Do you have a question or comment concerning the operation of your Haas machine? Do you need help with a tough programming task, or want to know a better way to produce your parts? Maybe you have a better way to do something and want to share it. Check out the Technical Forum menu below for the right solution - or the right link!
Haas owners and operators have known for years how easy the Haas CNC is, but now the word is out. An independently published market survey showed industry professionals rating the Haas control as the most user-friendly control they've worked with. We'll show you some highlights on these pages.
The cursor arrows and the PAGE UP and PAGE DOWN keys get a lot of use when you're navigating the various Displays on a Haas control. To find a particular machine setting in the Settings display, for example, you just type the setting number in the input buffer and hit the down arrow. The PAGE UP / DOWN keys, obviously, take you to either the previous or the following page in the display.
Program Review - In the PRGRM display, Program Review allows you to cursor through and review the active program on the right side of the display screen, while also viewing the same program, as it's running, on the left side of the screen. To bring up Program Review, press F4 (you must be in MEM mode).
Background Edit - This feature allows you to edit a program (in MEM mode) from the PRGRM display while a program is running. Type in the program number you want to edit (Onnnnn) and press F4. You can then do simple edits (INSERT, ALTER, DELETE and UNDO) either to an existing program, a new program or even the program that is presently running. However, edits to the program that is running will not take effect until that program cycle ends with an M30 or RESET.
Quick Zero on DIST-TO-GO Display - You can use the Distance To Go screen to quickly zero out the Position display for a reference move. When in HAND JOG mode and in the Position display, press any other operation mode key (EDIT, MEM, etc.) and then go back to Handle Jog. This will zero out all axes on the DIST-TO-GO display, and begin showing the distance moved.
To Zero the POS-OPER Display - This display is used for reference only. Each axis can be zeroed out independently, to then show its position relative to where you selected to zero that axis. To zero out a specific axis, PAGE UP or PAGE DOWN in the POSIT display to the POS-OPER large-digit display page. When you Handle Jog the X, Y or Z axis and then press ORIGIN, the axis that is selected will be zeroed. Or, you can press an X, Y or Z letter key and then ORIGIN to zero that axis display. You can also press the X, Y or Z key and enter a number (X2.125), then press ORIGIN to enter the number in that axis display.
Pressing the OFFSET key repeatedly will toggle back and forth between the Tool Length Offsets and Work Zero Offsets pages.
Entering Offsets - Pressing WRITE/ENTER will add the number in the input buffer to the cursor-selected offset value. Pressing F1 will replace the selected offset with the number in the input buffer.
While F1 will set the entered value into the offsets, F2 will set the negative of the entered value into the offsets.
Coolant Spigot Position - The coolant spigot can be programmed to move to the location entered in the Offset display (Tool Offset page, Coolant Position column). The coolant nozzle can be adjusted to one of 10 positions for each tool - position 1 is the highest, 10 is the lowest. The nozzle will shift to that position whenever an M08 or Hnn code is encountered in the program.
Clearing All Offsets and Macro Variables - In the Tool Length Offset display, you can clear all the offsets at once by pressing the ORIGIN key. The control will prompt: "ZERO ALL (Y/N)?" to make sure this is what you really want to do. If Y is entered, all the offsets in the area being displayed will be zeroed. The Work Zero Offset page (and the Macro Variables page in the CURNT COMDS display) will do the same thing. (Any Mill Control ver. 10.02 and above; any Lathe Control ver. 3.00 and above)
Up to 200 Tool Offsets - Haas mills now offer up to 200 tool offsets, double the number in previous versions. (Any Mill Control ver. 10.22 and above)
The first page of the Current Commands display shows 15 lines of the active program, as well as feedrate and spindle speed. The column on the far right shows programmed feed and speed (PGM Fnnnn, PGM Snnnn), actual feedrate (ACT Fnnnn), commanded spindle speed (CMD Snnnn) and actual speed (ACT Snnnn).
Actual speed and feed values are just that - what the spindle and feedrate are really operating at with any adjustments using the Override keys. In addition, this page shows spindle load, axis loads, surface speed, chip load, and spindle CW, CCW or STOP commands. Current axis positions are shown in the upper right corner. Change the coordinates displayed (Operator, Work, Machine, or Distance to Go) by using the cursor up and down keys.
