X1.3536 Z-0.6464 /X1.0 /Z-0.2929 STORE Cuts the second portion of the arc since the tool passed through the quadrant line.

44: X2.0 Z0.0 STORE Cuts a 45 degree angle to the top right of the part.

FULL CIRCLES

In incremental mode, to execute a full circle, first enter the direction of initial tool movement followed by a zero, then enter a / followed by the direction and distance to the center of the circle.

NO: ENTRY COMMENTS

41: G91 STORE Puts the Shadow in incremental mode.

42: X-Y0 /Y1.0 STORE X-Y0 indicates a full circle in the XY plane starting with an X- Y+ move. The /Y1.0 indicates that the center of the circle is 1 inch in the Y+ direction from the start point.

In the example given, the tool starts on the edge of the circle closest to the operator and moves clockwise around the circle.

To cut full circles in absolute mode, use G2 or G3 commands, or enter G91 at the end of the circle command to execute only that instruction in incremental mode.

NO: ENTRY COMMENTS

1: G90 STORE Puts the Shadow in absolute mode.

.

.

.

42: X-Y0 /Y1.0 G91 STORE X-Y0 indicates a full circle in the XY plane starting with an X- Y+ move. The /Y1.0 indicates that the center of the circle is 1 inch in the Y+ direction from the start point since this command is executed in incremental mode.

43: X0 Y0 STORE Moves the tool to position 0, 0 since this command is executed in absolute.

SHADOW G CODES

G2/G3 QUADRANT ARCS

G2 and G3 commands describe quarter circles (90 degree arcs) that are contained entirely within one quadrant of the coordinate system. Any instruction to move a tool in a quarter circle or a full circle must have the following programming components:

radius of the circle,

initial direction of movement from the starting point,

and

direction of circular movement, clockwise (CW) or counterclockwise (CCW).

An example of milling a circular contour with a radius of 1.25" that forms a 90 degree arc clockwise from a starting point on the Y axis is:

NO: ENTRY COMMENTS

125: X1.25 G2 STORE Sets a radius of 1.25" and specifies an initial movement in the X positive direction. G2 specifies clockwise direction of tool movement.

If the program used G3 instead of G2 the 90 degree arc would be would be cut counterclockwise with an initial movement in the X+ direction.

Using these G codes to mill a half circle, program two quarter circles in succession:

NO: ENTRY COMMENTS

125: Y-1.25 G3 STORE 1/4 circle.

126: X1.25 G3 STORE Next 1/4 circle.

Using these G codes to mill a full circle, proceed the axis designation with a shift (/).

NO: ENTRY COMMENTS

125: /X1.2 G3 STORE Full circle CCW (note the /).

G10 DNC

To execute a program from an external device, i.e. direct numerical control or DNC, press 6 STORE in EXTernal mode or execute a G10 in MDI or auto modes. The Shadow will now execute and then discard the program lines it receives. In order for DNC to work correctly make sure that the CTS line is connected.

G12 & G13 HELICAL

G12 and G13 allow the user to program two axes to execute a circular motion while a third axis performs a linear move. The first two axes entries indicate direction and distance from the start point of the helix to the center point of the helix. Each of these entries is proceeded by a /. The third axis entry determines how far the linear axis moves during a complete revolution of the other two axes. This entry must be evenly divisible by .0004 inches. This entry is also proceeded by a /. The fourth entry determines the distance the linear axis actually moves. This entry is not preceded by a /. The final entry is either G12, for CW tool movement, or G13, for CCW tool movement.

In the following example the tool moves CW one fourth of a revolution in the X and Y axis while the Z axis moves up one half inch.

NO: ENTRY COMMENTS

34: /X-0.5 /Y0.5 /Z2.0 Z0.5 G12 STORE The /X-0.5 and /Y0.5 indicate the center of the helix is inch to the left of the start point and inch away in Y+. /Z2.0 specifies two inches linear move per revolution. Z0.5 indicates one half total inches of linear Z axis movement. G12 denotes clockwise tool movement.

In the next example, a half circle is cut with the X and Z axis while the Y axis moves two inches.

NO: ENTRY COMMENTS

98: /X1.0 /Z0 /Y4.0 Y2.0 G13 STORE The center point of the arc is one inch to the right of the tool (/X1.0 /Z0). The Y axis moves 4 inches per revolution of the X & Z axes (/Y4.0). The total distance traveled Y is 2 inches (Y2.0). The tool will move to the right and away from the operator (G13 = CCW).

G25 STEP-AND-REPEAT PATTERNS

A G25 command is used when the programmer wishes to perform the same operation at points of a grid. Normally the operation to be performed is an autocycle to drill or tap holes. If a / is entered before the axis designator (X and/or Y) the moves are executed at the rapid rate. Following are examples of drill autocycles used with G25 commands.

NO: ENTRY COMMENTS

78: Z-.25 G81 STORE An autocycle which lowers the tool 1/4 inch from its current position after each X or Y move. (see G81 commands).

79: /X-.5 /G5 /Y-1.0 /G3 G25 STORE /X-.5 indicates a hole to be drilled every inch in the X minus direction. /G5 indicates a pattern five holes wide. /Y-1.0 indicates a hole every inch along the Y minus axis, and /G3 indicates a hole pattern three holes deep. All moves in this example are rapid moves except the actual drilling. After the holes are completed, the tool is left above the last point in the pattern.

