A numerical control machining method based on macro chamfer and draft angle overall machining

Abstract

The application provides a numerical control machining method based on macro rounding and integral machining of a draft angle. K+1 When the innermost circle is cut, the macro variable D is substituted K+1 The corresponding macro variable completes the machining of the current layer of the rounding surface, and the cycle is repeated until the rounding surface is machined at the tangent point of the arc and the draft angle. The machining process of the draft angle is similar to that of the rounding. In the method, the tool is machined along the center trajectory to avoid the generation of large heat loss of the tool when the part contour is small and the rounding is high-speed machined, the surface smoothness of the part is improved, and the macro variable calculation process is simple.

Description

Technical Field

[0001] This invention belongs to the field of CNC machining technology, specifically relating to a CNC machining method for integral machining of fillet corners and draft angles based on macros. Background Technology

[0002] The paper "Macro Programming for Overall Machining of Fillet and Draft Angle Based on Variation Compensation," Machine Tool & Hydraulics, July 2013, Vol. 41, No. 14, discloses a macro programming method for overall machining of fillet and draft angle based on variation compensation. This method analyzes the relationship between the residual height and cutting step distance on the fillet and draft angle surfaces to determine the length and radius compensation values ​​for different cutting layers. The length and radius compensation values ​​are then written into the CNC memory using parameter input instructions from the CNC system. Milling of fillet and draft angle surfaces is achieved through different compensation values. For example, the paper describes machining a part whose basic contour is a boss composed of straight lines and arcs, with fillet and draft angle features around the boss. (See [reference needed]). Figure 13 For the rounded corners, see... Figure 11 The fillet surface is the position where the rounded corner arc is tangent to the draft angle, and 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 toolpath spacing. i+1 With length compensation value H i+1 For the draft angle section, see [link / reference]. Figure 12 The draft angle is the position from the tangent point to the bottom surface of the part. The tool radius compensation value D is obtained from the conversion relationship between the residual height of the inclined plane and the tool path distance. j+1 With length compensation value H j+1 By combining the radius and length compensation values ​​from both parts, a complete general macro program, i.e., the main program, is developed to realize the machining of parts with rounded corners and draft angles. This program then calls a contour machining subroutine to machine the rounded corners and draft angles of the boss parts. This method achieves continuous machining of rounded corners and draft angles.

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

[0004] 1. When the G10 L12 command in the literature is used in conjunction with tool offset, it can only be used for finishing. When machining boss parts with rounded corners and draft angles as described in the literature, rough machining must be performed first before machining can be carried out 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. This allows the tool radius value to be adjusted arbitrarily during program execution, thereby achieving continuous changes in the machining contour. Therefore, this instruction must be used in conjunction with tool offset. Thus, each cut requires sufficient straight-line distance to add or cancel tool offset. If the distance is insufficient, the tool will overcut the part. Furthermore, the strong impact force of the tool during straight-line entry and exit will also cause poor surface finish of the part.

[0006] 3. If small fillets are used in the processing described in the literature, the following problems may occur:

[0007] (1) It will increase the difficulty of processing, making it difficult to control the cutting tool during processing, thus leading to 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 also increase the speed of tool wear and shorten the tool's service life.

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

[0011] 4. The literature describes the construction of a tool radius compensation value D in the rounded corner portion. i+1 Length compensation value H i+1 Constructing tool radius compensation value D in the draft angle region j+1 Length compensation value H j+1 The calculation process for macro variables at that time is very complicated; see [link / reference]. Figure 14 Construct a tool radius compensation value D in the rounded corner area. i+1 Length compensation value H i+1 Since OW = OG = R (rounding radius), we can deduce that ∠OWG = ∠OGW, and ∠VWO = ∠OGV = 90°, ∠VWG = ∠VGW, thus leading to... H i+1 =h i+1 -R; see also Figure 15 Construct a tool radius compensation value D in the draft angle region. j+1 Length compensation value H j+1 At that time, by With an increase in compensation values, confusion can easily arise when writing compensation values, as it is difficult to distinguish between commonly used and uncommon compensation numbers.

[0012] In summary, the processing methods disclosed in the literature have limitations. Summary of the Invention

[0013] The present application aims to overcome the distance requirement of the existing chamfer and draft angle machining method greater than the tool radius when the tool is linearly advanced and retracted, otherwise overcutting is easy to occur, and the tool is linearly advanced and retracted, the surface finish of the workpiece at the advancing and retracting points is poor; the chamfer is too small to be compensated in product contour machining; excessive length compensation value and radius compensation value are easy to cause confusion, so that other machining programs are easy to use the modified compensation value to cause errors, and the existing method is only suitable for finishing, and a macro-based overall machining numerical control machining method for chamfering and draft angle is provided.