Tool Life Management - In the CURNT COMDS display, you can PAGE DOWN to the Tool Life management page. On this page, the Usage register increases by 1 every time that tool is called up in the spindle. Enter the number of times you want that tool to be used in the Alarm column, and when the Usage number for that tool reaches the number of uses in the Alarm column, it will stop the machine with an alarm. This helps you monitor tools to prevent them from breaking and parts being scrapped.
Tool Load Management - The next PAGE DOWN in Current Commands will bring you to the Tool Load page. Spindle load condition can be defined for a particular tool, and the machine will stop if it reaches the spindle load limit defined for that tool. A tool overload condition will result in one of four actions by the control; the action is determined by Setting 84. ALARM will generate an alarm when overload occurs; FEED HOLD will do just that; BEEP will sound an audible alarm; or AUTOFEED will automatically decrease the feedrate. This also helps you monitor tools.
Clearing CURNT COMDS Values - The values in the Current Commands display pages for Tool Life, Tool Load and Time registers can be cleared by cursor-selecting the one you wish to clear and pressing ORIGIN. To clear everything in a column, cursor to the top of that column (onto the title) and press ORIGIN.
Alarm History - Pressing the right or left cursor arrow while in the Alarm display will list the last 100 alarms, with date and time. Use the cursor up arrow to see the earlier alarms. Pressing either the left or right arrow again will bring you back to the normal Alarm display.
Alarm History saved to RS-232 and Disk - This is a new feature. From the Alarm History screen, the alarm history (the last 100) can be saved to a floppy disk by entering a file name and pressing F2. Alternately, the alarm history can be sent to a PC by pressing SEND RS232. The output from either method will contain a percent sign (%) on the first and last lines. (Any Mill control ver. 10.22 and above; any Lathe control ver. 4.02 and above)
Leaving Messages - You can enter a message in the Messages display for the next person, or for yourself. It will be the first display shown when you power up the machine, IF there are no alarms other than the usual 102 SERVOS OFF alarm. If the machine was powered down using EMERGENCY STOP, the Messages display will not show up when you turn the machine on again. Instead, the control will display the active alarm generated by the emergency stop. In this case, you would have to press the ALARM/MESGS key to view a message.
Changing Parameters - Parameters are seldom-modified values that change the operation of the machine. These include servo motor types, gear ratios, speeds, stored stroke limits, lead screw compensations, motor control delays and macro call selections.
Modifying some of these functions will void the warranty on the machine. If you need to change parameters, contact Haas Automation or your dealer. Parameters are protected from being changed by Setting 7. Be sure to download and save a copy of your machine parameters so you'll have a backup if needed (refer to the LIST PROG section to see how to save your offsets, settings and parameters to a floppy disk).
The Diagnostics display is used by Haas Service technicians to check the status of the machine for diagnostics and servicing.
Zooming in - In the Graphics display, use F2 to zoom in on the graphic. After pressing F2, press PAGE DOWN to zoom in further and PAGE UP to expand the view. Use the cursor arrows to position the zoom window over the section of the part that you wish to view in close-up.
Press WRITE/ENTER to save the new zoom window, and Cycle Start to see the close-up graphic run. Press F2 and then HOME to get back to the original full table view.
Because the settings give users a great deal of powerful and helpful command over the control, we recommend reading the entire Settings section of the operator's manual. Go here for some examples of how useful they are.
To see a list of all the G and M codes available for the machine, press HELP and then the letter C. Press the letter D for a list of all the subject areas available in the Help directory; then select the subject you want by pressing the indicated letter. Press HELP/CALC again to access the calculator.
Transferring Simple Calculations - In the Trigonometry, Circular or Milling and Tapping calculator, the number in the simple calculator box (in the upper left corner) can be transferred down to any cursor-selected data line. Cursor to the register you wish to transfer the calculator number to and press F3.
Transferring Calculated Values - You can transfer the highlighted value in a Trig, Circular, or Milling data register into the calculator box by pressing F4. Use the up and down arrow keys to select the data registers, including the calculator box, and the left and right arrows to select LOAD + - * /. To enter a highlighted data value into the calculator box, LOAD must be selected when you press F4. If one of the operations is selected, pressing F4 will perform that operation, using the number in the highlighted data register and the number in the calculator box.
Transferring to EDIT or MDI - In either EDIT or MDI mode, pressing F3 will transfer the number in the calculator box (when the cursor is on the number in the box) to either the EDIT or MDI input buffer. You will need to enter the letter (X, Y or Z) you wish to use with the number from the calculator.