80: G80 STORE G80 cancels the autocycle so that holes will no longer be drilled after X or Y moves.

It is possible to skip every other point in the sequence between the start and the end. To skip the odd numbered points, omit the / before the first G, or, to skip the even numbered points, omit the / before the second G when entering the command. Omitting the / before the X and Y in the following example causes all moves to be executed at the programmed feedrate except for the withdrawal of the drill.

NO: ENTRY COMMENTS

56: Z-1.0 /T.5 G81 STORE This autocycle drills a hole to a depth one inch lower than the tool tip with a second pause before retraction.

57: Y1.0 G3 X.5 /G5 G25 STORE Y1.0 indicates one inch spacing in the positive Y direction. Omitting the / before the first G causes the Shadow to skip the odd numbered points of the grid. The points with even numbers will be drilled because the / is not omitted before the second G.

58: G80 Cancels the G81 autocycle.

Subroutines and autoroutines can also be programmed at the points of the grid. The following is an example of a G25 command programmed with a subroutine that will use a G3 command to enlarge the holes in a grid.

NO: ENTRY COMMENTS

153: /N200 G25 STORE Tells the Shadow to execute a subroutine on line 200 at each grid point during the following G25 command.

154: /X1.0 /G7 /Y2.0 /G5 G25 STORE Describes a grid seven inches by ten inches with grid points spaced every inch in the X direction and every two inches in the Y direction.

Now the subroutine on line 200.

NO: ENTRY COMMENTS

200: Z-.35 STORE Lowers the tool into the work-piece.

201: /X.25 G3 STORE The tool moves CCW in a full circle with a 1/4 inch radius starting in the positive X direction.

202: /Z-.35 STORE Rapid withdrawal from the part.

203: /N0 STORE Return from subroutine and move tool to next hole.

G26 CORNER START AUTOROUTINES

G26 commands are usually used to mill out rectangular pockets where the tool starts and stops in a corner.

NO: ENTRY COMMENTS

123: X1.0 Y2.0 G26 STORE The tool center starts in the close left corner and runs around the outside of a pocket one inch by two inches.

A zig-zag pattern can be programmed for roughing out the inside of the pocket by including an incremental entry after a dimensional entry. An example follows.

NO: ENTRY COMMENTS

145: X-1.0 Y2.0 Y.2 G26 STORE The second Y entry of .2 indicates a .2 inch spacing in the Y dimension between the steps of the zig-zags.

For rectangular pockets either the X or the Y dimension may be entered first but each incremental entry, if used, must follow the dimension entry of the same axis.

Stops can be programmed along the X axis moves with an additional X entry. The stops can be used to implement autocycles or autoroutines at points along the moves.

NO: ENTRY COMMENTS

113: Z-1.3 Z-.1 /T.25 G83 STORE This peck-drill autocycle will drill a one inch deep hole with a quarter second pause after every tenth of an inch. Once implemented it will drill a hole following every X or Y move until disabled.

114: X3.2 X.4 Y-4.5 Y-.5 G26 STORE X3.2 defines the total X dimension of the pocket. X.4 defines stops at .4 inch increments along the X axis where the holes will be drilled. Y-4.5 indicates a total Y minus dimension of 4.5 inches and the Y-.5 tells the Shadow to increment inch between zig-zag steps.

G27 CENTER START AUTOROUTINES

G27 commands are usually used to mill out circular or rectangular pockets. The tool starts in the center and also stops in the center after the pocket is completed. The outside dimensions entered into a G27 command are always one-half of the total dimension of the completed pocket (i.e. the radius from the center to the perimeter). The incremental entries are the actual distances between spirals. First, rectangular pockets:

Following is an example of an autoroutine to finish a pocket.

NO: ENTRY COMMENTS

169: X1.0 Y1.5 G27 STORE The X1.0 and the Y1.5 dimension entries indicate a rectangle two by three inches. The tool starts in the center of the pocket, moves in a half circle to the perimeter, then cuts the entire rectangular perimeter starting in the positive X direction. Then the tool describes a half circle back to the center of the pocket.

Now an example that incrementally spirals out to the perimeter for roughing out the entire rectangular pocket.

NO: ENTRY COMMENTS

157: Y1.0 Y.125 X-1.5 X-.25 G27 The Y1.0 and X-1.5 dimensional entries indicate a total pocket dimension of two inches by three inches. The Y.125 and X-.125 incremental entries indicate a 1/8 inch increment between the spirals in the Y and X directions.

For rectangular pockets either the X or the Y dimension entry may come first on the line but each incremental entry, if used, must follow the dimension entry of the same axis, and it must have the same sign.

Now, circular pockets:

G27 commands can also be used to create circular pockets. The circular pocket routines always begin with an XY (minus signs optional) which must be followed immediately by a number. The optional minus signs in the XY entry indicate the initial tool movement direction at the start of the perimeter cut. The /X or /Y (minus sign optional) indicates direction to the center when the tool reaches the perimeter. The tool always returns to the circle's center at the end of the routine via a half-circle. The example that follows is used to rough out a circular pocket with spiral passes starting in the X+, Y+ direction at the center and spiraling out to the outside perimeter. When the tool reaches the perimeter the center is in the X+ direction.