[0014] To achieve the above object, the technical solution provided by the present application is:

[0015] A macro-based overall machining numerical control machining method for chamfering and draft angle, comprising the following steps:

[0016] Step 1: determining a basic machining contour according to the contour shape and size of the formed part;

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

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

[0019] Step 2: determining the ring cutting tool path and ring cutting sequence according to the basic machining contour;

[0020] Step 2.1: determining the end point coordinates of the left side straight line machining tool path and the right side straight line machining tool path of the outermost circle according to the basic machining contour;

[0021] Defining the length of the cuboid blank to be machined as L and the width as S; establishing a machining coordinate system, wherein the X axis and Y axis zero points are located at the center of the cuboid blank, and the Z axis zero point 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 side straight line tool path and the right side straight line tool path are parallel to the Y axis and symmetrical with respect to the Y axis; the distance from the left side straight line tool path to the Y axis is The distance from the end points of the left side straight line tool path and the right side straight line tool path to the X axis is Wherein D is the tool diameter, and the first fluctuation value ranges from 0 to 1 millimeter;

[0023] Define the end points of the right straight line tool path as a and b, and the end points of the left straight line tool path as g and h, wherein the end point a and the end point g are located on the positive direction of the Y axis; take the end point a as the lower tool point;

[0024] Step 2.2: Determine the innermost circle of the circular interpolation tool path;

[0025] Firstly, offset each part in the basic machining profile determined in step 1 outwardly Form a straight line uk, a small circular arc kl, a straight line lm, a small circular arc mn, a straight line segment np and a large circular arc segment pu which are sequentially connected, wherein the radius of the small circular arc kl and the small circular arc mn is

[0026] Extend the straight line uk to the left to Obtain point j; extend the large circular arc pu from the point u to a position with the same Y coordinate as the end point a to obtain point q, and take the point q as the tool-out position of the whole machining process;

[0027] Then the innermost circle of the circular interpolation tool path is obtained in the order of j-k-l-m-n-p-q.

[0028] Step 2.3: Determine the right end transition circular interpolation tool path and the left end transition circular interpolation tool path, which are located between the right end straight line machining tool path and the left end straight line machining tool path of the outermost circle and the innermost circle of the circular interpolation tool path;

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

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

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

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

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

[0034] Take the point j in the innermost circle of the circular interpolation tool path as a symmetric point s with respect to the X axis, and draw a circular arc passing through j and s with the sum of the major circular arc p1j1 in the basic machining profile and the tool radius as the radius, and the circular arc js intersects the horizontal line drawn from the end point h at point i, thereby obtaining the left end transition circular arc tool path ji;

[0035] Step 2.4: Determine the circular interpolation sequence:

[0036] In the chamfering and draft angle machining, the tool is lowered from the end point a, and the machining is performed in the order of right to left and outside to inside, and the machining sequence is: a-b-c-d-e-f-g-h-i-j-k-l-m-n-p-q.

[0037] Step 3: determining the chamfering surface variable and the draft angle variable;

[0038] The chamfering surface variable includes a depth independent variable #1 in the height direction, a distance #2 from the zero point of the Z axis downward to the position between the chamfering surface arc and the tangent position of the draft angle inclined line, a chamfering radius #3, a difference #4 between the chamfering radius and the depth independent variable in the height direction, and a distance D corresponding to the change of the tool tip to the chamfering surface. K+1

[0039] The height direction is downward along the zero point of the Z axis; #1 decreases from zero, and decreases by a depth value h1 from top to bottom layer by layer until the position where the chamfering surface arc and the draft angle inclined line are tangent.

[0040] The draft angle variable includes a depth independent variable #9, a distance #2 from the zero point of the Z axis downward to the position between the chamfering surface arc and the tangent position of the draft angle inclined line, a chamfering radius #3, a total height #6 of the part, a draft angle #7, and a distance D corresponding to the change of the tool tip to the draft angle. L+1 ; The initial value of #9 is zero, and the depth value h2 decreases from top to bottom layer by layer from the position where the chamfering surface arc and the draft angle inclined line are tangent, and the layers are machined until the bottom surface of the part is finished.

[0041] Step 4: designing the numerical control machining program of the chamfering surface and the draft angle surface respectively.

