This command allows you to specify how the GPM outputs code to control the lathe head, turret index, tool adjust, tool offsets, and coordinate parameters.
|
Description: |
This command generates code to select the turret and the assignable offsets used.
|
|
Parameter Definitions: |
1. "FACE,n" defines the turret position number for the turret. 2. "ADJUST,a" defines one of the offset switch pairs that is output with the tool code. Zero (0) will output zeros to cancel selectable tool offsets. 3. "ADJUST,ON" will re-instate the last selected offset register. If no offset register has been selected, the default value will be output. If offset registers are not programmable, the "ON" G code will be output. 4. "ADJUST,OFF" will output code to cancel the offsets. 5. "PLUS" or "MINUS" will output appropriate G code. 6. "XOFF,+c" defines the signed distance from the turret reference point to the tool tip along the machine Z axis (centerline). 7. "YOFF,+d" defines the signed distance from the turret reference point to the tool tip along the machine X-axis (diameter). 8. "ZOFF,+z" defines the length in inches or millimeters of the replacement tool. This command is only meaningful if production center mode has been enabled in the MDF and mill mode is in effect. 9. "CLW" and "CCLW" specify clockwise and counterclockwise turret indexing, respectively. If this parameter is not specified, the postprocessor will determine the direction of shortest rotation. 10. "FRONT", "REAR", "SIDE", and "SADDLE" define the turret to be used. 11. "TLANGL, a RADIUS,r is used to specify the location of the "imaginary tool tip" relative to the center of the current tool. TLANGL, a, RADIUS,r offsets the tool by "r" amount on the 0,90,180,270 degree directions, and by r times the square root of 2 in the 45,135,225,315 degree directions. See Figure 1-10. Figure 1-10 Examples Parameter Definition 11
|
|
Considerations: |
1. This command is applicable only to lathes. 2. Unless explicitly stated otherwise in the parameter definitions, any parameter not present in the input statement will be assumed to have not changed from the previous input and will be used as a modal value. At the startup, all numerical parameters are assumed to be zero except for turret position number 1. 3. A FROM is not output but should be given prior to the first selected TURRET so the tool tip position can be determined. The postprocessor will offset for subsequent turret changes when XOFF and YOFF are programmed. 4. "XOFF" and "YOFF" values are programmed relative to the part coordinate system. 5. The last TURRET indexed will be used with subsequent motion. 6. TLANGL 0 is in +X part coordinate direction. The angles get bigger in the CCLW direction. 7. The MDFG allows you to designate any valid vocabulary word for the turret names. Figure 1-11 Examples of Tool Tip Reference Points |
NOTE: Several of the TOOLNO and TURRET parameters are identical. The values given for TURRET override the TOOLNO stored values.
NOTE: This command works in conjunction with the TOOLNO command. The TOOLNO command stores the tool parameter information (FACE, XOFF, YOFF, and ADJUST) that is activated by using the corresponding TURRET number. For Example: TOOLNO/3 is activated by TURRET/FACE,3.
Parameter Definitions:
1. "a" is FACE,n. "b" is ADJUST,a. "c" is XOFF,c. "d" is YOFF,d.
After you select TURRET you have the following choices:
Heads
Adjust
Turret Miscellaneous
You can specify either one or two heads. In either case, you must specify the Word Address format for the tool code.
When you specify one head, you select one head you have the following choices:
Maximum and Minimum Face Number - Enter the maximum and minimum turret face positions.
When you specify two heads, you have the following choices:
Max Face Number Independent Head - Enter the maximum turret face positions for independent head.
Min Face Number Independent Head -Enter the minimum turret face positions for independent head.
Max Face Number Dependent Head - Enter the maximum turret face positions for dependent head.
Min Face Number Dependent Head - Enter the minimum turret face positions for dependent head.
Name Of Dependent Or Independent Head - Enter the name as either FRONT, REAR, SIDE, SADDLE, RIGHT, Left, or OTHER (and define your own.) When you select OTHER, you must enter a Vocabulary Word and enter the value which represents the integer word code.
Two Turret Lathe Head Control - You can specify whether the two heads are a fixed distance apart and have one tracking point, or whether they are controlled independent and are merging.
X and Y Distance To Dependent Head - Enter the distance from the independent to dependent head. These are only selectable if you select non-merging heads. The GPM adds this distance to every dependent head Goto point.
Reverse Circular G Codes For Dependent Head - You can specify whether GPM should switch G02 to G03 and G03 to G02.
Mirror Cl Data About Z Axis For Dependent Head - You can specify whether GPM should mirror (X coordinates) about Z.
Refer to the ADJUST section of the command LOAD for a description of this option.
When you select this option, you have the following options:
Indexing Direction - You can specify the following Turret Index Direction parameters:
Is Index Direction Tape Controlled - This option allows you to specify whether or not the indexing direction is controlled by the tape input or by the operator/machine tool. If you specify No, then you cannot specify any other indexing parameters.
Does Sign (or M Code) Control Index Direction - This option allows you to specify whether the index direction is controlled by a plus or minus sign or by M codes. You cannot specify both.