NO: ENTRY COMMENTS

136: XY0. /X1.5 /X.2 G27 STORE The XY entry signifies a circular pocket, and the 0 indicates an inside radius of zero (remember, the zero must be entered). /X1.5 defines an outside diameter of three inches. /X.2 specifies 1/5 inch between spirals.

Since initial tool movement was in the X+, Y+ direction and the center is in the X+ direction as the tool reaches the perimeter, the entire pocket was cut clockwise.

The spirals can be programmed to start between the center and the perimeter by entering a non-zero inside radius, as follows.

NO: ENTRY COMMENTS

169: XY-1.1 /Y-2.3 /Y-.05 G27 STORE XY-1.1 indicate an internal diameter of 2.2 inches before the tool starts its spiral. /Y-2.3 signifies an outside diameter of 4.6 inches and /Y-.05 indicates .05 inches between spirals.

The combination of XY- and /Y- indicate clockwise movement with the tool meeting and leaving the perimeter on the edge away from the operator.

Last, here is an example which finishes a pocket by swinging the tool out from it's center in a counter-clockwise half-circle to the right side perimeter, completing the counter-clockwise perimeter move back on the right side then swinging the tool left in a half-circle back to the center.

NO: ENTRY COMMENTS

186: X-Y0. /X-2.35 G27 STORE Initial tool movement is X-Y+, remember the zero! Direction to center after tool reaches perimeter is X- or left, and radius of pocket is 2.35 inches.

G29 EXECUTE LAST AUTOCYCLE

G78, G79, G81, G82, G83, G84, G85 and G86 are all autocycles which can be re-executed with a G29. An autocycle must be enacted by an axis move before it can be executed by a G29. G29 works even after autocycles have been disabled with a G80.

G40, G41 & G42 TOOL RADIUS COMPENSATION

G41 turns on tool radius compensation for the tool to the left of the workpiece. G42 turns on tool radius compensation for the tool to the right of the workpiece. G40 turns tool radius compensation off. In both examples following, the part path was programmed and then the actual tool radius (a positive amount) was entered in the setup page for the radius compensation.

NO: ENTRY COMMENTS

1: G90 STORE Puts the Shadow in absolute mode.

.

.

40: T400 STORE Executes a tool length offset for tool #4

41: T20000 STORE Sets up tool radius compensation for tool #2, press setup twice to change the values.

42: G41 STORE Turns on tool radius compensation for the tool to the left of the workpiece. Tool will actually move as this is executed.

43: Z-0.5 STORE

44: X-1.5 STORE

45: Y1. STORE

46: X0. STORE

47: Y-.5 STORE

48: Z0. STORE

48: G40 STORE Cancels tool radius compensation.

In the next example, a positive tool radius compensation was entered for tool 13.

When starting in the center of an inside cut, enter the G41 or G42 on the same line as the initial move so that the start of the move is not compensated but the end of the move will be.

66: T131313 Tool 13 is inserted, T.L.O. for tool 13 is used and radius comp for tool 13 is set up and waiting for the G42.

67: X1. G42 Moves tool right less than one inch so that the edge of the tool is on the circle.

68: Y-1. G2 Cuts the circle.

On line 67, the tool does not move toward the operator as it would if the G42 occurred on a line by itself.

G50 BOLT CIRCLE

To generate a bolt circle, you must first enter

/R followed by the radius of the pattern.

In the middle of the line you must enter

T followed by the number of holes in the pattern.

Last on the line enter G50.

The command starts the tool from the center of the pattern and returns it to the center after completion.

It is possible to rotate the pattern CCW, and to skip up to 8 random holes in the pattern.

The first hole will be directly to the right of the center, unless you rotate the pattern. To rotate it enter /T followed by the degrees to rotate CCW.

S must be entered before each hole to be skipped in the pattern and they must be entered sequentially.

If you enter S- and a hole number then that hole and all the following holes will be skipped.

NO.	COMMAND	COMMENTS
15:	/Z-1.0 Z-0.1 /Z-.05 G83	Peck drill cycle to be executed at each hole.
16: :	/R1.0 T4 /T15.00 G50	Hole pattern has a radius of one inch, with four holes, rotated fifteen degrees.
:		Cancel drill cycle, change tools, move to center of 2nd pattern, and set up autoroutine.
22:	/R1.0 T8 S4 G50	Hole pattern has a radius of one inch, with 8 holes, but skip hole number four

G54 Through G59 JIG OFFSETS

G54 through G59 jig offsets are now active. To use them press the setup key three times (once= Shadow installation and twice = tool offsets) then select 54, 55, 56, 57, 58, or 59, then enter the offset amounts under the correct axis.

When the Shadow encounters a G54 in the program it will look at this table and add the offset listed here to it's current position. Then when an absolute move is executed it will move according to this new calculated position. G54 through G59 all work in this manner giving the operator a total of six jig offsets to choose from plus the original G92 offset position.

To cancel the jig offset, use a G53 in the program.