[0042] Step 5: chamfering and draft angle machining.

[0043] According to the set ring cutting tool path, ring cutting sequence, chamfering surface variable and draft angle variable, the numerical control machining of the chamfering surface and the draft angle surface is sequentially completed.

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

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

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

[0047] ​Further, the step 4 comprises the following sub-steps:

[0048] Step 4.1: determining the program starting point of the numerical control machining program: taking the determined lower knife point a as the program starting point;

[0049] Step 4.2: determining the tool length compensation mode: adopting the square shoulder knife with hard alloy insert to realize the tool length compensation;

[0050] Step 4.3: setting the variable parameters of the fillet surface and the draft surface by using the WHILE-DO loop instruction, wherein the variable parameters of the fillet surface and the draft surface are determined by step 3;

[0051] Step 4.4: setting the loop cutting tool path and the loop cutting sequence determined by step 2;

[0052] Step 4.5: determining the macro variable #5 and the macro variable #8; when machining the fillet surface, the macro variable #5 makes the tool return to the lower knife point a from the current layer cutting end position point q, and then enter the next layer cutting, starting from the Z axis coordinate zero point and ending at the tangent point of the fillet and the draft surface; when machining the draft surface, the macro variable #8 makes the tool return to the lower knife point a from the current layer cutting end position point q, and then enter the next layer cutting, starting from the tangent point of the fillet and the draft surface and ending at the bottom surface of the part.

[0053] Further, the step 5 comprises the following sub-steps:

[0054] Step 5.1: machining the fillet surface:

[0055] Starting the numerical control machine tool, the tool moves to the lower knife point a outside the cuboid blank, and the tool moves along the designed loop cutting tool path in the order of a-b-c-d-e-f-g-h-i-j-k-l-m-n-p-q by the center track tool path mode, and completes the current layer cutting;

[0056] The tool moves out of the current layer point q and returns to the lower knife point a; then the next layer cutting is performed by decreasing the depth h1 along the Z axis, and for each depth value h1, the tool tip has a corresponding distance D K+1 to the fillet surface; the tool is sequentially and circularly cut until the tangent position of the fillet surface and the draft surface; the machining of the fillet surface is completed;

[0057] Step 5.2: machining the draft surface:

[0058] After the tool is lifted back to the initial lower point a, the tool is walked along the designed ring 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, and the current layer cutting is completed;

[0059] The tool is lifted from the current layer point q and returned to the lower point a; then the next layer cutting is performed by decreasing along the Z axis by a depth h2, and for each depth value h2, the tool tip to the draft angle changes by a corresponding distance D L+1 ; The tool is sequentially and cyclically cut from the tangent point of the fillet arc and the draft angle straight line, and the machining of the row of draft angles is completed until the bottom surface of the part.

[0060] The advantages of the present application are:

[0061] 1. In the method of the present application, the basic machining profile is determined according to the profile of the part to be machined, and the ring cutting tool path and the ring cutting sequence are specially designed. The XY direction zero point is placed in the center of the cuboid blank, the Z direction zero point is placed on the top surface of the cuboid blank, and a square shoulder tool with a hard alloy blade is directly used to process the part features from the blank state according to the set ring cutting tool path and ring cutting sequence. Only one program is used at a time, the machining process is efficient and fast.

[0062] 2. In the present application, the tool center trajectory is used for cutting, and the feed point and the retreat point are both outside the part, which greatly improves the smoothness of the part surface.

[0063] 3. In the present application, the tool is walked along the center trajectory during the entire machining process, and the actual tool path is offset by a tool radius The radius value is the sum of the tool radius and the radius of the smaller fillet, which is not affected by the smaller fillet.

[0064] 4. In the present application, the macro variable calculation process of the fillet portion and the draft angle portion is simple, and the program running does not need too many compensation numbers, which is clear and easy to understand.

[0065] 5. The method of the present application does not need to lift the tool to cancel the tool compensation at the end of machining, effectively saving the time of tool empty running and improving the machining efficiency.

