JPH0512097B2 - - Google Patents

Description

DETAILED DESCRIPTION OF THE INVENTION <Industrial Application Field> The present invention relates to a method for creating an NC program for a four-axis lathe, and particularly to a method for creating NC data for a four-axis lathe having a balance cut process.

<Prior art> In machining control of a 4-axis lathe having two turrets, a first and a second, NC programs are provided for the first and second turrets, each having a waiting command corresponding to each turret. While synchronizing with commands, the first and second NC programs independently control the movement of the corresponding tool rests to machine the workpiece. For this reason, with a 4-axis lathe, for example, a tool attached to one turret can machine the external shape of a workpiece, and a tool attached to the other turret can simultaneously perform internal machining, reducing machining time. be able to.

Furthermore, a 4-axis lathe allows cutting called balance cutting, which allows highly accurate turning of long and narrow workpieces. In this cutting method, when machining a long and narrow workpiece WK as shown in Fig. 12, the first and second tools TL1 and TL2 are applied from both sides of the workpiece,
Each tool is moved synchronously to perform machining at the same time, which prevents deflection of the workpiece, enables highly accurate machining, and enables heavy cutting. In addition, CHK in FIG. 12 is a check.

NC programs for such four-axis lathes are automatically created interactively by the automatic programming function of the NC device or by a separate automatic programming device.

However, conventional automatic programming devices do not have a function to automatically create an NC program for balance cutting, making programming work when a balance cutting process is included.

For this reason, a 4-axis lathe that can automatically create an NC program including NC data for balance cutting has been developed.
A method for creating NC programs has been proposed.

However, in the proposed NC program creation method, the first,
If the shape of the tool in the second tool post is different, in other words, if the cutting edge angle or edge angle of the tool in the first and second tool posts is different, it will be considered unsuitable as a balance cut tool and the process will proceed to the next data input step. I'm trying not to proceed.

Fig. 13 is an explanatory diagram of the tool shape. Figure A is an explanatory diagram of the tool shape of an outer diameter machining tool that is moved in the -Z direction for cutting, and Figure B is a tool shape explanatory diagram of an outer diameter machining tool that is moved in the +Z direction for cutting. It is an explanatory diagram of the tool, TL1, TL2
is the tool, MB is the main cutting edge, SB is the minor cutting edge, and WK is the workpiece.

The angle from the main cutting edge MB to the vertical line VL (counterclockwise is positive) is the cutting edge angle AC, and from the main cutting edge MB to the minor cutting edge SB
The angle up to this point (clockwise is positive) is the cutting edge angle AN.
However, RN is the radius of the cutting edge.

Now, the reason why it is said that a tool having a different cutting edge angle or edge angle in the first and second tool rests for balance cutting is inappropriate as a balance cutting tool is as follows.

Now, if the cutting edge of the tool TL11 shown in FIG. 14A is moved along the solid line (desired shape) SL for processing, the tool will interfere with the workpiece WK at the inclined portion. In such a case, the automatic programming device creates NC data so that the tool does not interfere with the workpiece at the inclined portion, for example, so that the cutting edge moves along the dotted line in FIG. 14B.

On the other hand, in the case of tool TL12 shown in FIG. Figure 14D
NC to move along the dotted line (solid line) shown in
Create data.

Therefore, if the shapes of the tools in the first and second tool rests for balance cutting are different, and one tool interferes with the workpiece when the cutting edge is moved along the desired shape, the cutting edge path of the tools will be different from each other. It will become different and you will not be able to make a balanced cut. For this reason, it is considered inappropriate if the cutting edge angles or edge angles of the tools in the first and second tool rests for balance cutting are different.

Note that if NC data for balance cutting of both tools is created using one tool as a reference, the cutting edge paths will match, but the other tool may interfere with the workpiece.

<Problems to be Solved by the Invention> If the cutting edge angle or edge angle is different and it is unsuitable as a balance cutting tool, the degree of freedom in tool selection will be reduced, making it difficult to determine the tool. Furthermore, there are frequent cases where the appropriate tool is not present on the tool rest, resulting in a situation where balance cutting cannot be performed.

From the above, an object of the present invention is to provide a method for creating an NC program for a 4-axis lathe that allows balanced cutting even when the cutting edge angle and tip angle are different.

<Means to solve the problem> FIG. 1 is a schematic explanatory diagram of the present invention.