G60 MIRROR IMAGE

In incremental mode, the G60 command mirrors axis movement (i.e. X-2.0 would cause a positive X axis move of 2.0 inches if the X axis was mirrored). In absolute mode, the G60 command mirrors axis position (i.e. X-2.0 would cause the tool to move to X+2.0). This command is useful for making parts that are symmetrical.

In the following example, the tool path is a diamond with two inch sides.

NO: ENTRY COMMENTS

1: G91 STORE Puts the Shadow in incremental mode.

2: /N42 STORE Execute subroutine starting on line 42.

3: Y G60 STORE Mirrors the Y axis.

4: /N42 STORE Execute subroutine starting on line 42.

5: XY G60 STORE Mirrors both the X and the Y axes.

6: /N42 STORE Execute subroutine starting on line 42.

7: X G60 STORE Mirrors the X axis.

8: /N42 STORE Execute subroutine starting on line 42.

9: G60 STORE Deactivates mirroring.

Subroutine on line 42:

NO: ENTRY COMMENTS

42: XY1.4142 STORE Moves the tool 2 inches at a 45 degree angle.

43: /N0 STORE Return from subroutine.

G61 & G62 DRY RUN

The purpose of the G61 command is to allow the operator to perform a dry run of a program. Any axes can be enabled and the enabled axes can run at the rapid rate if desired. G62 operates the same as G61 except it also inhibits M, S, and T functions.

NO: ENTRY COMMENTS

42: X Y G62 START Enables the X and Y axes and disables the M, S and T functions.

42: /X Y Z G61 START X, Y and Z axes now execute all moves at rapid, even though the program may contain feedrates. M, S and T functions will operate as normal.

42: X Y Z U V W G61 START Shadow operation returns to normal. U, V and W are only required on a six axes Shadow.

G68 CLEAR CURRENT PROGRAM

The G68 command clears the current program from the MDI page.

NO: ENTRY COMMENTS

42: G68 START Deletes all commands, programs, subroutines, etc. currently in the MDI page.

G70 & G71 ENGLISH/METRIC TEST

The G70 command tests to make sure the Shadow is in English units of measurement. The G71 command tests to make sure the Shadow is in Metric units of measurement.

NO: ENTRY COMMENTS

42: G71 STORE Results in an error code number 14 if the Shadow is in English

G72 PART SCALING

The G72 command allows the user to scale a part program to make identical parts in various sizes. Any combination of any axes may be scaled for any amount. Part scaling is disabled by: G72 STORE, executing an M2 command, or powering up the Shadow.

NO: ENTRY COMMENTS

1: X1.5 Y0.5 G72 STORE Scales the X axis moves to one and a half times the programmed moves and the Y axis moves to one half the programmed moves. The Z axis moves are still as programmed.

NO: ENTRY COMMENTS

1: X Y Z 0.25 G72 STORE Scales all three axes to one-forth size.

2: /R 0.25 G72 STORE Scales all active axes to one-forth size.

In the following example, an oval will be cut, one inch wide by two inches 5Ð Ý
²GET http://www.shadowcnc.com/shadowmanu="br2">

NO: ENTRY COMMENTS

42: X2.0 G72 STORE Scales the X axis to move twice the programmed amount.

43: /X1.0 G2 STORE Cuts a circle stretched in the X direction.

44: G72 STORE Cancels part scaling.

G75 AUTOCYCLE CLEARANCE VALUE

G75 is another way to program the R or /R clearance and can be programmed immediately after an autocycle or between moves while an autocycle is active. It generally has a /Z- move programmed to provide clearance above the part so that the tool will clear fixtures or part protrusions. When G75 is active and an autocycle is fired the G75 move is executed first then the autocycle itself, then the reverse of the G75 move is executed at rapid leaving the tool at its starting point. Here is an example of G75 clearance used with a G81 drill autocycle.

NO.	COMMAND	COMMENTS
15:	G90	Puts the Shadow in absolute mode so that moves other than G-codes will be referenced from the zero of the part.
16:	T505	Calls up tool 5 and its Z offset.
17:	/Z1.6	Positions end of tool 1.6 inches above the part
18:	Z-1.23 G81	Drills 1.13 inches down into the part, since the first .100 will cut air.
19:	/Z-1.5 G75	Provides extra clearance of 1.5 inches above part which will be taken up at rapid before G81drills the hole
20: :	/X0.5 /Y3.4	Position of the first hole.
41:	G80	Disable autocycle.
42:	/X 12.98 /Y4.535	Go to holes to the right of fixtures.
43:	G75	Cancel the clearance moves.
44:	G89	Re-enable autocycle.
45:	/Z0.1	Bring the tool down to just above the part.
46: :	/X11.645	Move X axis to next hole.

G78 MILL AUTOCYCLE

The G78 command is most commonly used for multi-passed milling in a straight line. It is only activated by programmed rapid moves. After G78 is activated; when a rapid move is encountered the move programmed with G78 is always executed at rapid. Next, the rapid move that was encountered is executed. Finally, the mirror of the G78 move is automatically executed. The move in a G78 always occurs at rapid. If the axis move portion of the G78 command is proceeded by a shift (/), then the mirrored move will be in rapid also.

