Content Menu
● Part. 01 Preface
● PART. 02 Process division and workpiece clamping
● PART. 03 Tool selection
● PART. 04 Cutting program compilation
● 4.1 05 Sequence end face drilling center hole
● 4.2 10-sequence head turning
● 4.3 15-sequence middle turning
● 4.4 20-sequence finished product cutting
● PART. 05 Conclusion
Using a bar tensile specimen without a threaded head as an example, this article outlines CNC machining techniques including process division, workpiece clamping, tool selection, and program compilation. Users can operate on a single machine tool equipped with a FANUC system or can achieve a "blank to finished product" delivery using a modern intelligent cutting system. Machine tool users with SINUMERIK, MITSUBISHI, and GSK systems can directly apply this analysis process.
Part. 01 Preface
Testing the mechanical properties of metal materials is an essential requirement for raw materials before they enter the factory and the warehousing process. One of the key indicators evaluated is the plasticity index, which is determined by measuring the elongation and cross-sectional shrinkage obtained from tensile tests.
When users conduct tensile tests, they need to prepare specimens that meet the standards outlined in GB/T 228.1-2021 "Metallic Materials Tensile Test Part 1: Room Temperature Test Method."
To create the tensile specimen shown in Figure 1, users can perform mechanical processing using production equipment such as CNC lathes, vertical machining centers, band saws, and vertical milling machines, following the established process flow and processing procedures.
PART. 02 Process division and workpiece clamping
The tensile specimen made from the bar without a thread on the head is typically fabricated using a CNC lathe or a circular tensile specimen processing center. This process involves four main steps:
1. Drilling a central hole on the end face (Sequence 05)
2. Turning the head (Sequence 10)
3. Turning the middle section (Sequence 15)
4. Cutting the finished product (Sequence 20)
Additionally, there are two auxiliary operations: feeding the bar and removing the finished product.
Some users have operators manually load and unload the workpieces on a single machine before executing the CNC program to complete the processing in one go. Others may employ industrial robots for the loading and unloading of workpieces, enabling the CNC lathe to automatically load the bar and adjust the length in the Z direction under the M auxiliary function code, based on different processing requirements.
The bar used to create the tensile specimen has a diameter of 40 mm and a length of 600 mm. After drilling the central hole on one end, the spindle side is clamped using a hydraulic self-centering chuck, while the tailstock side is secured by a rotary center. The CNC lathe is equipped with CNC systems such as GSK 25Ti, FANUC 0iTF, or SINUMERIK 828D. The machine bed is designed as an inclined bed made from resin sand casting. It features a 12-station rear-mounted servo turret, with maximum sizes for square and round shanks being 25 mm x 25 mm and 40 mm in diameter, respectively. The spindle through hole diameter is 66 mm, and the pull rod through hole diameter is 52 mm.
1—Lathe spindle 2—Hydraulic self-centering chuck 3—Test piece 4—Cut-off insert 5—T-Max® Q-Cut conventional toolholder 6—CoroTurn® 107 turning insert 7—CoroTurn® 107 turning conventional toolholder 8—T-Max® P turning insert 9—T-Max® P turning square toolholder 10—Tailstock rotary center MT5
PART. 03 Tool selection
The bar is turned from a diameter of 40mm to 35mm and then to 22mm, as illustrated in Figure 1. The corresponding single-side cutting amounts are 2.5mm and 9mm. To meet the requirements for the center hole on the end face of the tensile specimen, as well as to turn the outer cylindrical surfaces at both ends, the middle outer circle, and the arc, various brands of cutting tools can be selected (see Table 1). For the numbering instructions for Sandvik Coromant's indexable external cylindrical turning tool bars and inserts, please refer to the sample manual available on Sandvik Coromant's official website.
To effectively reduce cutting temperature and extend tool life, a 5% cutting fluid is applied for cooling during the turning of the workpiece. For creating tool graphics, you can use the online tool assembler available on the Sandvik Coromant official website (refer to Figure 3). After selecting the tool bar and blade based on the material of the bar, you can assemble them online to create a two-dimensional graphic. Once completed, download the graphic in DXF format for further drawing and trajectory programming.
