Understand the tool compensation function of CNC lathe processing in one article
1. Tool exchange Instruction format 1: T0101; This instruction is a tool rotation instruction for the FANUC system. The front T01 indicates changing tool No. 1, and the back 01 indicates using tool No. 1 for compensation. The tool number and tool compensation number can be the same or different. Instruction format 2: T04D01; This instruction is a tool rotation instruction for the SIEMENS syste
Understand the tool compensation function of CNC lathe processing in one article
1. Tool exchange function for CNC lathe
1. Tool exchange
Instruction format 1: T0101;
This instruction is a tool rotation instruction for the FANUC system. The front T01 indicates changing tool No. 1, and the back 01 indicates using tool No. 1 for compensation. The tool number and tool compensation number can be the same or different.
Instruction format 2: T04D01;
This instruction is a tool rotation instruction for the SIEMENS system. T04 indicates changing tool No. 4, and D01 indicates using tool No. 1 of tool No. 4 as tool compensation memory.
2. Tool change point
The so-called tool change point refers to the position when the tool holder automatically rotates.
For most CNC lathes, the position of the tool change point is arbitrary. The tool change point should be selected at a position that does not interfere with the workpiece or fixture during the tool exchange process. There are also some machine tools whose tool change point is a fixed point. Usually, these points are selected near the machine tool reference point, or the second reference point of the machine tool is used as the tool change point.
2. Tool compensation function
1. Definition of tool compensation function
In the process of CNC programming, in order to make programming more convenient, the tip of the CNC tool is usually imagined as a point, which is called the tool position point or tool tip point.
The function of the CNC machine tool to automatically change the position of the machine tool coordinate axis or the tool position point according to the actual size of the tool so that the actual processing contour and the programming trajectory are completely consistent is called tool compensation ("tool correction" on the system screen) function.
The tool compensation of CNC lathes is divided into:
· Tool offset (also known as tool length compensation)
· Tool tip arc radius compensation
2. The concept of tool position point
The so-called tool position point refers to the point used to represent the tool characteristics when programming and processing, and it is also the reference point for tool setting and processing. The tool position point of CNC lathe tools is shown in the figure. The tool position point of a pointed turning tool usually refers to the tool tip; the tool position point of an arc-shaped turning tool refers to the center of the arc edge; the tool position point of a forming tool also usually refers to the tool tip.
3. Tool offset compensation
1. Meaning of tool offset
Tool offset is a function used to compensate for the length difference between the assumed tool length and the reference tool length. The lathe CNC system stipulates that the X-axis and Z-axis can realize tool offset at the same time.
Tool geometry offset: tool offset caused by different tool geometry and tool installation positions.
Tool wear offset: tool offset caused by tool tip wear.
Example of tool offset compensation function:
The tool geometry offset parameter settings of the FANUC system are shown in the figure. If you want to set the tool wear offset, just press the soft key [Wear] to enter the corresponding setting screen.
2. Tool setting using tool geometry offset
(1) Definition of tool setting
The process of adjusting the tool position of each tool so that it coincides with an ideal reference point as much as possible is called tool setting.
(2) Process of tool setting
1) Manually process the end face and record the Z-axis mechanical coordinate value of the tool position.
2) Manually process the outer circle and record the X-axis mechanical coordinate value of the tool position. Stop the machine to measure the workpiece diameter and calculate the mechanical coordinate value of the spindle center.
3) Enter the X and Z values into the corresponding tool geometry offset memory.
(3) The essence of tool setting using tool geometry offset
The essence of tool setting using tool geometry offset is to use tool geometry offset to make the origin of the workpiece coordinate system coincide with the origin of the machine tool.
3. Application of tool offset
The tool offset function can be used to correct workpiece processing errors caused by incorrect tool setting or tool wear.
Example: When machining an outer cylindrical surface, if the outer diameter is 0.2 mm larger than the required size, the machining error can be corrected by reducing the X value in the tool offset memory by 0.2 and re-machining the part with the original tool and program. Similarly, if an error occurs in the Z direction, the correction method is the same.
IV. Tool tip arc radius compensation (G40, G41, G42)
1. Definition of tool tip arc radius compensation
In actual machining, due to tool wear and the need for fine machining, the tool tip of the turning tool is often ground into an arc with a smaller radius. At this time, the tool position point is the center of the tool tip arc.
In order to ensure the contour shape of the workpiece, the center movement trajectory of the tool tip arc is not allowed to coincide with the contour of the workpiece being processed during processing, but should be offset from the workpiece contour by a radius value. This offset is called tool tip arc radius compensation. The tool edge radius offset of the arc-shaped turning tool is the same.
2. Imaginary tool tip and tool tip arc radius
Ideally, we always imagine the tool position point of the pointed turning tool as a point, which is the imaginary tool tip (point A in the figure).
When aligning the tool, it is also done with an imaginary tool tip. However, in actual machining, due to process or other requirements, the tool tip of the turning tool is often not an ideal point, but an arc (such as the BC arc in the figure).
The so-called tool tip arc radius refers to the radius of the imaginary circle formed by the tool tip arc of the turning tool (r in the figure). In practice, all turning tools have tool tip arcs of varying or similar sizes, and the imaginary tool tip does not exist in actual machining.