In the following example, a slot is cut into a part 3.75 inches long and .25 inches deep in five passes. The tip of the bit is 0.1 inches above the part before line 41.

NO: ENTRY COMMENTS

1: G91 STORE Puts the Shadow in incremental mode.

.

.

41: Z-0.15 STORE Feeds the bit into the part in preparation for the first pass.

42: Z0.2 G78 STORE Before the /Y move is executed on line 44, the Z axis will move +0.2 inches at rapid to clear the part. Then the Y axis rapids back to the starting point as programmed on line 44. Then the Z axis feeds back down 0.2 inches.

43: X3.75 STORE This line actually mills the slot.

44: /X-3.75 STORE This activates the G78 auto-cycle.

45: Z-.05 STORE The Z axis feeds down an additional .05 inches for the next pass.

46: /G4 N43 STORE Repeat command. Line 43 will be executed a total of four times.

47: X3.75 STORE Mills the slot one last time and will not be followed by the G78 cycle.

48: G80 STORE Disables auto-cycle.

49: /Z0.35 STORE Lifts the bit to .1 inches above the part.

G79 PROGRAMMABLE CYCLE

G79 allows the programmer to make up an autocycle that will be executed after each axial move. The autocycle may consist of arcs, circles, subroutine calls, etc.

NO: ENTRY COMMENTS

42: Y0.25 G3 G79 STORE The Shadow will execute a quarter circle arc after each move.

43: X-1.0 STORE

44: X-2.0 STORE

45: X-3.0 STORE

46: G80 STORE Disables autocycles so that future moves will not be followed by a quarter circle.

In this example a subroutine is executed after each move which mills a rectangular pocket.

NO: ENTRY COMMENTS

68: G91 STORE Selects incremental mode.

69: /N100 G79 STORE Calls the subroutine at line 100 after each move.

70: /X-1.0 STORE

71: /X-2.0 STORE

72: G80 STORE Disables autocycles so that future moves will not be followed by a subroutine call.

.

.

100: Z-1.0 STORE

101: Y-.25 STORE

102: X.25 STORE

103: Y.5 STORE

104: X-.25 STORE

105: Z1.0 STORE

106: /N0 STORE

G80 DISABLE AUTOCYCLE

A G80 command is used to disable autocycles (G78, G79, G81, G82, G83, G85, and G86). G89 can be used to re-enable the last autocycle, or G29 can be used to execute the last autocycle if it has been enacted with an axis move.

G81 DRILL AUTOCYCLE

The drill autocycle G81 is used to feed the tool into the workpiece at the established feedrate with an optional pause and then extract the tool at the rapid rate. The tool can be raised an extra clearance distance above the part and then moved down to the part by entering a /R- & amount just before the G81. The clearance amount can be changed between holes with the G75command. Notice that all autocycles are programmed first, and then the tool is moved into position over the first hole.

NO: ENTRY COMMENTS

41: F10.0 STORE Establishes the feedrate at 10 IPM.

42: Z-1.0 /T1.0 G81 STORE Feeds tool down one inch, at feedrate of 10 IPM, dwells for one second then raises tool at rapid. Executed after line 43 and after every subsequent move until disabled.

43: /X0.5 STORE Executes a rapid inch X move which will be followed by a Z- one inch drill autocycle.

NO: ENTRY COMMENTS

41: F10.0 STORE Establishes the feedrate at 10 IPM.

42: Z-1.0 /R-.5 G81 STORE Moves the tool down at rapid " to the part, then feeds tool down one inch, at feedrate of 10 IPM, then raises tool 1" at rapid. Executed after line 43 and after every subsequent move until disabled.

43: /X0.5 STORE Executes a rapid inch X move which will be followed by a Z- one inch drill autocycle.

G82 BORE AUTOCYCLE

The bore autocycle G82 is used to feed the tool into the workpiece at the established feedrate with an optional pause and then extract the tool at that feedrate. The tool can be raised an extra clearance distance above the part and then moved down to the part by entering a /R- & amount just before the G82. The clearance amount can be changed between holes with the G75command. Notice that all autocycles are programmed first, and then the tool is moved into position over the first hole.

NO: ENTRY COMMENTS

41: F10.0 STORE Establishes the feedrate at 10 IPM.

42: Z-1.0 /T1.0 G82 STORE Feeds tool down one inch, at feedrate of 10 IPM, dwells for one second then raises tool at 10 IPM. Executed after line 43 and after every subsequent move until disabled.

43: /X0.5 STORE Executes a rapid inch X move which will be followed by a Z- one inch bore autocycle.

NO: ENTRY COMMENTS

41: F10.0 STORE Establishes the feedrate at 10 IPM.

42: Z-1.0 G81 STORE Feeds tool down one inch, at feedrate of 10 IPM, then raises tool at 10 IPM. Executed after line 43 and after every subsequent move until disabled.

43: /X0.5 STORE Executes a rapid inch X move which will be followed by a Z- one inch bore autocycle.

G83 PECK DRILL AUTOCYCLE

The peck drill autocycle G83 is used to feed the tool in increments into the workpiece at the established feedrate with an optional pause and then extract the tool. The tool can be raised an extra clearance distance above the part and then moved down to the part by entering a /R- & amount just before the G83. The clearance amount can be changed between holes with the G75command. Notice that all autocycles are programmed first, and then the tool is moved into position over the first hole.

