Numerical control machining method based on macro fillet and draft slope integral machining

Abstract

The invention provides a numerical control machining method based on macro fillet and draft slope integral machining. According to the method, in the whole machining process, a cutter is fed according to a center track, the cutter is made to conduct ring cutting from right to left and from outside to inside in sequence through ring cutting of a cutter path, fillet face chamfering, inclined face draft, macro variable substitution and machining scheme design, and during round face chamfering machining, when the cutter descends by a depth value h1, machining is completed. A correspondingly changed distance DK + 1 appears at the point A of the tool nose, at the moment, the macro variable corresponding to the DK + 1 is substituted into the innermost ring cutting tool path to complete the processing of the current layer of fillet surface, and the process is circulated until the processing of the fillet surface is completed at the tangent point of the arc and the draft inclined plane. The draft slope machining process is similar to rounding machining. According to the method, the cutter is fed according to the central track, so that huge heat loss of the cutter during high-speed machining of a small round corner of a part contour is avoided, the surface smoothness of the part is improved, and the macro-variable calculation process is simple.

Description

Technical Field

[0001] The invention belongs to the technical field of mechanical numerical control machining, and in particular relates to a numerical control machining method for integral machining of fillet corners and draft bevel surfaces based on macros. Background Art

[0002] The document "Macro Programming for Overall Processing of Chamfered Corners and Draft Bevels Based on Variable Compensation", Machine Tools and Hydraulics, Vol. 41, No. 14, July 2013, discloses a method for compiling macro programs for overall processing of chamfered corners and draft bevels based on variable compensation. This method determines the length compensation value and radius compensation value of different cutting layers by analyzing the relationship between the residual height and the cutting step on the fillet surface and the draft bevel, and writes the length compensation value and radius compensation value into the CNC storage by using the parameter input command of the CNC system, and realizes the milling of chamfered corners and draft bevels through different compensation values. For example, in the document, a part with a basic contour of a boss composed of straight lines and arcs and a chamfered corner and draft angle features around the boss is to be processed, see Fig.13 In the Rounding section, see Fig.11 The fillet surface is the position where the arc of the fillet surface is tangent to the oblique straight line of the draft chamfer surface. Its total height is R×(1-sinβ). The tool radius compensation value D is obtained based on the conversion relationship between the residual height at the fillet surface and the tool path spacing. i+1 and length compensation value H i+1 . In the Draft Angle section, see Fig.12 The draft angle is the position from the tangent point to the bottom of the part. The tool radius compensation value D is obtained by the conversion relationship between the residual height of the inclined surface and the tool path spacing. j+1 and length compensation value H j+1 The radius compensation value and length compensation value of the two parts are combined to compile a complete general macro program for machining parts with rounded corners and draft angles, namely the main program, and then the contour machining subroutine is called to realize the machining of the rounded corners and draft bevels of the boss parts. This method realizes the continuous machining of the rounded corners and draft bevels.

[0003] The disadvantages of the above processing method are:

[0004] 1. The G10 L12 command in the literature can only be used for fine machining when used in conjunction with tool offset. In the machining of boss parts with rounded corners and draft angle features in the literature, rough machining must be performed first before machining can be performed using the method described in the literature.

[0005] 2. The literature uses the G10 L12 instruction, which is used to store the tool radius compensation value in the CNC register. In this way, the tool radius value can be adjusted arbitrarily during program operation to achieve continuous changes in the machining contour. Therefore, this instruction must be used in conjunction with the tool offset. In this way, each cutting requires sufficient straight-line distance to add or cancel the tool offset. If the distance is not enough, the tool will overcut the part, and the linear advance and retract will also cause poor surface finish of the part due to the strong impact force of the tool.

[0006] 3. If too small a fillet is used for processing, the following problems will occur in the literature:

[0007] (1) It will increase the difficulty of processing and make the tool difficult to control during processing, resulting in a decrease in processing accuracy.

[0008] (2) Too small a radius will cause the tool to generate too much heat during high-speed machining, resulting in tool damage or workpiece deformation due to heat concentration.

[0009] (3) Too small a radius will increase the wear rate of the tool and shorten the service life of the tool.

[0010] There cannot be very small fillets in contour processing, otherwise compensation cannot be performed;

[0011] 4. The tool radius compensation value D is constructed in the rounded corners in the literature i+1 , length compensation value H i+1 The tool radius compensation value D is constructed in the draft angle part j+1 , length compensation value H j+1 The macro variable calculation process is very cumbersome, see Fig.14 , construct tool radius compensation value D in the rounded part i+1 , length compensation value H i+1 When OW=OG=R (rounding radius), we can infer that ∠OWG=∠OGW, and ∠VWO=∠OGV=90°, ∠VWG=∠VGW, and then we can infer H i+1 =h i+1 -R; see Fig.15 , construct the tool radius compensation value D in the draft angle part j+1 , length compensation value H j+1 When As the number of compensation values ​​increases, confusion may arise when writing compensation values ​​in order to distinguish between commonly used and uncommon compensation numbers.

[0012] Based on the above analysis, the processing method disclosed in the literature has limitations. Summary of the invention

[0013] The purpose of the present invention is to overcome the shortcomings of existing methods for processing chamfered corners and draft bevels, such as the distance during linear advance and retreat needs to be greater than the tool radius, otherwise it is easy to produce overshoot, and the tool is advanced and retreated in a linear manner, and the surface finish of the workpiece at the entry and retreat points is poor; the fillet is too small in product contour processing and cannot be compensated; too many length compensation values ​​and radius compensation values ​​are easy to cause confusion, making it easy for other processing programs to misuse the modified compensation values ​​and cause errors, and the existing methods are only suitable for fine processing. Instead, a CNC processing method for the overall processing of chamfered corners and draft bevels based on macros is provided.