3. Analysis of machining errors when tool tip radius compensation is not used
(1) When machining a step surface or end surface, the size and shape of the machined surface are not greatly affected, but residual errors will be generated at the center position of the end surface and the corner clearance position of the step, as shown in the figure.
(2) When machining a conical surface, it will not affect the taper of the cone, but it will have a greater impact on the size of the large and small ends of the cone surface. Usually, the size of the outer cone surface will become larger, while the size of the inner cone surface will become smaller, as shown in the figure.
(3) When machining an arc, it will affect the roundness and radius of the arc.
When machining an outward convex arc, the radius of the arc after machining will become smaller
Its value = theoretical contour radius R – tool tip arc radius r, as shown in the figure.
When machining a concave arc, the radius of the arc after machining will become larger
Its value = theoretical contour radius R + tool tip arc radius r, as shown in the figure.
4. Tool tip arc radius compensation command
1) Command format
G41 G01/G00 X_Y_F_;
Tool tip arc radius left compensation
G42 G01/G00 X_Y_F_;
Tool tip arc radius right compensation
G40 G01/G00 X_Y_;
Cancel tool tip arc radius compensation)
2) Instruction description
Determination of tool tip arc radius compensation offset direction:
a) Rear tool holder, +Y axis outward
b) Front tool holder, +Y axis inward
5. Determination of the cutting edge position of the arc turning tool
According to the different cutting edge shapes and cutting edge positions, there are 9 types of cutting edge positions for CNC turning tools as shown in the figure.
a) Rear tool rest, +Y axis outward
b) Front tool rest, +Y axis inward
c) Corresponding tool edge number of specific tool
P – imaginary tool tip point S – tool edge circle center position r – tool tip arc radius
Cutting edge numbers of some typical cutting tools
a) The cutting edge position number of the rear tool holder
b) The cutting edge position number of the front tool holder
6. Tool tip arc radius compensation process
·The tool tip arc radius compensation process is divided into three steps:
·Establishment of tool compensation
·Tool compensation execution
·Tool compensation cancellation
O0010;
N10 G99 G40 G21;
(Program initialization)
N20 T0101;
(Turn tool No. 1, execute tool compensation No. 1)
N30 M03 S1000;
(Spindle forward at 1000r/min)
N40 G00 X85.0 Z10.0;
(Fast point positioning)
N50 G42 G01 X40.0 Z5.0 F0.2;
(Tool compensation establishment)
N60 Z-18.0;
(Tool compensation execution)
N70 X80.0;
(Tool compensation execution)
N80 G40 G00 X85.0 Z10.0;
(Cut tool compensation canceled)
N90 G28 U0 W0;
(Return to reference point)
N100 M30;
(1) Tool compensation establishment
The establishment of tool compensation refers to the process in which the center of the arc edge of the turning tool changes from coinciding with the programmed trajectory to deviating from the programmed trajectory by an offset when the tool approaches the workpiece from the starting point. This process must be implemented together with the G00 or G01 function to be effective.
N50 G42 G01 X40.0 Z5.0 F0.2;
(Tool compensation establishment)
FC – Tool compensation established CDE – Tool compensation carried out EF – Tool compensation cancelled
(2) Tool compensation in progress
After the G41 or G42 program segment, the program enters the compensation mode. At this time, the center of the arc edge of the turning tool is always an offset away from the programmed trajectory until the tool compensation is canceled.
N60 Z-18.0;
(Tool compensation in progress)
N70 X80.0;
(Tool compensation in progress)
FC – Tool compensation established CDE – Tool compensation carried out EF – Tool compensation cancelled
(3) Tool compensation cancellation
The process in which the tool leaves the workpiece and the center trajectory of the arc cutting edge of the turning tool transitions to coincide with the programmed trajectory is called tool compensation cancellation, as shown in the EF segment (i.e., N80 program segment) in the figure. Tool compensation cancellation is performed using G40. It should be noted that G40 must be used in pairs with G41 or G42.
N80 G40 G00 X85.0 Z10.0;
(Tool compensation cancellation)
FC – Tool compensation established CDE – Tool compensation carried out EF – Tool compensation cancelled
7. Matters needing attention when performing tool radius compensation
(1) The program segments for establishing and canceling tool arc radius compensation mode are only valid in G00 or G01 movement command mode.
(2) G41/G42 does not have parameters, and its compensation number (representing the tool nose radius compensation value corresponding to the tool used) is specified by the T command. The tool nose arc radius compensation number corresponds to the tool offset compensation number.
(3) Use the tangent entry method or the normal entry method to establish or cancel tool compensation. When it is inconvenient to cut in or out along the workpiece contour line in the tangential or normal direction, an auxiliary program segment of a transition arc can be added according to the situation.
(4) In order to prevent the tool from overcutting during the process of establishing and canceling tool radius compensation, when establishing and canceling compensation, the starting position and end position of the program segment should preferably be on the same side as the compensation direction.
(5) In tool compensation mode, it is generally not allowed to have more than two consecutive non-movement instructions in the compensation plane, otherwise the tool will also have dangerous actions such as overcutting. Compensation plane non-movement instructions usually refer to program segments with only G, M, S, F, T instructions (such as G90, M05) and program pause segments (G04 X10.0).
(6) When selecting the tool tip arc offset direction and tool edge position, pay special attention to the difference between the front tool holder and the rear tool holder.