Design and implementation of an innovative canned cycle for variable pitch thread cutting on CNC milling machines

Heidenhain control system [9] provides a range of parameters denoted as Q, allowing users to program both internal and external threading operations (Fig. 1). By using parameter Q355 with a value of either 0 or 1, users can specify the type of cutter they wish to utilize, whether it is a single form or multi-form thread milling cutter (Fig. 2).

For HAAS control [10], thread milling involves employing a conventional G02 or G03 command to achieve circular motion in the X–Y plane, followed by a Z-axis command to establish the desired thread pitch. This process completes one revolution of the thread, while the remaining revolutions are generated by the teeth of the multiple-form cutter (Fig. 3).

A typical code line for this operation might appear as follows:

This line creates a 1.5 mm pitch thread with a 40 mm radius.

Similarly, for FANUC control [11], thread cutting using an appropriate fitting tool is facilitated through the dedicated G33 code, as shown in Fig. 4.

The corresponding G-code line takes the following format:

Parameters Z and F represent the hole depth and pitch, respectively, creating a 1.5 mm thread in a 50 mm depth hole.

Despite the convenience of these programming techniques, they share a common limitation—the absence of provisions for threads with variable pitch. Existing programming approaches rely on predefined cycles with fixed pitch values, while cases requiring variable pitch threads often require CAM system interpretation, involving laborious design and calculation processes. In response to this limitation, the present work introduces an innovative canned cycle, allowing straightforward and user-friendly programming of threads with variable pitch. This new cycle is developed using a parametric programming language, present in all modern CNC controls under various names.

The development of an advanced, accurate, and user-friendly canned cycle for milling threads with variable pitch required careful consideration of several key factors. The algorithm was designed to meet specific performance objectives, ensure ease of use during programming, and offer flexibility for comprehensive coverage of threading cases. Performance: The primary objective of the canned cycle was to enable efficient thread cutting with variable pitch on CNC milling machines. To achieve this, the algorithm needed to support both internal and external threads, accommodate left- or right-hand threading, and allow for the selection of variable pitch by defining either the starting or ending pitch alongside the number of turns. The tool step motion needed to be adjustable, allowing machinists to set the desired precision. User-friendliness: The canned cycle aimed to accommodate the programming process and minimize the need for complex CAM system interpretations. A dedicated control panel was designed as an interface between the user and the canned cycle. The control panel incorporated all the necessary parameters, simplifying data input and reducing the risk of errors during programming. Flexibility: Recognizing the diversity of threading cases in practical applications, the algorithm was designed with the capability to adapt to various cases. The control panel allowed users to input specific values for parameters such as helix radius, starting or ending pitch, number of turns, left-hand or right-hand thread, feedrate, and spindle speed, thereby providing comprehensive flexibility in programming.

In order to cut threads with variable pitch on a 3-axis CNC milling machine, the capability of generating 3D motion along a helix with a variable pitch is essential. This necessitates obtaining the solution of parametric equations x(t), y(t), z(t) of the helix within an interpolation algorithm framework. The parametric equations of a helix [18] with constant radius and pitch are given by Eq. 1 (Fig. 5).where,

't' serves a dual purpose in defining the helix's geometry. First, it determines the angular step position for X and Y coordinates.

As 't' varies from 0 to 1, it effectively traces the path around the helix in an angular sense. Second, 't' simultaneously controls the vertical departure from the starting point, which is expressed by the Z coordinate. Therefore, it plays a pivotal role in defining both the planar angular position and the vertical position along the helix. A smaller value of 't' yields shorter linear segments, which, in turn, enhances the precision of the traced helix.

For a helix with a constant radius and variable pitch, the equations (Eq. 1) can be expressed as follows:

To adapt these equations based on the CNC milling machine's tool-part setup, allowing the tool to move from the top to the bottom of the part with the upper surface considered as Z = 0, the following adjustments are made for the case of an increasing pitch:

Accordingly, for the case of a decreasing pitch the equations take the form:

Furthermore, by exchanging the sine and cosine functions in the first two equations, it is possible to achieve a left-hand or right-hand thread type. The verification of the two cases, a left-hand thread with increasing pitch (R = 50, n = 5, ending pitch p = 25) and a right-hand thread with decreasing pitch (R = 60, n = 8, starting pitch p = 30), is depicted graphically in Fig. 6 through two distinct numerical examples.

The G-code algorithm is formulated within the environment of Heidenhain control. Additionally, it can be easily translated for use with any other CNC control that supports parametric programming. Inputting the required thread data and cutting conditions into the G-code algorithm is achieved through the utilization of Q parameters (see Sect. 3). The algorithm comprises a main program and four subprograms. The main program initializes thread data by setting parameters Q1-Q8 (Table 2), drives the cutter to the starting point, and controls the execution flow towards one of the four subprograms. Each of the four subprograms is specifically designed to handle a distinct case of threads, namely: right-hand decreasing pitch, right-hand increasing pitch, left-hand decreasing pitch, and left-hand increasing pitch. The flowcharts in Figs. 7 and 8 form the basis for developing the G-code parametric algorithm, as they illustrate the logical structure of the main program and the four subprograms. While the flowchart of the subprogram (Fig. 8) represents the case of a right-hand decreasing pitch thread, similar flowcharts can be easily generated using the appropriate equations for the other three cases.

The zero-reference point is positioned at the top center of the helix. Driving the tool to the starting position involves two steps. The first step is common for both external and internal threads, where the tool is directed to the zero-reference point. In the second step, for internal threads, the tool is driven linearly at X = R₁-R₂, Y = 0, and Z = 0, while for external threads, it moves to X = R₁ + R₂, Y = 0, and Z = 0, (with R₁ representing the helix radius and R₂ the tool radius). The user initializes this value through the Q4 parameter.

Based on the flowcharts presented above, the logic depicted in them facilitated the development of the G-code parametric algorithm. The corresponding code, along with accompanying comments, is provided in Tables 3 and 4. Table 3 presents the main program, while Table 4 details subprogram 1. The remaining three subprograms were developed by utilizing the appropriate equations.

Generally, canned cycles are standardized and codified using a G-code in conjunction with a series of parameters. It is important to note that CNC controllers intentionally reserve certain G-codes for future use, allowing for customized implementations and increased flexibility. Specifically, in the context of Heidenhain control, the unassigned G100 code has been selected for the proposed implementation. Complementary data required for the canned cycle can be expressed through a statement following the format:

Within this format, the G100 code is suggested to represent the canned cycle for milling threads with variable pitch. The parameters P00 to P08 are utilized to specify the following:

In all cases, the appropriate tool for threading is a single-form cutter (Fig. 2a).

To ensure a user-friendly environment and prevent the entry of unacceptable values, a control panel (Fig. 9) has been designed using a high-level programming language. This panel incorporates all the necessary parameters that need to be updated for any new desired case of variable pitch thread cutting. By appropriately completing the designated fields and pressing the “G” button, the corresponding values are transferred to the respective parameters P01…P08 in the G100 statement. The completed statement is then displayed on the screen, ready to be transferred to the CNC controller. In addition to its user-friendly interface, the panel includes a built-in validation mechanism that checks the inserted values for acceptability. Only when all the values are valid does the G100 statement is displayed ready for further processing.