[0014] To achieve the above purpose, the technical solution provided by the present invention is:

[0015] A macro-based numerical control machining method for integrally machining rounded corners and draft bevels comprises the following steps:

[0016] Step 1: Determine the basic processing profile according to the contour shape and size of the part after molding;

[0017] The basic machining profile is a closed contour line composed of a straight line j1k1, a small arc k1l1, a straight line l1m1, a small arc m1n1, a straight line n1p1 and a large arc p1j1, wherein the straight line j1k1 is parallel to the straight line n1p1, the straight line l1m1 is opposite to the large arc p1j1 and is perpendicular to the straight line j1k1; wherein the small arc k1l1 and the small arc m1n1 have the same radius, and the radius range is 0-1 mm;

[0018] Define the side of the basic machining contour close to the straight line l1m1 as the right side, and the side close to the large arc p1j1 as the left side;

[0019] Step 2: Determine the circular cutting tool path and circular cutting sequence according to the basic processing contour;

[0020] Step 2.1: According to the basic machining profile, determine the endpoint coordinates of the left and right linear machining tool paths of the outermost circle;

[0021] Define the length of the cuboid blank to be processed as L and the width as S; establish a processing coordinate system, in which the zero points of the X-axis and Y-axis are located at the center of the cuboid blank, and the zero point of the Z-axis is located at the center of the top surface of the cuboid blank; the length of the cuboid blank is along the X-axis, and the width is along the Y-axis;

[0022] The left linear tool rail and the right linear tool rail are parallel to the Y axis and symmetrical with respect to the Y axis; the distance from the left linear tool rail to the Y axis is The distance from the end point of the left linear tool rail and the right linear tool rail to the X axis is Where D is the tool diameter, and the range of the first fluctuation value is 0-1 mm;

[0023] Define the endpoints of the right linear tool path as a and b, and the endpoints of the left linear tool path as g and h, where endpoints a and g are located in the positive direction of the Y axis; take endpoint a as the cutting point;

[0024] Step 2.2: Determine the innermost circle cutting tool path;

[0025] First, offset each part of the basic machining contour determined in step 1 outward. The straight line uk, small arc kl, straight line lm, small arc mn, straight line segment np and large arc segment pu are formed in sequence, where the radius of the small arc kl and the small arc mn is

[0026] Extend the line uk to the left Get point j; extend the arc pu from point u to the position where the Y coordinate is equal to the end point a, and get point q, which is used as the tool exit position of the entire machining process;

[0027] Then the order of the innermost ring cutting tool path is j-k-l-m-n-p-q;

[0028] Step 2.3: Determine a right transition circular cutting tool track and a left transition circular cutting tool track, wherein the right transition circular cutting tool track and the left transition circular cutting tool track are respectively located between the right end linear machining tool track and the left end linear machining tool track of the outermost circle and the circular cutting tool track of the innermost circle;

[0029] Step 2.3.1: Determine the right end transition circular cutting tool path;

[0030] Define the coordinates of the intersection point H of the straight line l1m1 in the basic machining profile and the X-axis as (X2, 0);

[0031] The small arc kl, straight line lm and small arc mn in the innermost circle circular cutting tool path are offset to the right according to the set offset distance L1 to obtain the right end transition circular cutting tool path, including arc dc, straight line ed and arc fe, and the end point f of arc fe is collinear with the end point g of the left straight line tool path determined in step 2.1, and the formed straight line fg is parallel to the X axis;

[0032] in: N is the number of offsets;

[0033] Step 2.3.2: Determine the left transition arc tool path;

[0034] Take the midpoint j of the innermost circle cutting tool path as the symmetrical point s relative to the X-axis, and take the sum of the large arc p1j1 in the basic machining profile and the tool radius as the radius, and make an arc passing through j and s. The arc js intersects the horizontal line drawn from the end point h at point i, and the left end transition arc tool path ji is obtained;

[0035] Step 2.4: Determine the order of circumcision:

[0036] When processing chamfers and draft bevels, the cutter starts from end point a and cuts in a circular pattern from right to left and from outside to inside. The circular cutting sequence is: a-b-c-d-e-f-g-h-i-j-k-l-m-n-p-q.

[0037] Step 3: Determine the fillet surface variables and draft slope surface variables;

[0038] The fillet surface variables include the depth independent variable #1 in the height direction, the distance from the Z axis zero point downward to the tangent position between the fillet surface arc and the draft bevel oblique straight line #2, the fillet radius #3, the difference between the fillet radius and the depth independent variable in the height direction #4, and the change distance D corresponding to the tool tip to the fillet surface. K+1 ;

[0039] Among them, the height direction is downward along the zero point of the Z axis; #1 decreases from zero, and decreases by a depth value h1 layer by layer from top to bottom until it ends at the position where the rounded surface arc is tangent to the oblique straight line of the draft bevel surface;

[0040] The draft bevel variables include the depth independent variable #9, the distance from the Z axis zero point downward to the tangent position between the rounded corner arc and the draft bevel straight line #2, the rounded radius #3, the total height of the part #6, the draft angle #7, and the distance D corresponding to the change from the tool tip to the draft bevel L+1 ; Among them, the initial value of #9 is zero, starting from the tangent point of the rounded surface arc and the draft angle oblique line, the depth value h2 is gradually reduced from top to bottom, and processing is completed layer by layer until the bottom surface of the part is finished;

[0041] Step 4: Design the CNC machining programs for the rounded corners and draft bevels respectively;

[0042] Step 5: Process the rounded corners and draft bevels;

[0043] According to the set circular cutting tool path, circular cutting sequence, and chamfer surface variables and draft bevel surface variables, the CNC machining of the chamfer surface and the draft bevel surface is completed in sequence.

[0044] Furthermore, in step 1, the radii of the small arc k1l1 and the small arc m1n1 of the basic processing contour are between 0-1 mm, and the radii of the small arc k1l1 and the small arc m1n1 are equal; the diameter of the large arc p1j1 is between 150-200 mm.