Circular Calculator - The Circular calculator will list four different ways that a circular move can be programmed using the values entered for a calculated solution. Four different program lines for executing the circular move will be listed at the bottom of the display. One of the four program lines can be transferred to either EDIT or MDI.
One-Line Expressions - A new feature of the Calculator display is that it will now evaluate a simple math function (previously, it was only possible to enter a number into the input line). Enter a simple, one-line expression without parentheses, such as 23*4–5.2+6/2. It will be evaluated when the WRITE/ENTER key is pressed, and the result (89.8 in this case) displayed in the calculator box. Multiplication and division are performed before addition and subtraction. (Any Mill Control ver. 9.49 and above; any Lathe Control ver. 2.24 and above)
When you press EDIT, the first display you see is the Advanced Editor, which has a number of very useful menus (see next item). Pressing the PRGRM/CONVRS key will display the program by itself, without the menus. Pressing PRGRM/CONVRS a second time will bring up the Quick Code editor, and another press brings up Visual Quick Code (VQC). Quick Code and VQC can also be accessed via the Advanced Editor Help menu.
Advanced Editor Menus - Pressing F1 in the Advanced Editor will activate the menus. Menu selections can be made with the jog handle (turning it either clockwise or counterclockwise) or with the cursor arrow keys. Press the WRITE/ENTER key to activate a cursor-selected menu item.
Undo a Simple Edit - Pressing UNDO will change back as many as the last ten simple edits that were done using INSERT, ALTER, or DELETE. Sometimes you can even edit some code, run the program, and then use UNDO to change it back - don't count on this, however! NOTE that the UNDO key does not undo program edits done in Block Edit (that is, when you've selected an entire program line or more than one line). When using Block Edit, UNDO will only deselect text.
Advanced Editor On-line Help - In the Advanced Editor, pressing F1 to access the menus also brings up on-line "Help - How to Use the Editor," displayed in the lower right corner of the screen. To scroll through the Help text, use the PAGE UP, PAGE DOWN, HOME, and END keys (the cursor arrows move you through the Adv Edit menu items, not the Help text). Pressing F1 during the use of a menu option also brings up the corresponding Help text; press F1 again to exit the Help display. (Any Mill Control ver. 9.32 and above; any Lathe Control ver. 2.16 and above)
Advanced Editor Searching - When the Search menu item "Find Text" is used and the text is found, the next press of F1 to activate the menus will automatically select the "Find Again" option. Likewise, when the "Select Text" function on the Edit menu is used, the next activation of the menus will cause the "Copy Selected Text" option to be highlighted.
Advanced Editor Block Editing - In the 80-column Advanced Editor you can select a program block, copy or move it to another location, or delete it. To start the block definition, press F1 to get into the menus, use the jog handle or the cursor arrows to select the Edit menu and the "Select Text" menu item, then press WRITE/ENTER. Another way to begin text selection is to put the cursor on the program line where you want the selection to begin and press F2. In either case, once you've defined the beginning, you then use the cursor arrows to go to the line where the selection should end, and press F2 or WRITE/ENTER. This will highlight the section you want to copy, move, or delete. Then, use the Advanced Editor Edit menu (or the EDIT hot keys) to "Copy Selected Text" (or press INSERT), "Move Selected Text" (or press ALTER), or "Delete Selected Text" (or use the DELETE key) for the selected block.
Advanced Editor Block Editing to Another Program - You can copy a line or a block of lines from one program into another. Select the program block you wish to transfer to another program Using the method outlined in the above paragraph. Then press SELECT PROG (or use the Adv Ed Program menu, "Select Program ..." item), scroll to the program you want to copy to, and press WRITE/ENTER to select it. The selected program will open up on the right side of the screen. Cursor to where you want the selected text to be placed and press INSERT. Use the EDIT key to go back and forth between two open programs on the screen (to deselect text after it's been copied, press UNDO).
Advanced Editor Quick Cursor Arrow - You can call up a cursor arrow with which to scroll through your program quickly, line by line, when you're in the Advanced Editor. For the quick cursor arrow, press F2 once; then you can use the jog handle to scroll line by line through the program. To get out of this quick-cursor mode and remain where you are in the program, just press the UNDO key. (Any Mill Control ver. 9.49 and above; any Lathe Control ver. 2.24 and above).
