This command allows you to specify the z axis position for the upper and lower wire guides (in the part reference system) and the wire contact length.
|
Description: |
This command defines a relationship between the machine reference system zero point and machine coordinate system zero to be used in coordinate value calculations.
|
|
Parameter Definitions: |
"AXIS,+n" defines the signed delta distances from the machine coordinate system zero point to the machine reference system zero along the X,Y, or Z axes. Signs are determined by the part coordinate directions. Figure 1-9 Machine Coordinate System Zero
|
|
Considerations: |
The Machine Reference System Zero is the center of rotation of the rotary table. If there is no rotary table, Machine Reference System Zero and Machine Coordinate System Zero are the same location. |
None
|
Description: |
For Wire EDM, this command will set the parameters for wire feed heads and the wire contact.
|
|
Parameter Definitions: |
1. "UPPER,a" specifies the z axis position (a) for the upper wire guide in the part reference system. 2. "LOWER,b" specifies the z axis position (b) for the lower wire guide in the part reference system. 3. "LENGTH,c" specifies the wire contact length.
|
|
Considerations: |
SET/LENGTH,c provides the same functionality as SET/HEIGHT,h and is only used for 4 axis Wire EDM machine tools. For more information on SET/HEIGHT,h see that discussion. |
Same
This option allows you to define the codes and formats required for the surface feet per minute GPM output. This option is used primarily for lathes. You can specify the Word Address formats for the spindle SFM code and the spindle SMM code. You have the following options for SFM output:
Should All CSS Data Be Output In One Block? - toggles between YES and NO.
G Code For CSS Mode - Enter the validity and value for the spindle speed SFM output mode G code.
Max RPM For Constant Surface Speed - This option allows you to specify the Word Address format for the MAXRPM value and the MAXRPM default value.
G Code To Go Out With MaxRPM - This option allows you to specify the validity and value of MAXRPM G code. This is usually G92.
G Code To Inhibit SFM During Rapid Moves - This option allows you to specify the G code that the GPM outputs to prevent spindle speed change during rapid moves. SPINDL/SFM,...,AUTO must be programmed to activate the SFM inhibit code for Rapid moves.
G Code To Cancel SFM Inhibit - This option allows you to specify the G code to cancel the previous option.
Radius Or Diameter Required For CSS Startup - This option allows you to specify whether the SPINDL/SFM,...RADIUS,r value is output by the GPM as a RADIUS, DIAMETER, or is not required. If you specify RADIUS or DIAMETER, then you must also specify the Word Address format for the radius value and whether this code is output in the G92 block or the G96 block.
The radius value establishes the initial radius to be used for CSS mode. The radius is the distance from the current location of the tool tip to the centerline. If the radius is not programmed, the GPM uses the current tool tip radius for the initial RADIUS. If "X" output is in diameters, the start up radius is output as a DIAMETER.
Should GPM Output Calculate G97 RPM Block Before SFM - This option directs the GPM to output an RPM block (G97) calculated for the next cut radius before a programmed SFM block. This is useful in allowing the part to achieve proper speed when moving from the tool change position to the first cut position. Also, if your control inhibits RPM changes during rapid moves the RPM should be at the correct speed for the first cut. Otherwise you might want to program the SPINDL/SFM command after you have moved to the correct radius for the first cut.
G95 Needed Prior To G96 Block - This option insures that the controller is in the IPR mode for SFM. The GPM automatically outputs a G95 with an IPR based on the SFM at the first cutting radius immediately prior to the G96 block.
You can either specify the Range Change Data for all ranges or Range Change parameters for a specific range.
This option allows you to specify the codes that the GPM outputs to change spindle speed ranges. You can specify the Range Change Data option and you have the following options:
Number Of Ranges - Enter the number of spindle speed ranges for your machine tool. If you specified that a spindle table was required for RPM values, the number of ranges you specified appears as the current status.
Is Dwell Required For Range Change - This allows you to specify the amount of DWELL time between spindle changes.