[0045] Furthermore, in step 2, the range of the first fluctuation value is 0-1 mm.

[0046] Furthermore, in step 3, the range of the depth value h1 is 1 mm ≤ h1 ≤ 2 mm, and the range of the depth value h2 is 1 mm ≤ h2 ≤ 2 mm.

[0047] Furthermore, step 4 includes the following sub-steps:

[0048] Step 4.1: Determine the starting point of the CNC machining program: Take the determined cutting point a as the program starting point;

[0049] Step 4.2: Determine the tool length compensation method: Use a square shoulder tool with a carbide insert to achieve tool length compensation;

[0050] Step 4.3: Use the WHILE-DO loop instruction to set the variable parameters of the fillet surface and the draft bevel surface respectively, and the variable parameters of the fillet surface and the draft bevel surface are determined by step 3;

[0051] Step 4.4: Set the circular cutting tool path and circular cutting sequence determined in step 2;

[0052] Step 4.5: Determine macro variables #5 and macro variables #8; when processing the chamfered surface, the macro variable #5 causes the tool to return from the current layer cutting end position point q to the next cutting point a, and cycle into the next layer of cutting, starting from the Z-axis coordinate zero point until the chamfer and the draft chamfer oblique straight line are tangent to each other; when processing the draft chamfer, the macro variable #8 causes the tool to return from the current layer cutting end position point q to the next cutting point a, and cycle into the next layer of cutting, starting from the chamfer and the draft chamfer oblique straight line tangent to the bottom surface of the part.

[0053] Furthermore, the step 5 includes the following sub-steps:

[0054] Step 5.1: Processing of rounded corners:

[0055] Start the CNC machine tool, move the tool to the cutting point a outside the rectangular blank, and move the tool along the designed circular cutting tool path in the order of a-b-c-d-e-f-g-h-i-j-k-l-m-n-p-q in the center trajectory to complete the current layer cutting;

[0056] The tool starts from the current layer point q and returns to the next cutting point a; then it decreases a depth h1 downward along the Z axis to cut the next layer, and every time the tool descends a depth value h1, there will be a corresponding change in the distance D from the tool tip to the rounded arc surface. K+1 ; The tool cuts cyclically in sequence until the arc of the chamfered corner surface is tangent to the oblique straight line of the draft chamfered corner surface; the processing of the chamfered corner surface is completed;

[0057] Step 5.2: Processing of draft bevel:

[0058] After the tool is out of the cutter, it is lifted back to the initial cutting point a. The tool moves along the designed circular cutting tool path in the order of a-b-c-d-e-f-g-h-i-j-k-l-m-n-p-q in the form of the center trajectory to complete the current layer cutting;

[0059] The tool starts from the current layer point q and returns to the next cutting point a; then it decreases a depth h2 downward along the Z axis to cut the next layer, and every time the tool descends a depth value h2, there will be a corresponding change in the distance D from the tool tip to the draft chamfer. L+1 The tool cuts in a cycle from the point where the rounded corner arc is tangent to the oblique straight line of the draft chamfer, and then cuts downward in a cycle until the bottom surface of the part is reached, completing the processing of the draft chamfer.

[0060] The advantages of the present invention are:

[0061] 1. In the method of the present invention, the basic machining contour is determined according to the contour of the part to be machined, and the circular cutting tool path and the circular cutting sequence are specially designed. The zero point in the XY direction is placed in the center of the rectangular blank, and the zero point in the Z direction is placed on the top surface of the rectangular blank. A square shoulder tool with a carbide blade is directly used. According to the set circular cutting tool path and the circular cutting sequence, the part features are machined into shape from the blank state at one time using only one program, and the machining process is efficient and fast.

[0062] 2. The present invention uses the tool center trajectory for cutting, and the entry point and the exit point are both outside the part, which greatly improves the surface finish of the part.

[0063] 3. In the whole processing process of the present invention, the tool moves along the center trajectory, and the actual tool path is to offset the smaller fillet in the basic contour 2 outward by a tool radius. The radius value is the tool radius The sum of the radius of the smaller fillet, which is not affected by very small fillets.

[0064] 4. The macro variable calculation process of the rounded corner part and the draft angle part in the present invention is simple, does not require too many compensation numbers during program operation, and is clear and concise.

[0065] 5. When the method of the present invention is used, there is no need to lift the tool to cancel tool compensation at the end of processing, which effectively saves the time of tool idle running and improves processing efficiency.

[0066] Additional aspects and advantages of the present invention will be given in part in the following description and in part will be obvious from the following description, or will be learned through practice of the present invention. BRIEF DESCRIPTION OF THE DRAWINGS

[0067] The above and / or additional aspects and advantages of the present invention will become apparent and easily understood from the description of the embodiments in conjunction with the following drawings, in which:

[0068] Figure 1 : A flow chart of a CNC machining method for integrally machining rounded corners and draft bevels based on macros of the present invention;

[0069] Figure 2 : Schematic diagram of the shape characteristics of the basic profile II in the embodiment of the present invention;

[0070] Figure 3 : Schematic diagram of the rightmost and leftmost tool path designs in an embodiment of the present invention;

[0071] Figure 4 : Schematic diagram of the innermost ring cutting tool track design in an embodiment of the present invention;

[0072] Figure 5 : Schematic diagram of the distance determination path between the right transition tool path and the left transition tool path Mj segment in an embodiment of the present invention;

[0073] Figure 6 : Schematic diagram of an embodiment of the present invention in which the left end assumes overcutting of the transition straight line tool path;

[0074] Figure 7 : A schematic diagram of determining the radius of the left transition arc tool path and the end point i in an embodiment of the present invention;

[0075] Figure 8 : Schematic diagram of the design sequence of the circular cutting tool path in the embodiment of the present invention;

[0076] Fig. 9 : Schematic diagram of variable design of rounded corner surface in an embodiment of the present invention;