In the following example the tool drops one inch using .2 inch increments at feedrate, full withdrawals and re-entries at rapid after the increments, then a rapid withdrawal.

NO: ENTRY COMMENTS

41: F10.0 STORE Establishes the feedrate at 10 IPM.

42: /Z-1.0 Z-0.2 G83 STORE The /Z-1.0 indicates a total depth of one inch, the / is optional and indicates rapid withdrawal and re-entry to the bottom of the hole so far. Z-0.2 indicates increments of 0.2 inches which will be drilled at feedrate.

43: /X0.5 STORE Executes a rapid inch X move which will be followed by a Z- one inch peck drill autocycle.

The next example uses a .01 chip breaking move, notice the sign change.

NO: ENTRY COMMENTS

42: Z-1.0 Z-0.25 Z.01 /T1.0 G83 STORE The Z-1.0 indicates a total depth of one inch, a / would indicate a rapid withdrawal. Z-0.25 indicates increments of 1/4 inch. The Z.01 indicates a chip breaking withdrawal of .01 inches. The optional /T1.0 indicates a one second dwell.

The next example uses a full withdrawal chip breaking move with rapid re-entry to .1 inches above the bottom of the hole so far, notice all signs are negative.

NO: ENTRY COMMENTS

42: /Z-1.0 Z-0.25 /Z-0.1 /T1.0 G83 STORE The /Z-1.0 indicates a total depth of one inch, the / indicates a rapid withdrawal. Z-0.25 indicates increments of 1/4 inch. The /Z-0.1 indicates a full withdrawal with a rapid re-entry to 1/10 inch above the bottom of the last peck. The next peck is 1/10 plus 1/4 inch in depth at feedrate.

In the next example, G83 is used to cut a deep slot.

NO: ENTRY COMMENTS

21: /Z-2.5 Z-.5 X3.9 G83 STORE /Z-2.5 indicates total depth of slot with rapid withdrawal after each pass. Z-.5 indicates the depth of each pass. X3.9 indicates length and direction of the slot to be cut at feedrate.

G84 TAP AUTOCYCLE

The tap autocycle command:

turns the spindle off, (in case the spindle was turning CCW),

turns the spindle on CW,

executes the moves specified with the command, (usually a Z- move),

turns the spindle off,

executes dwell if specified, (G84 is immediately proceeded with a /T {dwell time}),

turns the spindle on CCW,

mirrors moves specified with the command,

turns the spindle off.

G84 is active until disabled, and will be executed after each subsequent axis move.

The tool can be raised an extra clearance distance above the part and then moved down to the part by entering a /R- & amount just before the G84. The clearance amount can be changed between holes with the G75command.

Notice that all autocycles are programmed first, and then the tool is moved into position over the first hole.

Use the following formulae when tapping:

* 1 / threads per inch = pitch

* RPM x pitch = feedrate

* RPM / threads per inch = feedrate

NO: ENTRY COMMENTS

40: F 25. STORE Sets the feedrate to match spindle speed/threads per inch.

41: Z-0.55 G84 STORE Sets up the autocycle to tap a hole after each subsequent move until disabled.

42: /Z0 STORE Activates the tap autocycle at the current XY position.

43: /X0.75 /Y0.98 STORE Move to the next hole to be tapped.

44: G80 STORE Disables autocycle.

G85 AND G86 BORE WITH SPINDLE CONTROL AUTOCYCLE

This autocycle turns the spindle on, {CW, M3 for a G86}, {CCW, M4 for a G85}, feeds the tool into the workpiece at the established feedrate with an optional pause, turns the spindle off, and then extracts the tool at rapid. The tool can be raised an extra clearance distance above the part and then moved down to the part by entering a /R- & amount just before the G-code. The clearance amount can be changed between holes with the G75command. Notice that all autocycles are programmed first, and then the tool is moved into position over the first hole.

NO: ENTRY COMMENTS

41: F10.0 STORE Establishes the feedrate at 10 IPM.

42: Z-1.0 G86 STORE Turns the spindle on, feeds tool down one inch, at feedrate of 10 IPM, turns the spindle off, then raises tool at rapid. Executed after line 43 and after every subsequent move until disabled.

43: /X0.5 STORE Executes a rapid inch X move which will be followed by the G86 autocycle.

G89 RE-ENABLE AUTOCYCLE

A G80 command is used to disable autocycles (G78, G79, G81, G82, G83, G85, and G86). G89 can be used to re-enable the last autocycle, or G29 can be used to execute the last autocycle if it has been enacted with an axis move. The last /R or G75 clearance amount will also be re-evoked.

G90 ABSOLUTE MODE & G91 INCREMENTAL MODE

The absolute and incremental modes are independent for MDI and AUTO modes. What this means is that when executing a G90 in AUTO-C or AUTO-S mode, axis movements are measured from the zero point in the AUTO modes, however, MDI mode is not affected.

When executing a G91 in MDI mode, axis movements in MDI mode are executed incrementally from the previous position, however, AUTO-C and AUTO-S modes are not affected.

NO: ENTRY COMMENTS

1: G90 STORE Selects absolute mode, moves now measured from the zero point.