TL11~TL12 are tools for outside diameter machining, BT1
1 to BT12 are bits (cutting edges), MB11 to MB1
2 is a main cutting edge of each tool, and SB11 to SB12 are auxiliary cutting edges. Note that each tool is moved in the -Z direction for processing, and therefore the cutting direction is the -Z direction.

<Function> When the shapes of the cutting edges of the tools TL11 and TL12 in the first and second tool rests used for balance cutting are different, the main cutting edge MB11 of the first tool TL11 and the main cutting edge MB12 of the second tool TL12. The main cutting edge MB12 of the tool that is largely inclined toward the cutting direction (-Z direction) is regarded as the main cutting edge of a virtual balance cut tool. Also, the minor cutting edge of the first tool TL11
Among the SB11 and the auxiliary cutting edge SB12 of the second tool TL12, the auxiliary cutting edge SB11 of the tool that is largely inclined toward the side opposite to the cutting direction (+Z direction) is regarded as the auxiliary cutting edge of a virtual balance cut tool. Then, we searched for a cutting edge path that would not interfere with the workpiece even if the virtual balance cut tool was used to perform a balance cut.
Create NC data.

As a result, the path of the cutting edge of each tool coincides, and balanced cutting can be performed without interfering with the workpiece.

<Embodiment> FIG. 2 is a block diagram of an automatic programming device that implements the present invention.

11 is a processor, 12 is a ROM, 13 is a
RAM, 14 is a working memory, 15 is a display device (CRT), 16 is a keyboard for inputting data, and 17 is an NC data output device for outputting the created NC program to an external recording medium.

The CRT is provided with an interaction screen display area 15a and a plurality of soft key areas 15b, and a key (not shown) is provided corresponding to each soft key area, and when the key is pressed, a message is displayed in the corresponding soft key area. You can enter the data that is available.

Further, the RAM 13 is provided with a parameter storage area 13a for storing various parameters.

FIG. 3 is a flowchart of the automatic programming process for a four-axis lathe according to the present invention. This automatic programming process consists of the following 15 steps. That is, (1) the first step is to select the execution of "automatic programming", (2) the second step is to select the data to be input (the next step to be executed), and (3) the third step is to select the material of the material. (4) Fourth step to set the surface roughness, (5) Fifth step to select the drawing format, (6) Sixth step to input the material shape and its dimensions, (7) Part shape and its dimensions. 7th step to input, (8) 8th step to input machine origin and turret position, (9) 9th step to select machining process, (10) 10th step to select tool and input tool data, (11) 11th step to determine machining conditions, (12) 12th step to input the cutting direction, (13) 13th step to input the cutting range, (14) 1st step to input the presence or absence of an area to be cut with the same tool.
14 Steps (15) Consisting of the 15th step of tool path calculation (NC data creation), the automatic programming device shown in FIG. 2 sequentially displays predetermined question images (dialogue screens) on the display screen of the display device 15. The operator inputs the necessary data from the keyboard 16 according to the question, and finally the first and second NC programs for the 4-axis lathe are created using all the input data. .

FIG. 4 and FIG. 5 are flowcharts of the process of the method of the present invention, and the data input method and NC data creation method in the case including the balance cut step will be explained below.

Note that the processes in which balance cutting is possible are limited to outer diameter turning (outer diameter rough machining, outer diameter semi-finishing, outer diameter finishing), and balance cutting is performed in advance in the parameter storage area 13a of the RAM 13 (Fig. 2). The name of the process is memorized. In reality, the 1st, 2nd, and 3rd bits of the predetermined parameters are set to “1” or “0” to determine whether balance cutting is performed for outer diameter rough machining, outer diameter semi-finishing machining, and outer diameter finishing machining, respectively. It is specified. For example, if the first bit is "1", the automatic programming device recognizes that the outer diameter roughing is a balance cut.
If the second bit is "1", it is recognized that the outer diameter center finishing process is performed, and similarly, if the third bit is "1", the outer diameter finishing process is recognized as a balance cut.

(a) Now, in the 9th step in FIG. ).

(b) If it is not outside diameter turning, draw on the CRT an dialog screen (see Figure 6) for inputting data specifying the tool (one type) used in the machining process input in the ninth step.

(c) On the other hand, if the input process is one of outer diameter rough machining, outer diameter semi-finish machining, and outer diameter finish machining, the processor 11 stores parameter storage area 1.
Referring to the parameters stored in 3a, it is checked whether the process is a balance cut process.