[0077] Fig.10 : Schematic diagram of variable design of draft slope in an embodiment of the present invention;

[0078] Fig.11 : A schematic diagram of the relationship between the residual height of the fillet surface and the compensation value in the background technology;

[0079] Fig.12 : A schematic diagram of the relationship between the residual height of the draft bevel and the compensation value in the background technology;

[0080] Fig.13 : Schematic diagram of basic outline and shape characteristics in the background technology;

[0081] Fig.14 : Schematic diagram of mathematical parameter conversion between the residual height of the fillet surface and the compensation value in the background technology;

[0082] Fig.15 : Schematic diagram of mathematical parameter conversion between the residual height of the draft bevel and the compensation value in the background technology. DETAILED DESCRIPTION

[0083] Embodiments of the present invention are described in detail below. The embodiments are exemplary and intended to be used to explain the present invention, but should not be construed as limiting the present invention.

[0084] Reference Figure 1 The embodiment of the present invention provides a CNC machining method for integrally machining chamfered corners and draft bevels based on macros, comprising the following steps:

[0085] Step 1: Determine the basic processing profile based on the shape and size of the part molding profile.

[0086] The part to be machined has a boss composed of straight lines and arcs, and the boss has rounded corners and draft chamfers around it. Therefore, the basic machining profile to be determined includes straight lines and arcs, and the straight line connections have small fillets, such as Figure 2 As shown, the basic machining contour is a straight line j1k1, a small arc k1l1, a straight line l1m1, a small arc m1n1, a straight line n1p1 and a large arc p1j1 which are connected in sequence.

[0087] The radii of the small arc k1l1 and the small arc m1n1 are between 0-1 mm, and the radii of the small arc k1l1 are equal to the radii of the small arc m1n1; the diameter of the large arc p1j1 is between 150-200 mm.

[0088] It is defined that the side close to the straight line l1m1 on the basic processing contour is the right side, and the side close to the large arc p1j1 is the left side.

[0089] Step 2: Determine the circular cutting tool path and circular cutting sequence according to the basic processing contour. Specifically, it includes the following steps:

[0090] Step 2.1: According to the basic machining contour, determine the endpoint coordinates of the left straight machining tool path and the right straight machining tool path of the outermost circle circular cutting tool path.

[0091] Define the side length of the rectangular blank to be processed as L and the width as S; establish a processing coordinate system, in which the zero points of the X-axis and Y-axis are located at the center of the rectangular blank, and the zero point of the Z-axis is located at the center of the top surface of the rectangular blank; the length of the rectangular blank is along the X-axis, and the width is along the Y-axis;.

[0092] Define the right linear machining tool path as line ab, and the left linear machining tool path as line gh. Line ab and line gh are parallel to the Y axis and symmetrical with respect to the Y axis. Calculate the X and Y coordinate values ​​of the endpoints a and b of the right linear machining tool path, the X coordinate values ​​of the endpoints g and h of the left linear machining tool path, and the Y coordinate value of the endpoint h.

[0093] The principle of the tool cutting surface completely covering the blank, assuming that the X coordinate values ​​of the endpoints a and b of the right straight line are The X coordinate values ​​of the left straight line endpoints g and h are In order to make the tool cut outside the workpiece, the Y coordinate value of the end point a is To simplify the tool path, the Y coordinate values ​​of the right straight line endpoint b and the left straight line endpoint h are set to And the above-mentioned first fluctuation value is between 0-1 mm.

[0094] Step 2.2: Reference Figure 4 , determine the innermost circular cutting tool path.

[0095] Since the tool moves along the center trajectory during the entire machining process, it is only necessary to offset a tool radius outward along the shape of the basic machining contour. The straight line j1k1, straight line segment l1m1, straight line segment n1p1 and large arc segment j1p1 of the basic machining contour are offset to form straight line jk, straight line segment lm, straight line segment np and large arc segment pq, where arc segment pq intersects straight line jk at point u, and point u is extended outward to the coordinate value Y at the cutting point a. a At this point, point q is obtained, and point q is used as the tool exit position of the entire machining process. Among them, point j is obtained by offsetting the straight line gh in the outermost circle cutting tool path to the right by D-the first fluctuation value. Specifically, the distance from point j to the Y axis is The first fluctuation value ranges from 0 to 1 mm.

[0096] In the embodiment of the present invention, the tool moves along the center trajectory during the entire machining process. The actual tool path is to offset the small arc segments k1l1 and m1n1 in the determined basic machining contour outward by a tool radius. The arc segments kl and mn after the cutter are the tool radius. The sum of the first fluctuation radius value (this first fluctuation radius value is between 0-1mm). The purpose of this is to ensure that the basic processing contour is not affected by the small radius fillet.

[0097] Thus, the innermost circle's annular trajectory points j﹣k﹣l﹣m﹣n﹣p﹣q are determined.

[0098] Step 2.3: Reference Figure 5 , determine the right and left transition circular cutting tool paths, the right transition circular cutting tool path and the left transition circular cutting tool path are respectively located between the right end straight machining tool path and the left end straight machining tool path of the outermost circle and the innermost circle circular cutting tool path.

[0099] Sub-step 2.3.1: Design of right transition circular cutting tool path

[0100] The coordinate value of the intersection point H of the straight line segment l1m1 and the X-axis in the basic machining contour is defined as (X2, 0), and the coordinate value of the intersection point F of the large arc segment j1p1 and the X-axis is defined as (X1, 0).

[0101] Then, the distance PQ between the innermost circular cutting straight line tool path lm and the rightmost straight line tool path ab is:

[0102] (The first fluctuation value is between 0-1mm), assuming that the innermost circle circular cutting linear tool path lm shifts to the right N times, then the distance L1 of each shift satisfies (Based on the principle that the tool cutting surface completely covers the blank, it can be known that 60% of the tool diameter D < L1 < one tool diameter D.) Since the value range of the offset distance L1 is: 60% of the tool diameter D < L1 value < tool diameter D, the number of times N is determined by the value of L1. In this embodiment, N is 1.