[0066] Additional aspects and advantages of the present application will be partially given in the following description, partially will become obvious from the following description, or will be understood through the practice of the present application. BRIEF DESCRIPTION OF DRAWINGS

[0067] The above and / or additional aspects and advantages of the present application will become apparent and easy to understand from the description of the embodiments combined with the following drawings, in which:

[0068] Figure 1 A flow chart of a numerical control machining method based on macro chamfering and draft angle overall machining;

[0069] Figure 2 A basic profile two shape feature schematic diagram in the embodiment of the present application;

[0070] Figure 3 A rightmost end and leftmost end tool path design schematic diagram in the embodiment of the present application;

[0071] Figure 4 A most inner circle ring cutting tool path design schematic diagram in the embodiment of the present application;

[0072] Figure 5 A right end transition tool path and left end transition tool path Mj segment distance determination path schematic diagram in the embodiment of the present application;

[0073] Figure 6 A left end hypothetical transition straight line tool path cutting schematic diagram in the embodiment of the present application;

[0074] Figure 7 A left end transition circular arc tool path radius size and endpoint i determination schematic diagram in the embodiment of the present application;

[0075] Figure 8 A ring cutting tool path sequence design schematic diagram in the embodiment of the present application;

[0076] Figure 9 A chamfer surface variable design schematic diagram in the embodiment of the present application;

[0077] Figure 10 A draft angle surface variable design schematic diagram in the embodiment of the present application;

[0078] Figure 11 A chamfer surface residual height and compensation value relationship schematic diagram in the background art;

[0079] Figure 12 A draft angle surface residual height and compensation value relationship schematic diagram in the background art;

[0080] Figure 13 A basic profile one shape feature schematic diagram in the background art;

[0081] Figure 14 A chamfer surface residual height and compensation value relationship mathematical parameter conversion schematic diagram in the background art;

[0082] Figure 15 A draft angle surface residual height and compensation value relationship mathematical parameter conversion schematic diagram in the background art. DETAILED DESCRIPTION

[0083] The embodiments of the present application are described in detail below, which are exemplary and intended to explain the present application, and cannot be understood as a limitation of the present application.

[0084] Referring to Figure 1 , the embodiment of the present application provides a numerical control machining method based on macro chamfer and draft angle overall machining, comprising the following steps:

[0085] Step 1: According to the shape and size of the part forming contour, the basic machining contour is determined.

[0086] The part to be machined has a boss composed of straight lines and circular arcs, and the boss is provided with chamfer and draft angle features around. Therefore, the determined basic machining contour includes straight lines and circular arcs, and the straight line connection has a small chamfer, as shown in Figure 2 The basic machining contour is a straight line j1k1, a small circular arc k1l1, a straight line l1m1, a small circular arc m1n1, a straight line n1p1 and a large circular arc p1j1 in sequence.

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

[0088] The side close to the straight line l1m1 of the basic machining contour is defined as the right side, and the side close to the large circular arc p1j1 is defined as the left side.

[0089] Step 2: According to the basic machining contour, the ring cutting tool path and the ring cutting sequence are determined. Specifically, it comprises the following steps:

[0090] Step 2.1: According to the basic machining contour, the end point coordinates of the left side straight line machining tool path and the right side straight line machining tool path of the outermost ring cutting tool path are determined.

[0091] Define the side length of the cuboid blank to be machined as L, the width as S; establish the machining coordinate system, wherein the zero points of the X axis and the 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.

[0092] Define the right side straight line machining tool path as straight line ab, and the left side straight line tool path as straight line gh, which are parallel to the Y axis and symmetric with respect to the Y axis. The X and Y coordinate values of the end points a and b of the right side straight line machining tool path, the X coordinate values of the end points g and h of the left side straight line machining tool path, and the Y coordinate value of the h end point are solved.

[0093] According to the principle that the tool cutting surface completely covers the blank, the X coordinate values of the end points a and b of the right side straight line are set as The X coordinate values of the end points g and h of the left side straight line are In order to make the tool to be withdrawn outside the workpiece, the Y coordinate value of the end point a is set as In order to simplify the tool path, the Y coordinate values of the end point b of the right side straight line and the end point h of the left side straight line are set as And the above first fluctuation value is between 0-1mm.

[0094] Step 2.2: referring to Figure 4 , the most inner circle inscribed tool path is determined.

[0095] Since the tool is machined along the center trajectory in the whole machining process, only the basic machining profile shape is offset outward by a tool radius The straight line j1k1, the straight line segment l1m1, the straight line segment n1p1 and the large circular arc segment j1p1 of the basic machining profile are offset to form the straight line jk, the straight line segment lm, the straight line segment np and the large circular arc segment pq, wherein the circular arc segment pq intersects with the straight line jk at the point u, and the coordinate value Y of the point u is extended outward to the coordinate value Y of the tool withdrawal point a a , to obtain the point q, and the point q is taken as the tool withdrawal position of the whole machining process. Wherein, the point j is obtained by offsetting the straight line gh in the outermost circle inscribed tool path to the right by D-the first fluctuation value, specifically, the distance of the point j to the Y axis is The first fluctuation value is between 0-1mm.