(d) If it is not a balance cut process, the process jumps to step (b), and if it is a balance cut process, it is an interactive screen that asks about the two types of tools in the first and second tool rests used for the balance cut (see Figure 2). is displayed on the display screen CRT.

(e) The operator shall: (e-1) If it is not a balance cut process, the (i) tool management number, (ii) tool number, (iii) tool position correction number, (iv) turret number, etc. of one type of tool. (e-2) In the case of a balance cut process, the (i) tool management number, (ii) tool number, (iii) tool position correction number of the first and second tools used for the balance cut, Input (iv) turret number, (v) spindle rotation direction, etc.

However, if the tool number, tool position compensation number, turret, tool shape, etc. are stored in the RAM 13 as a tooling file for the tool management number, other data will be automatically transferred to the CRT just by inputting the tool management number. Is displayed.

In addition, on the dialog screen shown in FIG. 2, if only one tool data is input and other tool data are left undefined and the process proceeds to the next step, the balance cut process will not be performed. Furthermore, the turret numbers of the first and second tools cannot be the same, and the rotational directions of the spindles for the first and second tools must be the same. If the turret numbers are the same or the spindle rotation directions are different, it is not possible to proceed to the next step. Furthermore, in the case of balance cutting, if the specified tool is not present in only one turret, the processor 11 does not perform the balance cutting process.

(f) If the predetermined tool data is input in Figure 2 or Figure 6, the dialog screen for inputting the tool shape shown in Figure 7 will be drawn, so input the tool shape data one by one according to the questions. . Note that if the tooling file is stored in the RAM 13, a screen containing tool shape data is automatically displayed. Furthermore, in the case of balance cutting, if the first and second tools have different cutting edge radii (RN), it is not possible to proceed to the next step. This is because different cutting edge radii result in different tool paths.

(g) After all necessary data is entered interactively and in the second step (see Figure 3), creation of the first and second NC programs to control the first and second turrets is requested. Processor 11 is
Draw the process editing screen on the CRT.

For example, if both outer diameter rough machining and outer diameter finish machining are registered as a balance cut process, the "process definition" after the 9th step (see Figure 3)
If the process is defined as shown in FIG. 8, a process editing screen in which processes are divided by turret is drawn as shown in FIG. 9.

In FIG. 9, G96 is a G function command that commands constant circumferential speed control, Alphabet V is a word address word that commands cutting speed, and M03 is an M function command that commands normal rotation of the main shaft. Further, the number i (=1, 2) in parentheses at the right end means that a command (G96 S...) for specifying the spindle rotation speed is output to the i-th NC program.

(h) While the process editing screen is being drawn, the operator can modify the cutting speed V and the process order of each tool post. Therefore, if correction is necessary, perform a predetermined correction operation, and if correction is unnecessary, proceed to the next step.

If you want to modify the cutting speed V of a given process, move the cursor CSR forward /
Simply press the backward soft key to position the machine at a predetermined process, and then enter the cutting speed from the keyboard.

In addition, to modify the 5th process "thread cutting" of tool post 1 to be performed simultaneously with the "thread cutting" of tool post 2, position the cursor CSR on the 5th process, and then press the soft key "Knife 1". (or you may place the cursor on the fourth step and press the soft key "Knife 2 Down").

(i) If no correction is necessary or if the correction operation is completed and creation of an NC program is requested, the processor 11 executes the first
Create a second program.

In addition, if the machining process includes a balance cut process, a virtual balance cut tool is determined according to the flow shown in Fig. 5, and the NC data of the balance cut process is determined to be processed using the virtual balance cut tool. Create. However, the process in FIG. 5 may be performed after the tool shape data input step (step (f)) in FIG.

Hereinafter, the process for determining the virtual balance cut tool will be explained with reference to FIGS. 5 and 10.

(1) Cutting edge angle of first tool TL11 and second tool TL12
Using ACi (i=1, 2) and cutting edge angle ANi, the main cutting edge vectors V _Mi and V _Si (i=1, 2) of each tool
(see Fig. 10A and B).

(2) Next, calculate the cross product of the main cutting edge vector V _Mi and the minor cutting edge vector V _Si (i=1, 2) of each tool using the following formula V _Mi ×V _Si , and use the sign of the calculation result to determine the main cutting edge vector Direction W _i from cutting edge vector V _Mi to sub-cutting edge vector V _Si (i=1, 2)
seek. Note that if it is clockwise, it is negative, and if it is counterclockwise, it is positive.