[0103] After the innermost circle circular cutting linear tool rail lm, arc tool rails kl and mn are offset to the right by a distance L1 at the same time, the linear tool rail lm obtains the straight line ed; the arc tool rail kl obtains the arc 1. Due to the equidistant offset, one end point of the obtained arc 1 is co-point with the end point e of the straight line ed, and the other end point is drawn to the right through the end point g of the linear tool rail gh, parallel to the X axis, so that the horizontal line intersects with the obtained arc 1, and the intersection point is the other end point f, and the arc fe is determined; the arc tool rail mn obtains the arc 2. Due to the equidistant offset, one end point is co-point with the end point d of the straight line ed, and the other end point is drawn to the left through the end point b of the linear tool rail ab, parallel to the X axis, so that the horizontal line intersects with the obtained arc 2, and the intersection point is the other end point c, and the arc dc is obtained. Then the right end transition circular cutting tool rail is obtained, including the arc dc, the straight line ed and the arc fe, and the circular cutting order is c-d-e-f.

[0104] Sub-step 2.3.2: Design of left transition arc tool path

[0105] Reference Figure 5 , set point M as the intersection of tool path gh and straight line segment jk, point j is a point on straight line segment jk, and point M and point j are on the same horizontal straight line. The trajectory of any point on the straight tool path gh is the same, but point M can better reflect the actual movement of the tool. First, assume that the tool moves from point M on the leftmost straight circular cutting tool path gh to point j, and the distance between point M and point j satisfies Mj≤D﹣the first fluctuation value (the first fluctuation value is between 0-1mm). Since the effective cutting surface of the tool needs to completely cover the blank, the position of point j on the left transition circular cutting tool path can be determined at this time.

[0106] Assuming that the transition circular cutting tool path is a straight line tool path, draw a straight line parallel to the Y axis through point j, and draw a straight line parallel to the positive direction of the X axis through point h. The two straight lines intersect at point i, see Figure 6 It can be seen that in the shaded part, overcutting will occur when the tool cuts vertically, so the transition annular cutting tool path in the embodiment of the present invention adopts an arc tool path.

[0107] Reference Figure 7 : Determine the radius of the left transition arc tool path and the position of the end point of the transition arc tool path. The specific determination process is as follows:

[0108] The arc segment p1j1 in the basic machining contour intersects the X-axis at the coordinate point F(X1,0), and the arc segment pq of the innermost circle cutting trajectory intersects the X-axis at the coordinate point In order to prevent overcutting during cutting, a transition arc is made by passing through points j and s, with the sum of the radius of the large arc p1j1 and the radius of the tool as the radius.

[0109] Reference Figure 7 , use Master Cam software to make point s symmetrical to point j about the X-axis, and use the three-point circle drawing method to make an arc js through points j and S with a radius equal to the sum of the radius of the large arc p1j1 and the tool radius, and extend the arc js to intersect the horizontal straight line drawn from point h at point i, then point i is the other endpoint of the transition arc tool path, and the transition arc tool path is ji.

[0110] Step 2.4: Design the cutting sequence

[0111] See also Figure 7 In order to prevent the tool from being stuck during the machining process, the tool performs circular cutting in the order from right to left and then from outside to inside, starting from point a (starting point) and moving along the rear edge of the cutting tool - b - c - d - e - f (right) - g (left) - h - i - j (starting from the innermost circular cutting trajectory) - k - l - m - n - p - q (exiting the tool). Among them, the circular cutting trajectory segments cd, ef, ij, kl, mn, and pq are arc segments, and the circular cutting trajectory segments ab, bc, de, fg, gh, hi, jk, lm, and np are straight line segments, and the straight line segment ab intersects the X-axis at the coordinate point The straight line segment lm intersects the X-axis at the coordinate point The arc segment pq intersects the X-axis at the coordinate point At , the transition arc ji intersects the X-axis at point N.

[0112] Step 3: Design of fillet and draft slope variables

[0113] Sub-step 3.1: Fillet surface variable design

[0114] See also Fig. 9 , set the CNC machining Z zero point on the top surface of the part to be machined, process from top to bottom, and set the Z value equal to negative #1.

[0115] #1 is the independent variable of the depth in the height direction; it is a variable with an initial value of zero, which decreases from zero as it is processed layer by layer from top to bottom, until it ends at the position where the arc is tangent to the oblique straight line of the draft chamfer;

[0116] #2 is the distance H1 from the zero point to the tangent position between the arc of the fillet surface and the oblique straight line of the draft bevel surface;

[0117] #3 is the fillet radius R;

[0118] #4 is the difference between the fillet radius R and the depth independent variable, that is, #4 = #3 - #1.

[0119] #5 is the change distance D from the tool tip point A to the rounded corner surface K+1。

[0120] Among them, the value of #1 is less than or equal to the value of #2. As #1 gradually increases, the corresponding tool will gradually decrease by a depth value h1 in the Z direction, and the distance D from the tool tip point A to the chamfered corner surface will also change accordingly. K+1 .

[0121] Step 3.2: Design of draft slope variables

[0122] Reference Fig.10 ,#9 Depth independent variable is a variable with an initial value of zero. Starting from the point where the fillet surface arc and the draft angle oblique line are tangent, the depth value h2 is reduced layer by layer from top to bottom, and processing is completed layer by layer until the bottom surface of the part is finished. #2 is the distance H1 from the zero point to the position where the fillet surface arc and the draft angle oblique line are tangent.

[0123] #6 is the total height H of the part. The cuboid blank is at the same height as the part to be processed. Since the programmed Z-axis zero point is on the top surface of the part to be processed, this value is set to a negative value.