You can copy, move, or delete a block of lines in the same program, or move a block from one program to another. Press EDIT and then PRGRM/CONVRS once to get to the Block Editor; you will see F1-BEGBLK and F2-ENDBLK at the bottom of display. In this Editor, define a program block by first pressing F1, and then cursor to the last line you want to select and press F2. This will highlight that section of the program to copy, move, or delete. You will see prompts at the bottom of the screen: press INSERT to copy, ALTER to move, DELETE to perform that function on the selected block. You can also copy it into another program. Press LIST PROG, then SELECT PROG, cursor to where you want the selected block to go, and copy the selection into the new program by pressing INSERT.
Exiting Block Edit - You can turn off Block Edit highlighting by pressing the UNDO key; the cursor will remain where you're at in the program. UNDO will not change back an edit done in Block Edit. RESET will also turn off the block highlighting, but the cursor will go back to the beginning of the program.
Editing in Two Locations of the Same Program - In Edit mode, F4 is the hot key that displays another view of the active program for editing. The same program will be displayed on both sides of the screen, and each view can be edited alternately by using the EDIT key to switch from one side to the other. Both programs will be updated with the edits done while you're switching back and forth. This is useful for editing a long program; you can view and edit one section of the program on one side of the screen and another section on the other side.
Lower-Case Text - In the Editor, you can enter lowercase text if it's between parentheses (that is, for comments only). Press the SHIFT key first (or hold it in) and then the letter you want to be lower case (remember, this works for parenthetical comments only). When lowercase text is selected (highlighted), it will appear in caps; deselected, it returns to lower case. To type the white symbol in the upper left corner of a numeric key, press SHIFT and then the key. These symbols are used for parenthetical comments or for macros.
Program Beginning & End Format - Programs written on a PC and sent to the control from a floppy disk or through the RS-232 port must start and end with a % sign, on a line by itself. The second line in a program received via floppy or RS-232 (which will be the first line the operator sees) must be Onnnnn, a six-character program number that starts with the letter O followed by five digits. When you create a program on the Haas control the percent (%) signs will be entered automatically, though you won't see them displayed.
M19 (Orient Spindle) with a P or R Value - This feature works on any vector drive mill. Previously, the M19 command would orient the spindle to only one position - that suitable for a tool change. Now, a P or R value can be added that will cause the spindle to be oriented to a particular position (in degrees).
If a whole number is used for the value, the P command is used and no decimal point is needed. P270.001 (or any other fraction) will be truncated to P270. Also, P365 will be treated as P5. (Any Mill Control ver. 9.49 and above; any Lathe Control ver. 2.21 and above)
An M19 R123.4567 command will position the spindle to the angle specified by the R fractional value; up to 4 decimal places will be recognized. This R command now requires a decimal point: if you program M19 R60, the spindle will orient to 0.060 degree. Previously, R commands were not used for this purpose; only integer P values could be used. (Any Mill Control ver. 9.49 and above; any Lathe Control ver. 2.29 and above)
G150 Pocket Milling with 40 Moves - In the G150 command line, a P command (P12345) calls up a subprogram (O12345) that defines the geometry of a pocket. This pocket geometry must be defined in 40 moves (strokes) or less (any Mill Control ver. 11.11 and above). In software versions previous to 11.11, G150 Pocket Milling could only accommodate a subprogram with 20 moves or less.
Duplicating a Program - In LIST PROG mode, you can duplicate an existing program by cursor-selecting the program number you wish to duplicate, typing in a new program number (Onnnnn), and then pressing F1. You can also duplicate a program in the Advanced Editor, using the Program menu and the Duplicate Active Program item.
G84 or G74 Spindle Commands - When tapping, you don't need to start the spindle with an M03 or M04 command. The control starts the spindle for you automatically with each G84 or G74 cycle, and it will in fact be faster if you don't use M03 or M04. The control will stop the spindle and turn it back on again to get the feed and speed in sync. The operator just needs to define the spindle speed.