[0096] In the embodiment of the application, the tool is machined along the center trajectory in the whole machining process, and the actual tool path is the circular arc segment kl and mn which are offset by a tool radius after the small circular arc segment k1l1 and m1n1 in the determined basic machining profile. The radius value of the circular arc segment kl and the circular arc segment mn is the sum of the tool radius and the first fluctuation radius value (the first fluctuation radius value is between 0-1mm). The purpose of this is to make the basic machining profile not be affected by the small radius corner.

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

[0098] Figure 5 Step 2.3: referring to , the right end and left end transition inscribed tool paths are determined, and the right end transition inscribed tool path and the left end transition inscribed tool path are respectively located between the right end straight line machining tool path and the left end straight line machining tool path of the outermost circle and the inscribed tool path of the innermost circle.

[0099] Sub-step 2.3.1: design of the right end transition inscribed tool path

[0100] Define the coordinate value of the intersection H of the straight line segment l1m1 and the X axis in the basic machining profile as (X2, 0), and the coordinate value of the intersection F of the large circular arc segment j1p1 and the X axis as (X1, 0).

[0101] Then, the distance PQ between the innermost circle of the circular blade track kl and the rightmost linear blade track ab is:

[0102] (the first fluctuation value is between 0-1mm), assuming that the innermost circle of the circular blade track kl is offset to the right N times, then the distance L1 of each offset satisfies (the principle of the tool cutting surface completely covering the blank, it is 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 < the tool diameter D, the number of N is determined by the value of L1, and in the embodiment, N is taken as 1.

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

[0104] Substep 2.3.2: Left end transition circular blade track design

[0105] Referring to Figure 5 , set M point as the intersection point of the blade track gh and the straight line segment jk, and j point is a point on the straight line segment jk, and M point and j point are on the same horizontal line, and the trajectory of any point on the linear blade track gh is the same, but taking M point can better reflect the actual movement of the tool. First, assume that the tool moves along the M point on the leftmost linear circular blade track gh to the j point, and the distance between M point and j point satisfies Mj≤D-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 the j point of the left end transition circular blade track can be determined at this time.

[0106] Assuming that the transition circular blade track is a linear blade track, draw a straight line parallel to the Y axis through the j point, and draw a straight line parallel to the X axis positive direction through the h point, and the two straight lines intersect at point i, see Figure 6 , it can be seen that the tool will produce overcut phenomenon when it is vertically cut in the shadow part, therefore, the transition circular blade track adopts a circular blade track in the embodiment of the present application.

[0107] Referring to Figure 7 : determine the size of the left end transition circular arc tool path radius and the position of the end point of the transition circular arc tool path. The specific determination process is as follows:

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

[0109] Referring to Figure 7 , the symmetric point s of point j about the X-axis is obtained by using Master Cam software, a circular arc js with a radius equal to the sum of the radius of the large circular arc p1j1 and the tool radius is drawn through points j and s in a three-point circle drawing manner, and the circular arc js is extended to intersect a horizontal straight line drawn from point h at point i. Then, i is the other end point of the transition circular arc tool path, and the transition circular arc tool path is ji.

[0110] Step 2.4: Design the tangent sequence

[0111] Referring to Figure 7 In order to prevent the tool from being clamped during machining, the tool is used to perform tangent machining in the order from right to left and then from outside to inside, i.e., from point a (the starting point) to point g (left) to point i to point j (the start of the innermost tangent trajectory) to point k to point l to point m to point n to point p to point q (tool exit). Among them, the tangent trajectory segments cd, ef, ij, kl, mn, and pq are circular arc segments, and the tangent trajectory segments ab, bc, de, fg, gh, hi, jk, lm, and np are straight line segments. The straight line segment ab intersects the X-axis at coordinate point , the straight line segment lm intersects the X-axis at coordinate point , the circular arc segment pq intersects the X-axis at coordinate point , and the transition circular arc ji intersects the X-axis at point N.

[0112] Step 3: Design of chamfer and draft angle variables

[0113] Substep 3.1: Design of chamfer surface variables

[0114] Referring to Figure 9 Set the Z-direction zero point of numerical control machining at the top surface of the part to be machined, and process from top to bottom. Set the Z value equal to negative #1.