[0124] #7 is the draft angle β, #8 is the distance D from the tool tip point A to the fillet surface L+1。

[0125] During processing, every time #9 drops a layer height, there will be a corresponding change in the distance D from the tool tip point A to the draft angle slope. L+1 At the same time, the corresponding macro variable #8 is substituted into the trajectory point corresponding to the circular cutting tool path to complete the processing of the current layer; the tool returns to the lower cutting point a and cycles in sequence until the sum of negative #9 and negative #2 is greater than or equal to the value of #6, completing the processing of the draft bevel.

[0126] Step 4: Design the rounded surface and draft bevel programs separately

[0127] Step 4.1: Determine the starting point of the program.

[0128] The following knife point a(X a , Y a) position is taken as the program starting point. The position of the cutting point a is determined according to the length L and width S of the rectangular blank. Since the programming X and Y zero points are symmetrical about the length and width of the rectangular blank, the corresponding X coordinate of the cutting point a is The Y coordinate value is Where D is the tool diameter and the first fluctuation value is between 0-1 mm.

[0129] Step 4.2: Select the machining tool and perform tool length compensation.

[0130] In order to ensure that the tool can accurately reach the programmed position during processing, it is generally necessary to use many tools to process a part, and the length of each tool is different. To ensure that each tool can accurately reach the programmed position, the length of a standard tool must be set first, and then the length of other tools must be measured with a tool setting instrument. If it is longer than the standard tool, the tool must be moved upward along the Z axis by a length value to ensure that the tool tip is in the same position as the standard tool tip. At this time, it is positive compensation G43, and the length value is entered into the H register. If the compensation number of the first tool is 01, that is, H01; similarly, if the tool length is shorter than the standard tool, the tool must be moved downward along the Z axis by a length value, which is negative compensation G44. After setting the length compensation value of each tool, the processing can be started. When the tool is replaced, the new tool compensation will automatically replace the length compensation of the previous tool, so as to quickly and efficiently process the parts. In the embodiment of the present invention, a square shoulder tool with a carbide blade is selected to realize tool length compensation.

[0131] Step 4.3: Use the WHILE-DO loop instruction to set the variable parameters of the chamfer surface and the draft bevel respectively, and the variable parameters of the chamfer surface and the draft bevel are determined by step 3.

[0132] Step 4.4: Determine the circular cutting tool path and circular cutting sequence according to step 2, and substitute the coordinate values ​​of each point a-b-c-d-e-f-g-h-i-j-k-l-m-n-p-q in turn, where the circular cutting trajectory ab, bc, de, fg, gh, hi, jk, lm, np represents a straight line segment, expressed by G01, and the circular cutting trajectory cd, ef, ij, kl, mn, pq represents an arc segment, the arc segments cd, ef, ij are counter-clockwise arcs, expressed by G03, and the arc segments kl, mn, pq are clockwise arcs, expressed by G02.

[0133] Step 4.5: Substitute the innermost circle cutting tool path into the macro variable program design.

[0134] First, compare the basic machining profile j1﹣k1﹣l1﹣m1﹣n1﹣p1﹣j1 with the innermost circle annular cutting trajectory j﹣k﹣l﹣m﹣n﹣p﹣q:

[0135]

[0136] Then, draw a graph to obtain the horizontal coordinates of points p and q; draw a straight line through point n parallel to the negative direction of the X-axis, which intersects the pq arc at point p, and obtains the horizontal coordinate Xp of point p.

[0137] Draw a straight line through point a parallel to the negative direction of the X-axis. The straight line intersects the arc pq at point q. The horizontal coordinate of point q is Xq.

[0138]

[0139] When rounding the corners, substitute the value of macro variable #5 at the innermost circular cutting trajectory j, m, n, p, and point q. #5 is the corresponding change in distance D from the tool tip to the rounded arc surface. K+1 , after being substituted into the macro variable, the arc shape of the rounded corner surface is gradually formed as the cutting depth of the tool decreases layer by layer. After the current layer is cut, the tool returns from point q to the next cutting point a (X a , Y a ) position, and then circulate to the next layer of cutting until the bottom surface of the part ends, completing the processing of the chamfered surface. The macro processing program of the chamfered surface is as follows:

[0140] j point (Xj, Yj): G2 Xj Yj+[#5]Rj

[0141] The ordinate of point k, Yk, is equal to the ordinate of point j, Yj, which is displayed as G1 Xk in the G01 modal command program.

[0142] Arc segment kl corresponds to point l: G2 X l +[#5]Y l R l +[#5]

[0143] The horizontal coordinate of point m, Xm, is equal to the horizontal coordinate of point l, X l , which is displayed in the program as G1 Ym by the G01 modal command

[0144] n point (Xn, Yn): G2 Xn Yn﹣[#5]Rn+[#5]

[0145] Point p (Xp, Yp): G1 Xp﹣[#5], the ordinate of point p = the ordinate of point n, the program does not display Point q (Xq, Yq): G2 Xq﹣[#5]Yq Rq﹣[#5]

[0146] Similarly, when the draft angle is inclined, substitute the value of macro variable #8 at the innermost circle cutting trajectory j, m, n, p, and point q, and the distance D from the tip of #8 to the draft angle changes accordingly. L+1; After the macro variable is substituted, the chamfer shape of the draft chamfer is gradually formed as the cutting depth of the tool decreases layer by layer. After the current layer is cut, the tool returns from point q to the lower cutting point a (X a , Y a ) position, and then circulate to the next layer of cutting until the bottom surface of the part ends, completing the processing of the draft angle bevel. The macro processing program of the draft bevel is as follows:

[0147] j point (Xj, Yj): G2 Xj Yj+[#8]Rj

[0148] The ordinate of point k, Yk, is equal to the ordinate of point j, Yj, which is displayed as G1 Xk in the G01 modal command program.