G84 Quick Reverse - This feature allows the spindle to back out faster than it went into a tapped hole. This is specified with a J code on the G84 command line: J2 retracts twice as fast as the entry motion; J3 retracts three times as fast, and so on up to J9. A J code of zero will be ignored. If a J code less than 0 or greater than 9 is specified, Alarm 306 - "Invalid I, J, K or Q" - is generated. The J code is not modal and must be specified in each block where this effect is wanted. The J value should not contain a decimal point. (Any Mill Control ver. 10.13 and above)
G84 or G74 Tapping Back into a Hole - You can go back into a tapped hole to go deeper if you have the Rigid Tapping option and if you have not moved the tool or part. Parameter 57 bit 6, REPT RIG TAP, must be set to 1 (On). Edit the Z depth to go deeper, or offset down by the amount of one thread pitch to rerun a tapped hole. NOTE: If you move, offset, or change the starting position of the part or tap and it is not equal to one pitch of the thread, you will cross-thread the hole.
G84 or G74 Peck Tapping - You can also peck tap into a hole to go deeper (for tough/hard material) if Parameter 57 bit 6, REPT RIG TAP, is set to 1 (On). Then all you would need to do is repeat the tapping cycle at the same XY location, going deeper in the Z axis on each command line. See the following examples.
G90 G54 X1.5 Y-0.5
G43 H01 Z1.0 M08
G84 G99 Z-0.25 R0.1 F22.5
G00 Z1. M09
G90 G54 X1.5 Y-0.5
G43 H01 Z1.0 M08
G84 G99 Z-0.25 R0.1 F22.5
X1.5 Y-0.5 Z-0.5
X1.5 Y-0.5 Z-0.75
G00 Z1. M09
Note: On Mill software versions12.09 and above, REPT RIG TAP has been moved from the Parameters to Setting 133. This is now an On/Off setting that is much easier for the user to change.
You can select an axis for jogging by entering the axis letter on the input line and then pressing the HAND JOG button. This works for the X, Y, Z, and A axes as well as for B, C, U, and V auxiliary axes.
Jog Keys & Feedrates - There are a number of ways to control feedrate with the Haas CNC.
Spindle Speed - Similarly, pressing the HAND CNTRL SPIN key will allow you to adjust the programmed speed by 1%, up or down, with every increment of the jog handle.
You can stop or start the spindle with CW or CCW any time you're at a Single Block stop or a Feed Hold. When you restart the program with CYCLE START, the spindle will be turned back on to the previously defined speed.
Manual Overrides for Coolant & Chip Auger - The coolant pump can be turned on or off manually while a program is running, by pressing the COOLNT button.
This will override what the program is doing until another M08 or M09 coolant command is executed. This also applies to the chip conveyor, using the CHIP FWD/STOP/REV keys.
Coolant Spigot Position - The coolant spigot position can be changed manually when a program is running, with the CLNT UP or CLNT DOWN key. This will override what the program commands until another spigot position is commanded with an Hnn or M08 command.
Chip Conveyor - The chip conveyor can be turned on or off while a program is running, either manually using the control keys or via program M codes. The M code equivalent to CHIP FWD is M31, CHIP REV is M32, and CHIP STOP is M33. You can set the conveyor cycle time (in minutes) with Setting 114, and conveyor on-time (in minutes) with Setting 115.
Actual Spindle Speed - You can verify exact spindle speed on the first page of the CURNT COMDS display. The actual speed is displayed in the bottom right corner, as well as in the far right column of the G-code list (ACT Snnnn).
Block Delete - Program blocks beginning with a slash ( / ) will be ignored - i.e., that program line will not be executed - when Block Delete is on. This takes effect four lines after the BLOCK DELETE key is pressed when cutter compensation is in use, or two lines later when cutter compensation is not in use.
Block Look-Ahead - The Haas control looks up to 20 blocks ahead for block interpretation. This is used to ensure that DNC program input is never starved, and to allow cutter compensation to have non-XY moves inserted while cutter compensation is on.
Memory Lock Key Switch - This is an option that prevents the operator from editing or deleting programs, and from altering settings. Since the key switch (if installed) locks the settings, it also allows you to lock other areas within the settings. Setting 7 locks parameters; Parameters 57, 209, and 278 lock other features. Setting 8 locks all programs. Setting 23 locks 09xxx programs. Setting 119 locks offsets. Setting 120 locks macro variables. In order to edit or change these areas, the key switch (if installed) must be unlocked and the setting turned off. (Any Mill Control ver. 9.25 and above; any Lathe Control ver. 2.23 and above)
Rapid an Axis Home - You can rapid all axes to machine zero by pressing the HOME G28 key.