(3) Once the directions W ₁ and W ₂ are determined, it is determined whether these directions are equal or inside.

(4) If W ₁ ≠ W ₂ , perform the following process (4-1) or (4-2).

(4-1)...The cutting directions of the first and second tools TL11 and TL12 are reversed, making them unsuitable as balance cut tools, resulting in an error and outputting an alarm such as an error message.

(4-2) ...Temporarily reverse the minor cutting edge and the main cutting edge of the tool that is about to cut with the minor cutting edge,
By exchanging V _Si and V _Mi (i = 1 or 2), W ₁ = W ₂ , and the processes from step (5) onwards are executed to perform a balanced cut.

It is assumed that which process (4-1) or (4-2) is executed depends on the parameter specification.

(5) On the other hand, if W ₁ = W ₂ , calculate V _{PM and V PS using the following formula V M1 ×V M2 →V PM V S1 × V S2 →} V _PS , and calculate the main cutting edge vector by the sign of V _PM . Find the direction from V _M1 to the main cutting edge vector V _M2 , and use the sign of V _PS to determine the direction of the minor cutting edge vector.
Find the direction from V _S1 to the minor cutting edge vector V _S2 .
Note that if the sign is negative, the direction is clockwise, and if the sign is positive, the direction is counterclockwise.

(6) Next, check whether V _PM is zero (main cutting edge vector V _M1 ,
Check whether V _M2 matches) or whether the sign of V _PM (direction from main cutting edge vector V _M1 to main cutting vector V _M2 ) matches W ₁ .

(7) If V _PM = 0 or the sign of V _PM = W ₁ , the main cutting edge vector V _M1 is set as the main cutting edge vector of the virtual balance cut tool.

(8) On the other hand, V _PM is not 0 and its sign is
If it does not match W ₁ , the main cutting edge vector V _M2
Let be the main cutting edge vector of the virtual balance cut tool.

In addition, in the example shown in Fig. 10, the main cutting edge vector
V _M2 is considered as the main cutting edge vector of the virtual balance cut tool. That is, the main cutting edge of the first and second tools that is more inclined toward the cutting direction is regarded as the main cutting edge of the virtual balance cut tool.

(9) Next, check whether V _PS is zero (minor cutting edge vector V _S1 ,
Check whether V _S2 matches) or whether the sign of V _PS (direction from the minor cutting edge vector V _S1 to the minor cutting edge vector V _S2 ) does not match W ₁ .

(10) If V _PS =0 or the sign of V _PS ≠W ₁ , the minor cutting edge vector V _S1 is set as the main cutting edge vector of the virtual balance cut tool.

(11) On the other hand, V _PS is not 0 and its sign is W ₁
If it matches, the minor cutting edge vector V _S2 is set as the minor cutting edge vector of the virtual balance cut tool.

In addition, in the example shown in Fig. 10, the minor cutting edge vector
V _S1 is considered as the minor cutting edge vector of the virtual balance cut tool. That is, of the secondary cutting edges of the first and second tools, the secondary cutting edge that is more inclined in the direction opposite to the cutting direction is regarded as the secondary cutting edge of the virtual balance cut tool.

As described above, after determining the tool shape of the virtual balance cut tool, a tool path where the virtual balance cut tool does not interfere with the workpiece is determined, and NC data for the balance cut process is created.

Figure 11 shows the first and second NC programs NP1 and NP2 when machining is performed in the process order shown in Figure 9.
FIG.

In the first NC program NP1, 1a is the NC data part that specifies the tool path for outer diameter rough machining, which is the first machining process of tool post 1, and 1b is the tool for outer diameter finishing machining, which is the second machining process of tool post 1. NC data part that specifies the path, 1c is the NC data part that specifies the tool path for grooving, which is the third machining process of tool post 1, and 1d is the tool path for thread cutting, which is the fifth machining process of tool post 1. This is the NC data part that specifies the

In addition, in the second NC program NP2, 2a is the NC data part that specifies the tool path for balance cut (outside diameter rough machining) of tool post 2, and 2b is the NC data part that specifies the tool path for balance cut (outside diameter finishing machining) of tool post 2. The NC data section 2c is an NC data section that specifies the tool path for thread cutting, which is the fourth processing step of the tool post 2.