[0115] #1 is a height direction depth independent variable; it is a variable, and its initial value is zero. Process layer by layer from top to bottom, and decrease from zero until the position where the circular arc and the draft angle straight line are tangent.

[0116] #2 is the distance H1 from zero point to the tangential position between the arc of the fillet and the inclined line of the draft angle;

[0117] #3 is the radius R of the fillet;

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

[0119] #5 is the corresponding variable distance D between the tool tip A and the fillet; K+1。

[0120] wherein the value of #1 is less than or equal to the value of #2, and with the gradual increase of #1, the tool will gradually decrease by a depth value h1 in the Z direction, and the tool tip A will also have a corresponding variable distance D to the fillet. K+1 .

[0121] Step 3.2: Design of the variable of the draft angle

[0122] Referring to Figure 10 , #9 is a depth variable, which is initially zero, and decreases by a depth value h2 from the tangential point between the arc of the fillet and the inclined line of the draft angle, layer by layer from top to bottom, until the bottom surface of the part is finished. #2 is the distance H1 from zero point to the tangential position between the arc of the fillet and the inclined line of the draft angle.

[0123] #6 is the total height H of the part. The cuboid blank is the same height as the part to be machined, and since the Z zero point of the programming is on the top surface of the part to be machined, the value is negative.

[0124] #7 is the draft angle β, and #8 is the corresponding variable distance D between the tool tip A and the draft angle. L+1。

[0125] In the machining, #9 decreases by a layer height, and the tool tip A has a corresponding variable distance D to the draft angle. L+1 , and the corresponding variable macro variable #8 is substituted into the corresponding trajectory points of the circular tool path, so that the machining of the current layer is completed; the tool returns to the tool-down point a, and the cycle is repeated until the sum of the negative #9 and the negative #2 is greater than or equal to the value of #6, and the machining of the draft angle is completed.

[0126] Step 4: Design of the programs for the fillet and the draft angle respectively

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

[0128] The following tool point a (X a , Y aPosition as the program starting point, the lower knife point a position is determined according to the length L and width S of the cuboid blank, and since the programming X and Y zero points are symmetrically divided according to the length and width of the cuboid blank, the X coordinate corresponding to the lower knife point a is The Y coordinate value is Wherein D is the diameter of the tool, and the first fluctuation value is between 0-1mm.

[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 machining, a part is generally machined by using many tools, and the lengths of the tools are different. In order to ensure that each tool can accurately reach the programmed position, the length of a standard tool is first set, and then the lengths of other tools are measured by using a tool setting gauge. If the length of a tool is longer than that of the standard tool, the tool needs to be moved upward along the Z axis by a length value to ensure that the tool tip is at the same position as the tool tip of the standard tool. At this time, it is positive compensation G43, and the length value is input into the H register. If the first tool compensation number is 01, that is, H01. Similarly, if the length of the tool is shorter than that of the standard tool, the tool needs to be moved downward along the Z axis by a length value. This is negative compensation G44. After setting the length compensation value of each tool, the machining can be started. When the tool is replaced, the length compensation of the new tool will automatically replace the length compensation of the previous tool, so that the part can be machined quickly and efficiently. In the embodiment of the application, a square shoulder tool with a hard alloy insert is selected to realize tool length compensation.

[0131] Step 4.3: The variable parameters of the rounded corner surface and the draft surface are set by using the WHILE-DO loop instruction respectively, and the variable parameters of the rounded corner surface and the draft surface are obtained by step 3.

[0132] Step 4.4: The loop cutting tool path and the loop cutting sequence determined in step 2 are substituted into the a-b-c-d-e-f-g-h-i-j-k-l-m-n-p-q point coordinate values in turn, wherein the loop cutting paths ab, bc, de, fg, gh, hi, jk, lm, np represent straight line segments, which are represented by G01, and the loop cutting paths cd, ef, ij, kl, mn, pq represent circular arc segments, wherein the circular arc segments cd, ef, ij are inverse circular arcs, which are represented by G03, and the circular arc segments kl, mn, pq are direct circular arcs, which are represented by G02.

[0133] Step 4.5: Perform the substitution of the macro variable program of the innermost loop cutting tool path.

[0134] First, compare the basic machining contour j1-k1-l1-m1-n1-p1-j1 with the innermost loop cutting path j-k-l-m-n-p-q:

[0135]

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

[0137] Draw a straight line through point a that is parallel to the negative X-axis. This line intersects the arc pq at point q, where the x-coordinate of point q is Xq.