When you select Sign then you must indicate whether a + or a - determines clockwise rotation. This determines the codes for indexing and you cannot specify M codes.
When you select M code then you can specify an M codes for clockwise or counter-clockwise index for the independent or dependent head.
Output Index Direction M Code Before The Face Code - You can specify whether GPM should output the direction M code before the Face (T) code.
Indexing Time Factors - You can specify the time (in minutes) that the GPM adds to the current machine time for changing heads, indexing to the first face, and indexing to each additional face.
Coordinate Output Considerations - You have the following options for specifying lathe output coordinates:
The Output Coordinates Track - There are two methods for determining lathe output coordinates. They toggle between TURRET REFERENCE and TOOL TIP. The tool length offsets are the distances from the turret reference point to the tool tip. They are specified as XOFF and YOFF in the TURRET command.
Tracking Turret Reference Point - This method adds the tool length offsets to each Goto.
Tracking Tool Tip (center of Tool Nose) - This method outputs a Reset (G92) block to establish new tool offsets. The tool offsets are applied only at the reset block. When the TURRET command is used, the tool is assumed to be at its home position.
The G92 block =
the present coordinates:
- the previous tool offsets
+ the new tool offsets
The Initial From Point Represents - This defines the FROM position. This is used for the first tool change. This position is used as the present coordinates (in the previous equation) when tracking Tool Tip. This toggles between TOOL TIP and TURRET REFERENCE.
Apply Tlangl,a,Radius,r To The Output Coordinates - This allows you to specify whether the offset determined by TLANGL,a,RADIUS,r should be added to the output coordinates.
Output Reset Coordinates With The Turret Data - This allows you to specify whether a Reset block is output. This prevents the G92 block from being output when you use the Tool Tip method.
Apply Atangl,a,Radius,r, To The Reset Coordinate - This option allows you to specify whether the offset determined by TLANGL,a,RADIUS,r should be added to the coordinates in the Reset block. If you do not use a Reset block, you cannot use this option.
Two Minor Words are used to define the imaginary tool tip in the turret command. RADIUS is used to define the tool nose radius. TLANGL is used to specify the direction that the tool points, which determines whether the RADIUS is to be added to or subtracted from the incoming CLSF point. Starting with zero degrees in the positive X direction in the part coordinate system and going counter-clockwise in forty-five degree increments, the possible values for TLANGL are 0, 45, 90, 135, 180, 225, 270, and 315.
All incoming CLSF coordinates are transformed in X and Y by the length of the tool nose radius. The signs for the X and Y components of the radius are determined by the programmed tool angle. The points that are output are the actual points on the part (the same as would appear in the CLSF if the cutter diameter were zero.)
When tracking is based on the imaginary tool tip, you can program tool length offsets specifying the distance from the turret reference point to the tool tip (center of the tool nose, not the imaginary tool tip) as XOFF and YOFF in addition to the tool angle and tool nose radius. In this case, the XOFF and YOFF are applied in a reset (G92) block as described above, and the tool nose radius is used to transform the CLSF coordinates.
Does T Code Require A Dwell? This option allows you to specify whether the GPM outputs a DWELL with the T code output for the turret requires a machine tool dwell.
Does Turret Indexing Require An M Code? - This option allows you to specify an M code for turret indexing.
Does Turret Indexing Require A G Code? - This option allows you to specify a G code for turret indexing.
Should Turret Force Alignment Block? - If you choose this option you have the following choices:
Current Position In Tool Change Block - toggles between YES and NO. YES causes the GPM to output the current Goto point position in the alignment block which follows the TURRET command.
Turret Direction M Code - toggles between YES and NO. YES causes the GPM to output the Turret direction M code in the alignment block which follows the TURRET command.
Absol/Incr Mode G Code - Toggles between YES and NO. YES causes the GPM to output the G Code for the current coordinate mode (absolute or incremental) in the alignment block. NO suppresses output.
Spindl Speed & Direction Codes If On - Toggles in between YES and NO. YES causes the GPM to output the SPINDL speed and direction if the SPINDL is on. NO suppresses output.
Cutter Compensation Code - Toggles in between YES and NO. YES causes the GPM to output the code for cutter compensation G code. NO suppresses output.
Feed Rate Mode G Code - Toggles between YES and NO. YES causes the GPM to output the G Code for the current feed rate mode in the alignment block. NO suppresses output.
Motion G Code - Toggles between YES and NO. YES causes the GPM to output the current motion G code in the alignment block. NO suppress output.
Coordinates Of - Toggles between NEXT GOTO POINT or CURRENT POSITION. Next Goto Point causes the GPM to output the values in the next Goto point in the current alignment block. Current Position causes the GPM to output the coordinates of the current position in the alignment block.
Current Feed Rate - Toggles between YES and NO. YES causes the GPM to output the current feed rate in the alignment block. NO suppresses the feed rate output.
Coolnt Code If Coolnt On - Toggles between YES and NO. Yes causes the GPM to output the current COOLNT command if the COOLNT is on. NO suppresses output.
Usercm - Toggles between YES and NO. Yes allows you to specify which of the usercm output buffers are output by the GPM during the TURRET alignment block.