|
|
|
 |
|
 |
|
|
|
|
| |
Back to Main Control Tips Page
CONTROL TIPS - EDITING - for getting the most out of your Haas CNC.
EDIT Mode - Advanced Editor
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).
Block Editing
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.
Programming
 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.
Tapping
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.
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.
|
|
|
|
|
|
|