You can also send just one axis (X, Y, Z, A or B) to machine zero in rapid motion: Enter the letter X, Y, Z, A or B, then press HOME G28, and that axis alone will rapid home. There is no warning to alert you of any possible collision! Care must be exercised. (Any Mill Control ver. 9.49 and above; any Lathe Control ver. 2.24 and above)
Search for a Program Command - Searching for a specific command in a program can be done in either MEM or EDIT mode. Just enter the letter code, with or without a specified value (A or A1.23), and press the up or down cursor arrow. If you enter just the letter, the search will stop at the next use of that letter, regardless of its assigned value.
Search for a Program - When in EDIT or MEM mode, you can quickly select and display another program by simply entering the program number (Onnnnn) and pressing either the cursor down arrow or F4.
TOOL OFFSET MEASURE and PART ZERO SET - Use these keys to enter either a tool length offset or a work offset, to help save time during part setup. The NEXT TOOL key is then used to send the machine home for a tool change to the next tool. The cursor will then move to the next offset register, and the increment for the handle will go back to 10.0 inches per minute.
Rotate Tool Carousel - You can rotate the tool carousel without changing tools by using M39 and Tnn. This can be used to recover from some unusual conditions. However, it will also tell the control that there is a different tool in the spindle, which may not be the case. You can disable this command by turning on Setting 86 (M39 Lockout). (Any Mill Control ver. 2.3 and above)
Tool Change Command - It is not necessary to turn off the coolant, stop the spindle, or move the Z axis prior to a tool change (M06). The control will do this for you. When the Haas CNC reads "M06," it will:
Transferring an MDI Program - You can transfer and save a program from MDI to your list of programs. When in the MDI display, make sure that the cursor is at the beginning of the MDI program. Enter a program number (Onnnnn) that's not being used. Then press ALTER, and this will transfer the MDI data into your list of programs under that program number.
This feature allows the operator to interrupt program execution, jog away from the part to perform a desired task, and then return to the interruption point and resume program execution. Once RSJC is initiated, the operator is able to stop and start the spindle, jog the XYZ axes individually (axes other than X, Y, and Z cannot be jogged), or command a tool release. The following describes the RSJC procedure. (Any Mill Control ver. 11.10 and above)
Because the settings give users a great deal of powerful and helpful command over the control, we recommend reading the entire Settings section of the operator's manual. Listed below are some of the most useful settings.
Scrolling through Settings with Jog Handle - The jog handle can now be used to scroll through the settings. In previous versions, the jog handle could be used to scroll through (cursor-highlight) the parameters, but not the settings. This has been corrected. (Any Mill Control ver. 10.15 and above; any Lathe Control ver. 3.05 and above)
Setting 1 - AUTO POWER OFF TIMER - This turns the machine off after it has been idle for the number of minutes defined in this setting.
Setting 2 - POWER OFF AT M30 - This will power off the machine when an M30 command is executed. In addition, for safety reasons, the control will turn itself off if an overvoltage or overheat condition is detected for longer than 4 minutes.
Setting 8 - PROG MEMORY LOCK - When this is Off, program memory can be modified. When this setting is turned On, memory edits cannot be done and programs cannot be erased.
Setting 9 - DIMENSIONING - This allows the user to choose inch or metric dimensioning, which will change all Offset values and Position displays accordingly. This setting will not change program dimensions to or from inch or metric.
Setting 15 - H & T CODE AGREEMENT - When this is Off, no special functions occur. When it's On, a check is made to ensure that the H offset code matches the tool presently in the spindle. Usually you have one offset per tool, and it's usually the same number as the tool number. If it is not the same and this setting is On, you will get an alarm: "H and T Not Matched." This check can help prevent crashes. If you need to use a different offset number or more than one, this setting will need to be switched Off. In program restart, this check is not done until motion begins.
Setting 31 - RESET PROGRAM POINTER - When this is On, the RESET key will send the cursor back to the beginning of the program.
Setting 36 - PROGRAM RESTART - When this setting is Off, starting from anywhere other than the beginning of a program or a tool sequence may produce inconsistent results. When it is On, you are able to start a program from the middle of a tool sequence. Cursor onto the line where you want to start and press CYCLE START. The control will scan the entire program to ensure that tools, offsets, G codes, and axis positions are set correctly before starting or continuing from the block where the cursor is positioned. Note: Some alarm conditions are not detected prior to motion starting. It's best to turn this setting Off when not in use.