2: X1.0 STORE Moves the tool to one inch to the right of the zero point.

3: X1.0 STORE Does not move the tool since X is already at 1.0, however, will cause execution of any active autoroutine.

4: X0.0 STORE Moves the X axis left to zero.

NO: ENTRY COMMENTS

1: G91 STORE Selects incremental mode, moves now measured from the previous tool position.

2: X1.0 STORE Moves the tool one inch to the right from its previous position.

3: X1.0 STORE Moves the tool an additional inch to the right from its previous position.

4: X0.0 STORE Does not move the tool, but, will cause execution of any active autoroutine.

A G90 at the end of a command causes only the command on that line to be executed in absolute and a G91 at the end of a command causes only the command on that line to be executed in incremental.

NO: ENTRY COMMENTS

1: G92 STORE Sets the current position at absolute zero.

2: G91 STORE Selects incremental mode.

3: X1.0 STORE Moves the tool to one inch to the right.

4: X-0.5 G90 STORE Sets absolute mode for this line only so the tool moves inch to the left of zero.

5: X1.5 STORE Moves the X axis to the right 1 inches from its previous position. Now the tool is an inch to the right of the zero point.

G92 & G93 RESET ABSOLUTE ZEROES

G92, G93, G99, pressing the R key in jog mode, or turning the Shadow on, are all ways of resetting the absolute zero point. G92 resets all axes to zero except for an optional offset entered with the G92.

NO: ENTRY COMMENTS

1: X1.0 G92 STORE Sets the current position of all axes at zero except X. The current position of the X axis is one.

G93 only sets the axis given with the command.

NO: ENTRY COMMENTS

1: X1.0 G93 STORE Sets the current position of only the X axis to one point zero. The other axes are not affected.

G98 RETURN TO OFFSET

G98 causes all axes to move at rapid rate to the position where the last G92 offset was executed. If a G92 or G93 has not been entered the axes will travel to their zero position. If the Z axis' position is negative, the Z axis will run to zero first. If the Z axis' position is positive, the Z axis will run to zero last.

G99 HARDWARE RETURN TO HOME

In the set up procedure, the G99 position is defined as "undefined", "+limit", "-limit" or home . When G99 is executed, all axes defined, run to the switch specified, then back off the switch to the nearest marker pulse. The axes that are "undefined" do not move and their positions are not modified on the tracking displays.

SHADOW M-FUNCTIONS

This optional feature of the Shadow performs various procedures. M-functions can change spindle speeds and switch coolant, spindle, clamping on and off, etc.

Some special M-functions are listed below:

M0 STORE Program stop Triggers output solid-state relay, IF defined in setup, and then pauses program execution until the start button is pressed.

M2 STORE Program end Triggers output solid-state relay, IF defined in setup, and returns all M-functions to their default values, stops program execution, and resets (rewinds) the program to step one.

M3 STORE Spindle on CW If M3, M4, and M5 are all defined as ON outputs, executing any one of them will

M4 STORE Spindle on CCW turn on that output and turn off the others. Defining any one of these M-functions as

M5 STORE Spindle off a MOM turns off this feature.

M6 STORE Manual tool change Fires an M5, triggers output solid-state relay, IF defined in setup, and then stops program execution until the start button is pressed.

TOOL CHANGER AND TOOL LENGTH OFFSETS

If you use an M-function driven tool changer, these M-functions must be defined on set-up page 17: M20 (tool out), M21 (turret CW), M23 (tool in), M27 (turret home). If you have a bi-directional turret, you must define M22 (turret CCW).

The typical tool changer contains a turret with an assortment of tools assigned numbers 1 up to 96. If you call for a tool number after power-up, the Shadow will fire an M27 (turret home) before it selects the tool you have called for.

The format of the tool select command is, T (rroocc) STORE. Where cc=changer oo=offset rr=radius. The last two digits you enter after the T are the number of the tool to be selected from the turret. If these two digits are 00, then the current tool remains in the spindle. The third and fourth digits from the right, if entered, select which tool length offset value will be used (1 to 96, press setup twice to enter new values). If the third and fourth digits are omitted, the current tool length offset value will be used. If the third and fourth digits are 00, or if T0 is entered, no tool length offset value will be used.

The fifth and sixth digits from the right, if entered, select which tool radius compensation value will be used (1 to 96, press setup twice to enter new values). If the fifth and sixth digits are omitted, the current radius compensation value will be used when a G41 or G42 is encountered.

Commands for a typical tool change are depicted below.

NO: ENTRY COMMENTS

2: M5 STORE Turns the spindle off.

3: Z0 STORE Moves Z axis to zero position.

4: T0 STORE Removes tool length offset from the Z axis.

5: T 04 STORE Removes the current tool and selects tool #4 from the turret and inserts it into the spindle

6: T 0400 STORE The Shadow moves the Z axis by the difference in amount entered for tool four in the setup screen and the current amount used (set to 0 in line four above).

7: M3 STORE Turns the spindle on clockwise.

8: T 040000 STORE Sets up tool radius compensation for tool four in the setup screen.

9: G42 STORE This command actually executes the tool radius compensation, tool right of work.

Another example.