[0149] Arc segment kl corresponds to point l: G2 X l +[#8]Y l R l +[#8]

[0150] The horizontal coordinate of point m, Xm, is equal to the horizontal coordinate of point l, X l , which is displayed in the program as G1 Ym by the G01 modal command

[0151] n point (Xn, Yn): G2 Xn Yn﹣[#8]Rn+[#8]

[0152] Point p (Xp, Yp): G1 Xp-[#8], the vertical coordinate of point p = the vertical coordinate of point n, not displayed in the program

[0153] Point q (Xq, Yq): G2 Xq﹣[#8]Yq Rq﹣[#8]

[0154] Step 5: Process the chamfered surfaces and draft angle bevels.

[0155] Step 5.1: Process the rounded surface

[0156] The square shoulder tool with carbide insert is cut at point a outside the rectangular blank. Every time the tool descends a depth value h1 (1mm≤h1≤2mm), there will be a corresponding change in the distance D from the tool tip point A to the chamfered surface. K+1 In this way, the tool moves along the center trajectory in the order of a-b-c-d-e-f-g-h-i-j-k-l-m-n-p-q to complete the cutting of the current layer. Then the tool returns from point q to the next cutting point a and then decreases the depth value h1 in the Z direction to cut the next layer. The cycle continues until the fillet is tangent to the draft chamfer, completing the processing of the fillet surface. Fig. 9 and Fig.10 .

[0157] Step 5.2: Processing of draft bevel:

[0158] After the rounding is completed, the tool is raised and returned to the initial cutting position a(X a , Y a ) When the tool is lowered, every time the tool descends a depth value h2, there will be a corresponding change in the distance D from the tool tip point A to the draft chamfer. L+1 In this way, the tool follows the center trajectory in the processing order of a﹣b﹣c﹣d﹣e﹣f﹣g﹣h﹣i﹣j﹣k﹣l﹣m﹣n﹣p﹣q, and cuts downward in sequence from the tangent point of the chamfered surface arc and the oblique straight line of the draft chamfer until the bottom surface of the part, completing the processing of the draft chamfer.

[0159] It should be noted that D K+1 and D L+1 The setting of the middle corner mark is only used to distinguish the two different change parameters D when the rounded surface is processed and the draft bevel surface is processed. K+1 and D L+1 .

[0160] The method of the invention directly utilizes a square shoulder tool with a carbide blade, and according to the designed machining tool path, adopts a program to machine the part features from the blank state at one time, and efficiently completes the machining of the rounded corners and the draft chamfer angles.

[0161] The above description is only a specific implementation mode of the present invention, but the protection scope of the present invention is not limited thereto. Any technician familiar with the technical field can easily think of various equivalent modifications or substitutions within the technical scope disclosed in the present invention, and these modifications or substitutions should be included in the protection scope of the present invention.

Claims

1. A CNC machining method for integral machining of chamfered corners and draft bevels based on macros, characterized in that: The following steps are involved: Step 1: Determine the basic processing profile according to the contour shape and size of the part after molding; The basic machining profile is a closed contour line composed of a straight line j1k1, a small arc k1l1, a straight line l1m1, a small arc m1n1, a straight line n1p1 and a large arc p1j1, wherein the straight line j1k1 is parallel to the straight line n1p1, and the straight line l1m1 is opposite to the large arc p1j1 and perpendicular to the straight line j1k1; Define the side of the basic machining contour close to the straight line l1m1 as the right side, and the side close to the large arc p1j1 as the left side; Step 2: Determine the circular cutting tool path and circular cutting sequence according to the basic processing contour; Step 2.1: According to the basic machining profile, determine the endpoint coordinates of the left and right linear machining tool paths of the outermost circle; Define the length of the cuboid blank to be processed as L and the width as S; establish a processing coordinate system, in which the zero points of the X-axis and Y-axis are located at the center of the cuboid blank, and the zero point of the Z-axis is located at the center of the top surface of the cuboid blank; the length of the cuboid blank is along the X-axis, and the width is along the Y-axis; The left linear tool rail and the right linear tool rail are parallel to the Y axis and symmetrical with respect to the Y axis; the distance from the left linear tool rail to the Y axis is The distance from the end point of the left linear tool rail and the right linear tool rail to the X axis is Where D is the tool diameter, and the range of the first fluctuation value is 0-1 mm; Define the endpoints of the right linear tool path as a and b, and the endpoints of the left linear tool path as g and h, where endpoints a and g are located in the positive direction of the Y axis; use endpoint a as the cutting point; Step 2.2: Determine the innermost circle cutting tool path; First, offset each part of the basic machining contour determined in step 1 outward. The straight line uk, small arc kl, straight line lm, small arc mn, straight line segment np and large arc segment pu are formed in sequence, where the radius of the small arc kl and the small arc mn is Extend the line uk to the left The first fluctuation value is obtained to obtain point j; the large arc pu is extended from point u to the position where the Y coordinate is equal to the end point a to obtain point q, and point q is used as the tool exit position of the entire machining process; Then the order of the innermost ring cutting tool path is j-k-l-m-n-p-q; Step 2.3: Determine a right transition circular cutting tool track and a left transition circular cutting tool track, wherein the right transition circular cutting tool track and the left transition circular cutting tool track are respectively located between the right end linear machining tool track and the left end linear machining tool track of the outermost circle and the circular cutting tool track of the innermost circle; Step 2.3.1: Determine the right end transition circular cutting tool path; Define the coordinates of the intersection point H of the straight line l1m1 in the basic machining profile and the X-axis as (X2, 0); The small arc kl, straight line lm and small arc mn in the innermost circle circular cutting tool path are offset to the right according to the set offset distance L1 to obtain the right end transition circular cutting tool path, including arc dc, straight line ed and arc fe, and the end point f of arc fe is collinear with the end point g of the left straight line tool path determined in step 2.1, and the formed straight line fg is parallel to the X axis; in: N is the number of offsets; Step 2.3.2: Determine the left transition arc tool path; Take the midpoint j of the innermost circle cutting tool path as the symmetrical point s relative to the X-axis, and take the sum of the large arc p1j1 in the basic machining profile and the tool radius as the radius, and make an arc passing through j and s. The arc js intersects the horizontal line drawn from the end point h at point i, and the left end transition arc tool path ji is obtained; Step 2.4: Determine the order of circumcision: When processing chamfers and draft bevels, the cutter starts from end point a and cuts in a circular pattern from right to left and from outside to inside. The circular cutting sequence is: a-b-c-d-e-f-g-h-i-j-k-l-m-n-p-q. Step 3: Determine the fillet surface variables and draft slope surface variables; The fillet surface variables include the depth independent variable #1 in the height direction, the distance from the Z axis zero point downward to the tangent position between the fillet surface arc and the draft bevel oblique straight line #2, the fillet radius #3, the difference between the fillet radius and the depth independent variable in the height direction #4, and the change distance D corresponding to the tool tip to the fillet surface. K+1 ; Among them, the height direction is downward along the zero point of the Z axis; #1 decreases from zero, and decreases by a depth value h1 layer by layer from top to bottom until it ends at the position where the rounded surface arc is tangent to the oblique straight line of the draft bevel surface; The draft bevel variables include the depth independent variable #9, the distance from the Z axis zero point downward to the tangent position between the rounded corner arc and the draft bevel straight line #2, the rounded radius #3, the total height of the part #6, the draft angle #7, and the distance D corresponding to the change from the tool tip to the draft bevel L+1 ; Among them, the initial value of #9 is zero, starting from the tangent point of the rounded surface arc and the draft angle oblique line, the depth value h2 is gradually reduced from top to bottom, and processing is completed layer by layer until the bottom surface of the part is finished; Step 4: Design the CNC machining programs for the rounded corners and draft bevels respectively; Step 5: Process the rounded corners and draft bevels; According to the set circular cutting tool path, circular cutting sequence, and chamfer surface variables and draft bevel surface variables, the CNC machining of the chamfer surface and the draft bevel surface is completed in sequence.