PART. 04 Cutting program compilation
The plane representing the right end face of the sample blank, as shown in Figure 2, is aligned with the Xp axis, which points towards the rear turret in the positive direction. Meanwhile, the axis along which the center line of the blank is situated is the Zp axis, oriented away from the spindle as the positive direction.
A workpiece coordinate system, also known as the programming coordinate system, has been established with point W designated as the origin for this system in the corresponding process. It is important to note that the workpiece coordinate systems for sequences 10, 15, and 20 are identical.
According to the programming instruction format permitted by the selected CNC services machining, a processing program has been developed that includes the processes, process parameters (such as spindle speed, feed speed, etc.), and auxiliary actions, such as the cutting fluid switch, for the four processes. Comments are indicated by a semicolon following the relevant instructions.
4.1 05 Sequence end face drilling center hole
The center hole drilling process for the end face of the 05 sequence is illustrated in Figure 4. When setting up the center drilling tool, only the Z-axis needs to be controlled. The linear speed for drilling the center hole in the steel part on the lathe is typically maintained at 40 m/min. Using the formula \( v_c = \frac{\pi D n}{1000} \), the spindle speed \( n \) can be calculated to be approximately 965 r/min. The procedure for drilling the center hole on the end face of the 05 component is outlined as follows.
O0005 (ZHONGXINKONG); Program name for drilling center hole on end face of sequence 05 (FANUC 0i TF system) N0010 T0101; Call center drill No. 01 and tool compensation of No. 01 N0020 S965 M03; The spindle rotates forward at a speed of 965r/min in the feed per revolution mode, and the CNC parameter #3402.4/FPM of the FANUC system is set to "feed per revolution mode by default when the system is powered on" N0030 G00 X0. Z20. Center drill No. 01 moves rapidly along the X and Z axes to the positioning point N0040 G01 Z0. F1. M08: Move straightly to the end face at a speed of 1mm/r and open the cutting fluid N0050 Z-14.7042 F0.07; Drill type A center hole at a speed of 0.07mm/r N0060 Z0. F1. M09: retract the tool, turn off the cutting fluid N0070 G00 Z20. M05; retract the tool quickly, stop the spindle N0080 G28 U0 W0; quickly retract along the X and Z axes to the first reference point in preparation for subsequent safe tool change (program end symbol omitted)
4.2 10-sequence head turning
The recommended linear speed for the CNMG120408-PM4415 blade during stainless steel turning parts is 345 m/min, with a feed rate of 0.3 mm/rev. Using the formula \( v_c = \frac{\pi D n}{1000} \), we can calculate the spindle speed \( n \) to be approximately 2745 rpm.
The cutting path for the T03 turning tool is as follows: A → B → C → H → D → A → E → F → G → D → A, as illustrated in Figure 5.
The machining program for the 10-sequence head turning is provided below, excluding the call code for robot loading and unloading as well as the control for the machine door switch.
Program Instructions for Turning Operation (TOUBU)
Program Overview:
- This program is designed to control the 10th sequence head on the FANUC 0i TF system.
Initial Setup:
- Call Tool: Activate center drill No. 03 and tool compensation No. 03.
- Spindle Speed: Set the spindle to rotate forward at a speed of 2745 RPM in feed per revolution mode.
Movement Commands:
- Rapid Movement:
- Move the turning tool No. 02 rapidly along the X and Z axes to point A (X70, Z5).
- Linear Interpolation:
- Interpolate linearly to point B (X36, Z0) with a feed rate of 1 mm/rev and activate cutting fluid.
- Move to point C (Z-274.718) using a feed rate of 0.3 mm/rev.
- Interpolate to point D (X40).
- Retract Tool Rapidly:
- Rapidly retract the tool to point H (X70) and turn off the cutting fluid.
- Return rapidly to the starting point (Z5).
Additional Interpolation:
- To Point E:
- Interpolate linearly to point E (X32, Z0) at a speed of 1 mm/rev and activate cutting fluid.
- To Point F:
- Interpolate linearly to point F (X35, Z-1.5) at a speed of 0.2 mm/rev.