Setting 77 - SCALE INTEGER F - This can be used to change how the control interprets a feedrate. A feedrate that is entered in your program can be misinterpreted if you do not enter a decimal point in the Fnn.nn command. The selections for this setting are DEFAULT, which assumes a 4-place decimal if no decimal point is entered (i.e., if you enter F10, it assumes you mean 0.0010); INTEGER, which assumes a whole number (enter an F10, it assumes 10.0); or .1 (enter F10, it assumes 1.0), .01 or .001 (you get the idea), or .0001, which is the same as the Default setting.
Setting 84 - TOOL OVERLOAD ACTION - This is used to determine tool overload conditions as defined by the Tool Load monitor page in the Current Commands display (use page down in Current Commands to get there). A tool overload condition can result in one of four actions by the control, depending on Setting 84. ALARM will generate an alarm when overload occurs; FEED HOLD will cause a feed hold; BEEP will sound an audible alarm; or AUTOFEED will automatically decrease the feedrate.
Setting 85 - MAX CORNER ROUNDING - This setting is used to set the corner rounding accuracy required by the user. The accuracy defined in Setting 85 will be maintained even at maximum feedrate - the control will only slow at corners when it is needed. This setting defeats all the years of discussion by competitors who say you need multiple blocks of look-ahead. The Haas control actually does look ahead for block interpretation, up to 20 blocks. This is not needed for high-speed operation. It is instead used to ensure that DNC program input is never starved, and to allow non-XY moves to be inserted while Cutter Compensation is on.
Setting 88 - RESET RESETS OVERRIDE - When this is On, the RESET key sets all overrides back to 100%.
Setting 101 - FEED OVERRIDE > RAPID - When this setting is Off, the machine will behave normally. When it is On and HANDLE CONTROL FEEDRATE is active, the jog handle will affect both the feedrate override and the rapid rate override simultaneously. That is, changing the feedrate override will cause a proportional change to the rapid rate. The maximum rapid rate will be maintained at 100% or 50%, according to setting 10. (Any Mill Control ver. 10.22 and above. Any Lathe Control ver. 4.11 and above)
Setting 103 - CYC START / FH SAME KEY - This is really good to use when you're carefully running through a program. When this setting is On, the CYCLE START button functions as the Feed Hold key as well. When CYCLE START is pressed and held in, the machine will run through the program; when it's released, the machine will stop in a feed hold. This gives you much better control when testing a new program. When you're done using this feature, turn it Off. This setting can be changed while running a program. It cannot be On when Setting 104 is On (when one of these is turned on, the other will automatically turn off). (Any Mill Control ver. 9.06 and above; any Lathe Control ver. 4.11 and above)
Setting 104 - JOG HANDL TO SNGL BLK - When this is On and you are running a program in MEM mode, in the Program or Graphics display, you can use the SINGLE BLOCK key to cycle through your program one line at a time, with each press of the CYCLE START button. Again, this works either when the machine is running or you're in Graphics. Also, if you first press the CYCLE START button, then each counterclockwise click of the jog handle will step you through a program line. Turning the handle clockwise will cause a feed hold. This setting can be changed while running a program. It cannot be On when Setting 103 is On (when one of these is turned on, the other will automatically turn off). (Any Mill Control ver. 9.06 and above. Any Lathe Control ver. 4.11 and above)
Setting 114 - CONVEYOR CYCLE (MIN) - If this is set to zero, the conveyor will operate normally. If a number is entered, it defines how long (in minutes) each cycle will be when the chip conveyor is turned on. The chip conveyor cycle is started with either an M code (M31 or M32) or with the control CHIP FWD and CHIP REV keys. It will stay on for the time defined in Setting 115, then turn off and not restart until the cycle time in Setting 114 has elapsed. Short programs looped (M99) many times will not reset the chip conveyor if the intermittent feature is activated. The conveyor will continue to start and stop at the commanded times.
Setting 115 - CONVEYOR ON TIME (MIN) - This setting works with Setting 114, which defines the conveyor cycle time. Setting 115 defines how long the chip conveyor will stay on during each cycle.