[0138]

[0139] When rounding the corner surface, substitute the value of macro variable #5 at the innermost circumferential tangent trajectory j, m, n, p, and point q. #5 is the corresponding change in distance D from the tool tip to the rounded corner surface. K+1 After substituting this macro variable, the rounded shape of the fillet surface gradually forms as the depth of cut decreases layer by layer. After the current layer of cutting is completed, the tool returns from point q to the entry point a(X). a Y a Once the desired position is reached, the process repeats to the next cutting layer until the bottom surface of the part is reached, completing the rounded corner machining. The macro machining program for the rounded corner surface is shown below:

[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, and is displayed as G1 Xk in the G01 modal instruction program.

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

[0143] The x-coordinate of point m is Xm = the x-coordinate of point l. l The G01 modal instruction is displayed as G1 Ym in the program.

[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, point q (Xq, Yq) is not displayed in the program: G2 Xq﹣[#5]Yq Rq﹣[#5]

[0146] Similarly, when dealing with the draft angle bevel, substitute the values ​​of macro variable #8 at points j, m, n, p, and q on the innermost circumferential cutting trajectory. The distance D from the tool tip to the draft angle bevel will change accordingly. L+1; After the macro variable is substituted, the slope shape of the draft angle is gradually formed as the tool cutting depth decreases layer by layer. After the cutting of the current layer is completed, the tool returns to the lower tool point a (X a , Y a ) position from point q and reenters the next layer of cutting until the bottom surface of the part is completed, and the machining of the draft angle slope is completed. The macro machining program of the draft angle slope is as follows:

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

[0148] k point vertical coordinate Yk = j point vertical coordinate Yj, which is displayed as G1 Xk in the G01 mode instruction program

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

[0150] m point horizontal coordinate Xm = l point horizontal coordinate X l , which is displayed as G1 Ym in the G01 mode instruction program

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

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

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

[0154] Step 5: Machining of the rounded corner surface and the draft angle slope.

[0155] Step 5.1: Machining of the rounded corner surface

[0156] The square shoulder tool with a hard alloy insert is lowered at point a on the cuboid blank, and for each depth value h1 (and 1mm≤h1≤2mm) the tool tip A point to the rounded corner surface will have a corresponding distance D K+1 , so the tool performs tooling in the order of a-b-c-d-e-f-g-h-i-j-k-l-m-n-p-q in the form of a center track, completing the cutting of the current layer, and then the tool returns to the lower tool point a from point q and decreases by a depth value h1 in the Z direction for the next layer of cutting, and so on until the rounded corner and the draft angle slope straight line are tangent, completing the machining of the rounded corner surface. See Figure 9 and Figure 10 .

[0157] Step 5.2: Machining of the draft angle slope:

[0158] After the chamfered surface is finished, the tool is lifted to the initial down position a (X a , Y a ) and is lowered, and each time the tool is lowered by a depth value h2, the distance D L+1 between the tool tip A and the draft surface changes correspondingly, so that the tool is cut in the order of a-b-c-d-e-f-g-h-i-j-k-l-m-n-p-q in the center track, from the point of tangency between the chamfered surface arc and the draft surface straight line, and is cut down in turn until the bottom surface of the part, and the processing of the draft surface is completed.

[0159] It should be noted that the subscripts in D K+1 and D L+1 are set to distinguish the two different change parameters D K+1 and D L+1 during the processing of the chamfered surface and the draft surface.

[0160] The method directly uses a square shoulder tool with a carbide blade to process the features of the part from the blank state according to the designed tool path, and efficiently completes the processing of the chamfered corner and the draft surface angle.

[0161] The above is only a specific embodiment of the present application, but the protection scope of the present application is not limited thereto, and any person skilled in the art can easily think of various equivalent modifications or replacements within the scope of the present application, and these modifications or replacements should be covered within the protection scope of the present application.