- To Point G:
- Continue linear interpolation to point G (Z-274.718).
Final Movement:
- Rapidly retract along the X axis to point D and turn off the cutting fluid.
- Rapidly retract along the Z axis to point A and turn off the spindle.
- Finally, rapidly return along the X and Z axes to the first reference point in preparation for a safe tool change.
(Note: Program end symbol has been omitted.)
4.3 15-sequence middle turning
The recommended linear speed for the VBMT160404-UM1515 blade when turning steel is vc = 205 m/min, with a feed rate of 0.2 mm/rev. Using the formula vc = πDn/1000, the calculated spindle speed n is approximately 1865 r/min.
Due to the arcs on both sides of the middle turning, the arc ΔZ on the left side is increasing in the positive direction, while the arc ΔZ on the right side is decreasing in the negative direction. This configuration does not meet the requirements for the FANUC system's G73 contour rough turning cycle. To avoid overcutting or undercutting, tool-by-tool trajectory programming is employed for the rough machining and finishing of the 10-sequence semi-finished product.
Rough machining consists of five cuts, with a cutting depth of 1.2 mm in the X direction and 0.875 mm in the Z direction for each cut. Finishing is conducted in a single cut, with cutting depths of 0.5 mm in both the X and Z directions. The cutting trajectory for each cut follows the sequence: A → In → Jn → Kn → Ln → Mn → In, where n ranges from 1 to 6, as illustrated in Figure 6.
The machining program for the turning process in sequence 15 is outlined below (excluding the call codes for robot loading and unloading, as well as the machine door switch control).
Turning Program Overview
Program Start:
Document Number: O0015 (ZHONG)
Turn on the spindle with command: M03.
Initial Adjustments:
Adjust turning tool No. 05 with tool compensation S1865.
Movement Instructions:
- Initiate forward rotation: G00 X70 Z5 in spindle feed mode.
- Rapidly move the turning tool along the X and Z axes to Point A: G00 X66.12 Z-137.3592.
- Rapidly move to Point I1 from the first tool: G00 X37.0 Z-68.5387, activating cutting fluid: M08.
- Rapidly move to Point J1, then open cutting fluid: G03 X32.6 Z-76.3592 R15 F0.15.
Counterclockwise Interpolation:
- The rear turning tool will interpolate an arc of R15mm counterclockwise to Point K1: G01 Z-198.3592 F0.2.
- Perform linear interpolation to Point L1: G03 X37.0 Z-206.1797 R15 F0.15.
- Counterclockwise interpolation arc to Point M1: G00 X67.205 Z-137.3592.
Fast Retreat and Additional Movements:
- Fast retreat to Point I2 from the second cut: G00 X37.0 Z-65.9742.
- Fast move to Point J2: G03 X30.2 Z-75.4842 R15 F0.15.
- Counterclockwise interpolation arc to Point K2: G01 Z-199.2342 F0.2.
- Linear interpolation to Point L2: G03 X37.0 Z-208.7442 R15 F0.15.
- Counterclockwise interpolation arc to Point M2: G00 X68.125 Z-137.3592.
Continuing Cuts:
- Fast retreat to Point I3 from the third cut: G00 X37.0 Z-63.8.
- Fast move to Point J3: G03 X27.8 Z-74.6092 R15 F0.15.
- Counterclockwise interpolation arc to Point K3: G01 Z-200.1092 F0.2.
- Linear interpolation to Point L3: G03 X37.0 Z-210.9185 R15 F0.15.
- Counterclockwise interpolation arc to Point M3: G00 X68.9346 Z-137.3592.
Final Cuts:
- Fast retreat to Point I4 from the fourth tool: G00 X37.0 Z-61.8868.
- Fast move to Point J4: G03 X25.4 Z-73.7342 R15 F0.15.
- Counterclockwise interpolation arc to Point K4: G01 Z-200.9842 F0.2.
- Linear interpolation to Point L4: G03 X37.0 Z-212.8316 R15 F0.15.
- Counterclockwise interpolation arc to Point M4: G00 X69.6608 Z-137.3592.