The tool path for each process is automatically determined using the finished shape, cutting conditions, etc., and the NC data part 1
a to 1d and 2a to 2c are created.

In addition, in the first and second NC programs NP1 and NP2, the first "01001" and "01002" are the program numbers, and "G50X...Z..." are the machine origin and turret rotation position input in step 8 in Figure 3. NC data for the coordinate system setting specified from "G00 T...", "G00" is a G function command indicating that the subsequent path data is positioning until G01 to G03 are commanded, "T..." is NC data for tool selection specified by the tool data input in the 10th step, "G96 S...M03" is NC data for specifying spindle rotation, "G68" indicates that the subsequent cutting process is a balance cut process (balance cut mode) )
The function command "G69" is the G function command for balance cut mode cancel. "G68" is one NC
When commanded by the program, pulse distribution will stop until "G68" is commanded by the other NC program, and when "G68" is commanded by the other NC program, the pulse distribution in the cutting feed of the double turret will be synchronized. As a result, both turrets move at the same time, making it possible to perform balanced cutting. Therefore, in the example of FIG. 9, the NC data part 1a
and 2a are executed simultaneously, and NC data part 1
b and 2b are executed simultaneously.

"M100" to "M103" are M function commands for waiting. For example, when "M100" is commanded from one NC program, control is controlled by that one NC program until "M100" is commanded from the other NC program. stops.

If creation of an NC program is requested, the processor 11 (Fig. 2) creates a first NC program that controls the first turret in the order of machining steps using the finished shape, cutting conditions, tool data, etc. At the same time, "G68" indicating balance cut mode is inserted before the NC data for executing the balance cut process, and "G69" indicating balance cut mode cancellation is inserted after the NC data. After that, the processor 11 similarly creates a second NC program to control the second turret, and also writes "G68" before and after the balance cut NC data part.
Insert "G69" and finish the NC program creation process.

<Effects of the Invention> According to the present invention, even when the cutting edge angles and edge angles of the first and second tools specified as tools used for balance cutting are different from each other, the first and second tools are Since the NC data is created so that the cutting edge paths of the second tool match and do not interfere with the workpiece, the degree of freedom in tool selection is increased and tool identification becomes easier.
Furthermore, it is possible to reduce the number of situations in which balance cutting cannot be performed due to the absence of a suitable tool on the tool post.

[Brief explanation of drawings]

Figure 1 is a schematic explanatory diagram of the present invention, Figure 2 is a block diagram of an automatic programming device that implements the present invention, Figure 3 is a schematic flowchart of automatic programming processing, and Figures 4 and 5 are balance cuts. A flowchart of the process of creating an NC program according to the present invention including steps, FIG. 6 is an example of a dialog screen for inputting tool data, FIG. 7 is an example of a dialog screen for inputting tool shape data, and FIGS. 8 and 9 are An explanatory diagram of the process editing screen, Fig. 10 is an explanatory diagram of shape determination of a virtual balance cut tool, and Fig. 11 is a simultaneous four-step process including the balance cut process.
Explanatory diagram of the first and second NC programs of the axis lathe,
FIG. 12 is an explanatory diagram of balance cutting, FIG. 13 is an explanatory diagram of tool shape, and FIG. 14 is an explanatory diagram of drawbacks of already proposed methods. TL11~TL12...Tools for outside diameter machining, BT
11~BT12...Bite (cutting edge), MB11~
MB12...Main cutting edge of each tool, SB11~SB12
...Secondary cutting edge.

Claims (1)

[Claims] 1. Data for displaying a dialog screen corresponding to each step of a plurality of data input steps on a display device, and specifying a finished shape, machining process, tools used, etc. by referring to each dialog screen. In an NC program creation method, the input data is used to create first and second NC programs for controlling the first and second turrets in a 4-axis lathe. If the shapes of the cutting edges of the tools in the first and second tool rests are different, the main cutting edge of the first tool and the main cutting edge of the second tool, which is tilted more toward the cutting direction, should be The main cutting edge of a hypothetical balance cutting tool is considered as the main cutting edge, and the secondary cutting edge of the first tool and the second tool, which is tilted largely in the opposite direction to the cutting direction, is assumed to be the main cutting edge of the tool. NC of a 4-axis lathe, characterized in that the NC data of the balance cut process is created assuming that the auxiliary cutting edge of a virtual balance cut tool is used for balance cutting with the virtual balance cut tool.
How to create a program.