Setting 118 - M99 BUMPS M30 CNTRS - When this setting is On, an M99 command (used to run a program repeatedly) will activate the M30 counters that are in the CURNT COMNDS display (page down twice). Note that an M99 will only activate the counters when it is used in a loop mode in a main program, not a subprogram. An M99 that's used as a subprogram return, or with a P value to jump to another part of the program, won't be counted. (Any Mill Control ver. 9.58 and above; any Lathe Control ver. 3.00 and above)
Setting 130 - TAP RETRACT SPEED - This feature augments one introduced in version 10.13, the quick reversal out of a G84 rigid-tapped hole. If Setting 130 is set to 0 or 1, the machine behaves normally. Setting it to 2 is the equivalent of a G84 command with a J value of 2; that is, the spindle will retract twice as fast as it went in. If it is set to 3, the spindle will retract three times as fast. NOTE that specifying a J value in a G84 command for rigid tapping will override Setting 130. (Any Mill Control ver. 10.18 and above).
Setting 144 - FEED OVERRIDE–>SPINDLE - This feature is intended to keep the chip load constant when an override is applied. When this setting is Off, the control behaves normally. When it is On, any feedrate override that is applied will be applied to the spindle speed also, and the spindle overrides will be disabled. (Any Mill Control ver. 11.10 and above; any Lathe Control ver. 4.11 and above).
Program Format to Receive - You can receive program files from a floppy disk or the RS-232 port on the Haas control. A program must begin and end with a line containing only a % sign. The next line must begin with the letter "O" followed by the program number (newer machines use five digits, older machines four). If you want to identify a program by name as well as program number, enter the name between parentheses (Program Name), either on the same line as the program number (after the number) or on the next line. The program text name will show up with the program number in the list of programs.
Loading Programs from Disk - You can load program files from a floppy disk using the I/O menu and the DISK DIRECTORY item of the Advanced Editor. Pressing WRITE/ENTER when this menu item is selected will display a list of the programs on the program disk. Use the cursor arrow keys or the handwheel to select the file you need to load, and press WRITE/ENTER. After loading that file, the disk directory will remain on display to allow more files to be selected and loaded into the control. RESET or UNDO will exit this display.
SEND RS232 or SEND DISK - You can send programs to the RS232 port or a floppy disk from the Advanced Editor. After selecting the menu item you want (SEND RS232 or SEND DISK), a program list will appear. Select the program you want to save, or "ALL" (at the end of the list) if you wish to send all programs under one file name. Select any number of programs using the up and down cursor arrow keys or the handwheel plus the INSERT key to mark the specific programs to send. If no programs are selected from the list using the INSERT key, the currently highlighted program will be sent.
Sending a Program File - You can send a file or files to a program disk or through the RS-232 port from the LIST PROG display. Use the cursor arrow to select the program you want, or select "ALL" if you want to send all of the programs under one file name. When you press F2 to send the selected program(s), the control will ask for a file name, which can be up to eight characters long with a three-letter extension (8CHRCTRS.3XT). Then press F2 again to send it. (You can also use the I/O menu in the Advanced Editor to send and receive program files.)
Sending Multiple Program Files - Several programs can be sent through the RS-232 serial port from the LIST PROG display, by typing in all the program numbers together on the input line without spaces. Each program number should start with the letter O, and you can leave off any leading zeros if you choose (e.g., O123O4545O13579). Then press SEND RS232.
Send and Receive Offsets, Settings, Parameters and Macro Variables - You can save offsets, settings and parameters to a floppy disk, retrieve them from a floppy, and send/retrieve them via the RS-232 port. To send, press LIST PROG first, then select an OFFSET, SETNG or PARAM display page. Type in a file name, and then press F2 to write the display information to disk (or F3 to read that file from a disk). Press SEND RS232 to send the display page to the RS-232 port under the file name you entered, or RECV RS232 to read the file via RS-232. You can also do this with macro variables by first pressing LIST PROG, then selecting a macro variable display page (PAGE DOWN from CURNT COMDS).
Deleting a Program from a Floppy Disk - Haas machines allow you to delete files from a floppy disk. (Note that this requires the latest floppy driver EPROM chip version FV 2.11.) Go to the LIST PROG display page and type "DEL
RS-232 Communications Using X-Modem - If you are seeing occasional errors when using RS-232 communications, X-Modem (Setting 14) is a standard communications mode which is very reliable when only a few errors occur. Our control supports this, as do almost all software communication packages for PCs.
Haas Rotary Table Using the Serial Port and Macros - It is possible to regulate a Haas rotary table using the serial port and macros from the Haas control (or any Fanuc-compatible control). There is a set of sample macros available from the Haas Applications department.