Are M Codes Valid For Range Selection - This allows you to specify the M code that the GPM outputs to change spindle speed ranges.
Is Range Code Combined With RPM Code? This allows you to specify that the GPM should combine the range code with the RPM code. For example, Range 2, 500 RPM is output as S2500.
Is Range Code Combined With S Dir Code? - This allows you to specify that the GPM should combine the range code with the spindle direction code. One M code determines both the direction and the range.
For example:
M31 means range 1, CLW (Note: 3=CLW and 4=CCLW.)
M32 means range 2, CLW.
M41 means range 1, CCLW.
M42 means range 2, CCLW.
Must Range M Code Appear In RPM S Code Block? - This allows you to specify that the GPM should output spindle direction code in the block before the S code.
The GPM outputs only one M code per block unless the USERCM/ command is programmed. If the direction code is not specified to be output before the S code block when a range code is required, then the direction code is output after the S code block.
Are RPM Codes Restricted To Odd? (Even?) - This allows you to specify that the GPM should force the S codes in Range 1 to be odd and in Range 2 to be even.
Does Sign Of S Code Determine Range Selection - This allows you to specify that a + or - character determines the spindle ranges.
This option allows you to specify information for each of the ranges previously selected. You can specify the Range Code for each range, and set the Maximum and Minimum RPM for each range.
If you have previously specified that S codes must be odd or even, then you must specify whether each range is odd or even.
This command allows you to output code to control the tool at corners in order to remain within tolerance. This prevents, for example, overshooting end points at sharp corners. This option pertains primarily to those controls with inadequate corner control. Most machines do not need this option. These codes are output automatically by the GPM depending upon the options chosen and the change of direction between the current and next motion.
|
Description: |
This command generates code to control deceleration.
|
|
Parameter Definitions: |
1. "ON" causes the feed rate to decelerate to zero velocity at the end point of all contouring moves. 2. "OFF" cancels the deceleration of the feed rate. 3. "AUTO" causes the feed rate to decelerate to zero velocity at the end point of a move if the next motion vector is greater than "d" degrees change of direction. 4. "d" specifies the angle of direction requiring deceleration. If not specified, 3 degrees is assumed.
|
|
Considerations: |
1. AUTO establishes deceleration, but only for the motion block in which it appears. Forward analysis determines when to inhibit deceleration. 2. The feed deceleration code applies only to contouring operations. 3. OFF cancels deceleration. |
None
You can specify the following options:
Are Slowdown Codes G Codes - This option allows you to define whether the SLOWDN command output is either a G code or some other Word Address format. If you specify that G codes are used you can specify the following:
Code For Slowdn/On (Decel Active) - This causes slow down at the end of every linear and circular motion. Enter the code for SLOWDN/ON. This code is modal, staying active until a SLOWDN/OFF command is programmed.
Code For Slowdn/Off (Decel Cancel) - This allows the machine to position using its own continuous motion method at the end of every linear and circular motion. Enter the code for SLOWDN/OFF. This code is modal, staying active until a SLOWDN/ON command is programmed.
Non-modal Code For Slowdn - This is the G code for SLOWDN/AUTO. It is effective only for the block it appears in. Enter the code that the GPM is to output when the angular change in direction of motion exceeds the specified number of degrees.
The following option defines whether the non-modal G code is output when the change of direction exceeds or does not exceed the maximum angle.
Function Of Non-modal Code - the non-modal can either CAUSE DECELERATION or PREVENT DECELERATION depending upon the control. The control causes deceleration at the end of every motion unless the non-modal code appears.
If you specify that a code other than a G code is used you can specify the Word Address for that code. This code functions as a non-modal G code - it can cause or prevent deceleration.
Maximum Angle Before Deceleration Activated - This is the angle that determines whether non-modal deceleration is necessary. (For lesser angles there is no deceleration.) The angle can be either the Non-modal Code For Slowdn or the code other than a G code.