Additional Cuts:
- Fast retreat to Point I5 from the fifth cut: G00 X37.0 Z-60.17.
- Fast move to Point J5: G03 X23.0 Z-72.8592 R15 F0.15.
- Counterclockwise interpolation arc to Point K5: G01 Z-201.8592 F0.2.
- Linear interpolation to Point L5: G03 X37.0 Z-214.5478 R15 F0.15.
- Counterclockwise interpolation arc to Point M5: G00 X70.0 Z-137.3592.
Final Movements and Shutdown:
- Fast retreat to Point I6 from the sixth cut: G00 X37.0 Z-59.3688.
- Fast move to Point J6: G03 X22.0 Z-72.3592 R15 F0.15.
- Interpolate arc of R15mm counterclockwise to Point K6: G01 Z-202.3592 F0.2.
- Interpolate linearly to Point L6: G03 X37.0 Z-215.3496 R15 F0.15.
- Interpolate arc of R15mm counterclockwise to Point M6: G00 X70.0 Z-137.3592, turn off cutting fluid M09.
End of Program:
- Retreat to Point I6, turn off cutting fluid and return to Z5: M05.
- Return to the starting point A along the Z axis: G28 U0 W0.
- Quickly retreat to the first reference point along the X and Z axes: M30.
- End of Program: Final command N0140.
4.4 20-sequence finished product cutting
The N151.2-400-5E1125 T-Max® Q-Cut blade is designed for cutting steel with a recommended linear speed of vc = 180 m/min and a feed rate of 0.12 mm/r. The spindle speed, approximately n = 1433 r/min, is calculated using the formula vc = πDn/1000. Since the maximum depth of cut without barriers for the LF151.23-2020-40M1 T-Max® Q-Cut conventional tool holder is 25 mm, and the cutting radius of the tensile specimen is 20 mm, direct cutting can be performed without the need for macro programming during the longitudinal Z-axis reciprocating turning of the tool.
The cutting tool trajectory follows the path A → N → P → Q → P → N → A, as illustrated in Figure 7. The processing program for the 20-step finished product-cutting process is outlined below (excluding the robot loading and unloading commands, machine door operations, and automatic feeding control).
O0020 (CUT); Program name for cutting off 20-sequence finished products (FANUC 0iTF system)
N0010 T0707; Call cutting tool No. 07 and tool compensation amount No. 07
N0020 S21433 M03: Spindle rotates forward at a speed of 1433r/min in the feed per revolution mode N0030 G00 X70. Z5.; The turning tool moves rapidly along the X and Z axes to point A
N0040 Z-278.7184; Move rapidly along the Z axis to point N
N0050 G01 X42. F1.0 M08; Linear interpolation at a speed of 1mm/r to point P, open cutting fluid
N0060 X-8.0. F0.12; Linear interpolation at a speed of 0.12mm/r to point Q
N0070 X42. M09: Retract the tool along the X axis to point P, turn off the cutting fluid
N0080 G00 X70. Rapidly withdraw the tool along the X-axis to point N
N0090 Z5.M05: Rapidly withdraw the tool along the Z axis to point A and turn off the spindle
N0010 G28 U0 W0; Rapidly withdraw along the X and Z axes to the first reference point in preparation for subsequent safe tool change (program end symbol omitted)
PART. 05 Conclusion
Efficient and cost-effective modern CNC machining technology relies heavily on skilled technicians. When interpreting product drawings, technicians must consider a range of factors, including CNC machining process layout, equipment selection, division of process steps, workpiece clamping, tool selection, program development, and the supply of auxiliary materials. They must not only account for the processing of other products but also strive to quickly complete the processing of target products using existing resources. The goal is to achieve the shortest process flow, ensure smooth logistics, optimize cutting parameters, maximize tool life, maintain concise programming, and avoid any overcutting or undercutting.
If you want to know more or inquiry, please feel free to contact info@anebon.com
Anebon team's specialty and service consciousness have helped the company gain an excellent reputation among customers worldwide for offering affordable prototype machined parts, CNC cutting parts, and custom machined aluminum parts. The primary objective of Anebon is to help customers achieve their goals.
Post time: Feb-08-2025