NO: ENTRY COMMENTS

5: M5 STORE Turns the spindle off.

6: Z0 STORE Moves the spindle to the zero position.

7: T0 STORE Removes current tool length offset from Z axis.

8: T141414 STORE Tool #14 is inserted in the spindle, then the Shadow moves the Z axis by the difference in amount entered for tool fourteen in the setup screen and the current amount used (set to 0 in line 7 above).

9: M3 STORE Turns the spindle on clockwise.

10: G41 STORE Executes tool radius compensation for tool number fourteen, tool left of work.

SPINDLE SPEED SELECT

For a mechanical spindle speed changer, S-numbers 1 up to 22 are the assigned spindle speeds, with each number corresponding to an increment of spindle speed (from lower to higher speed). If you call for an S-number after power-up, the Shadow will fire an M26 (RPM home) before it selects the spindle speed you have entered. M-functions M24 (RPM up), M25 (RPM down), and M26 (RPM home) must be defined on set-up page 17 for use with a mechanical spindle speed changer. With an electronic analog spindle control, S-numbers 1 to 100 select the percentage of maximum spindle speed.

EXTERNAL MODE

Pressing the 'EXT' key will place the control in the external mode of operation.

The serial interface will default to 1200 BAUD rate, but will power up at the last BAUD rate selected in setup.

To store a program to extra ram (archive), set the cursor to the first line of the program (in MDI mode), then go to EXTernal. Press 1 and STORE, the Shadow will ask you for the program number (1 to 9999) and for the last line of the program.

To load a program from extra ram (archive), first (in MDI mode) make sure the area is clear (G68 clears entire MDI program). Next, in EXTernal, press 3 and STORE, the Shadow will ask for the program number, then the cursor will disappear until loading is completed.

To set up a computer to communicate with the Shadow, use hardware handshake, 8 data bits, 1 stop bit, no parity, and make sure the baud rates match. The Shadow will translate I, J, and K to /X, /Y, and /Z while it downloads a program from a computer.

To send a program to an external RS-232 device, such as a computer, first set up the device to receive, then, (in MDI mode) set the cursor to the top of the program (usually line 1:). Next, in EXTernal press 2 and STORE, then the Shadow will ask for the ending line number.

To load a program from an external RS-232 device, such as a computer, first (in MDI mode) make sure the area is clear (G68 clears entire MDI program.) Next, in EXTernal, press 4 and STORE, the cursor will disappear until one of the following occurs:

1. A key is pressed on the Shadow.

2. An invalid character is received. (The ASCII code for the character appears in the upper left of the Shadow screen, i.e. 79 for a capital o).

3. A control-D (ASCII 19) is received by the Shadow, indicating the end of the program.

To execute a program from an external device, i.e. direct numerical control or DNC, press 6 STORE in EXTernal mode or, execute a G10 in MDI or auto modes. The Shadow will now execute and then discard the program lines it receives. In order for DNC to work correctly make sure that the CTS line is connected as shown in the following diagram.

RS232	EXTERNAL I/O	AXES
1	1 ANALOG SPINDLE OUTPUT	1 TACH-
2 RECEIVE DATA	2 Common	2 TACH +
3 TRANSMIT DATA	3 REMOTE E-STOP INPUT	3 LIMIT CW
4	4 Common	4 LIMIT CCW
5 Common	5 REMOTE START INPUT	5 ENCODER MARK NOT
6	6 Common	6 ENCODER A
7	7 E-STOP OUTPUT N.C.	7 ENCODER B
8 CLEAR TO SEND	8	8 HOME SWITCH
9	9 +5 VOLTS D.C.	9 Common
	10	10 Common
	11 E-STOP OUTPUT N.O.	11 Common
	12 REMOTE SLIDE HOLD INPUT	12 Common
	13 E-STOP OUTPUT COMMON	13 Common
	14	14 +5 VOLTS D.C.
	15 ANALOG SPINDLE OUTPUT #2	15 +5 VOLTS D.C.

DRIVE AMPLIFIER CONNECTIONS:

Following is the connection diagram for the drive amplifiers.

SHADOW 9 PIN D SHELL CONN.	WIRE COLOR	GLENTEK GA370 CONNECTION
		1 diff. In.
		2 diff. ret
	index plug	MISSING PIN index
		1 aux. in.
1 SERVO COMMAND -10V to +10V	BROWN	2 SIG. IN.
2 TACHOMETER pin 2 of 15	RED	3 TACH. IN.
3 GND. / COMMON	ORANGE	4 COMMON
		5 dcs current sense
4 GND.=NORMAL OPERATION	YELLOW	6 RT. LIMIT
5 GND.=NORMAL OPERATION	GREEN	7 LT. LIMIT
6 GND.=FAULT	BLUE	8 LOCK OUT
		9 common
		10 +15v.d.c.
		11 common
		12 -15v.d.c.
7 GND.=DISABLE DRIVE	VIOLET	13 RESET
		14 common
8 drive enable N.C. contacts	white
9 drive enable N.C. contacts	black

SETUP MODE

When the setup key is pressed, the Shadow will ask for the password to enter the setup screens. Press the 'STORE' key unless you have changed the password. The following menu will appear:

PAGE 1