2. According to claim 1, a CNC machining method for integrally machining chamfered corners and draft bevels based on macros, characterized in that In: In the step 1, the radii of the small arc k1l1 and the small arc m1n1 of the basic processing contour are between 0-1 mm, and the radii of the small arc k1l1 and the small arc m1n1 are equal; the diameter of the large arc p1j1 is between 150-200 mm.

3. A CNC machining method for integrally machining chamfered corners and draft bevels based on macros according to claim 1 or 2, characterized in that: In step 2, the range of the first fluctuation value is 0-1 mm.

4. A CNC machining method for integrally machining chamfered corners and draft bevels based on macros according to claim 1 or 2, characterized in that: In step 3, the range of the depth value h1 is 1 mm ≤ h1 ≤ 2 mm, and the range of the depth value h2 is 1 mm ≤ h2 ≤ 2 mm.

5. A CNC machining method for integrally machining chamfered corners and draft bevels based on macros according to claim 1 or 2, characterized in that: The step 4 includes the following sub-steps: Step 4.1: Determine the starting point of the CNC machining program: Take the determined cutting point a as the program starting point; Step 4.2: Determine the tool length compensation method: Use a square shoulder tool with a carbide insert to achieve tool length compensation; Step 4.3: Use the WHILE-DO loop instruction to set the variable parameters of the fillet surface and the draft bevel surface respectively, and the variable parameters of the fillet surface and the draft bevel surface are determined in step 3; Step 4.4: Set the circular cutting tool path and circular cutting sequence determined in step 2; Step 4.5: Determine macro variables #5 and macro variables #8; when processing the chamfered surface, the macro variable #5 causes the tool to return from the current layer cutting end position point q to the next cutting point a, and cycle into the next layer of cutting, starting from the Z-axis coordinate zero point until the chamfer and the draft chamfer oblique straight line are tangent to each other; when processing the draft chamfer, the macro variable #8 causes the tool to return from the current layer cutting end position point q to the next cutting point a, and cycle into the next layer of cutting, starting from the chamfer and the draft chamfer oblique straight line tangent to the bottom surface of the part.

6. A CNC machining method for integrally machining rounded corners and draft bevels based on macros according to claim 5, characterized in that: The step 5 comprises the following sub-steps: Step 5.1: Processing of rounded corners: Start the CNC machine tool, move the tool to the cutting point a outside the rectangular blank, and move the tool along the designed circular cutting tool path in the order of a-b-c-d-e-f-g-h-i-j-k-l-m-n-p-q in the center trajectory to complete the current layer cutting; The tool starts from the current layer point q and returns to the next cutting point a; then it decreases a depth h1 downward along the Z axis to cut the next layer, and every time the tool descends a depth value h1, there will be a corresponding change in the distance D from the tool tip to the rounded arc surface. K+1 ; The tool cuts cyclically in sequence until the arc of the chamfered corner surface is tangent to the oblique straight line of the draft chamfered corner surface; the processing of the chamfered corner surface is completed; Step 5.2: Processing of draft bevel: After the tool is out of the cutter, it is lifted back to the initial cutting point a. The tool moves along the designed circular cutting tool path in the order of a-b-c-d-e-f-g-h-i-j-k-l-m-n-p-q in the form of the center trajectory to complete the current layer cutting; The tool starts from the current layer point q and returns to the next cutting point a; then it decreases a depth h2 downward along the Z axis to cut the next layer, and every time the tool descends a depth value h2, there will be a corresponding change in the distance D from the tool tip to the draft chamfer. L+1 The tool cuts in a cycle from the point where the rounded corner arc is tangent to the oblique straight line of the draft bevel, and then cuts downward in a cycle until the bottom surface of the part is reached, completing the processing of the draft bevel.

Images