Claims

1. A CNC machining method for integral machining of fillet corners and draft angles based on macros, characterized in that, Includes the following steps: Step 1: Determine the basic machining contour based on the shape and size of the formed part; The basic processing contour is a closed contour line composed of straight line j1k1, small circular arc k1l1, straight line l1m1, small circular arc m1n1, straight line n1p1 and large circular arc p1j1, and straight line j1k1 is parallel to straight line n1p1, and straight line l1m1 is opposite to large circular arc p1j1 and perpendicular to straight line j1k1. The side of the basic machining contour closer to the straight line l1m1 is defined as the right side, and the side closer to the large circular arc p1j1 is defined as the left side; Step 2: Determine the circumferential cutting toolpath and circumferential cutting sequence based on the basic machining contour; Step 2.1: Based on the basic machining contour, determine the endpoint coordinates of the left and right linear machining toolpaths of the outermost ring; Define the length of the cuboid blank to be processed as L and the width as S; establish a machining coordinate system, where 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 and right linear toolpaths are parallel to the Y-axis and symmetrical with respect to the Y-axis; the distance from the left linear toolpath to the Y-axis is... The distance from the endpoints of the left and right linear toolpaths 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 toolpath as a and b, and the endpoints of the left linear toolpath as g and h, where endpoints a and g are located in the positive Y-axis direction; take endpoint a as the tool entry point; Step 2.2: Determine the innermost circumferential cutting tool path; First, offset each part of the basic machining contour determined in step 1 outwards. Form a series of interconnected lines: uk, kl, lm, mn, np, and pu, where the radii of kl and mn are... Extend the straight line uk to the left. The first fluctuation value is used to obtain point j; the large circular arc pu is extended from point u to a position equal to the Y coordinate of the endpoint a, and point q is used as the exit position of the entire machining process. The innermost ring cutting tool path sequence is then obtained as j﹣k﹣l﹣m﹣n﹣p﹣q; Step 2.3: Determine the right-end transition ring cutting toolpath and the left-end transition ring cutting toolpath. The right-end transition ring cutting toolpath and the left-end transition ring cutting toolpath are respectively located between the outermost right-end straight machining toolpath and the left-end straight machining toolpath and the innermost ring cutting toolpath. Step 2.3.1: Determine the right-end transition ring cutting tool path; The coordinates of the intersection point H of the line l1m1 and the X-axis in the basic machining contour are defined as (X2, 0); The small circular arc kl, straight line lm and small circular arc mn in the innermost ring cutting tool rail are offset to the right by the set offset distance L1 to obtain the right end transition ring cutting tool rail, which includes circular arc dc, straight line ed and circular arc fe. The endpoint f of circular arc fe is collinear with the endpoint g of the left straight tool rail determined in step 2.1 and the resulting straight line fg is parallel to the X-axis. in: N is the offset number; Step 2.3.2: Determine the left-end transition arc toolpath; Take the midpoint j of the innermost circumferential cutting toolpath as the symmetrical point s relative to the X-axis. With the sum of the large circular arc p1j1 in the basic machining contour and the tool radius as the radius, draw an arc passing through j and s. The arc js intersects the horizontal line drawn from the endpoint h at point i, thus obtaining the left transition circular arc toolpath ji. Step 2.4: Determine the circumferential cutting sequence: When machining rounded corners and draft angles, the cutter is made from endpoint a, and the cutter is made in a circular cut from right to left and from outside to inside. The circular cut 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 angle variables; The rounded corner surface variables include: depth variable #1 in the height direction; distance #2 from the Z-axis zero point downwards to the position where the rounded corner arc is tangent to the draft angle; rounding radius #3; difference between the rounding radius and the depth variable in the height direction #4; and the corresponding change distance D from the tool tip to the rounded corner 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 corner arc is tangent to the draft angle straight line; The draft angle variables include depth variable #9, distance #2 from the Z-axis zero point downwards to the position where the fillet arc is tangent to the draft angle straight line, fillet radius #3, total height of the part #6, draft angle #7, and the corresponding change in distance D from the tool tip to the draft angle. L+1 ; Among them, the initial value of #9 is zero. Starting from the point where the rounded corner arc is tangent to the draft angle line, the depth value h2 is decreased layer by layer from top to bottom, and the machining is carried out layer by layer until the bottom surface of the part is finished. Step 4: Design the CNC machining programs for the rounded corner surfaces and draft angles respectively; Step 5: Perform filleting and draft angle machining; The CNC machining of the rounded corner surface and draft angle is completed sequentially according to the set circumferential cutting tool path, circumferential cutting sequence, rounded corner surface variables, and draft angle surface variables.

2. The CNC machining method for integral machining of fillet corners and draft angles based on macros according to claim 1, characterized in that... It lies in: In step 1, the radii of the small arcs k1l1 and m1n1 of the basic machining contour are between 0 and 1 mm, and the radii of the small arcs k1l1 and m1n1 are equal; the diameter of the large arc p1j1 is between 150 and 200 mm.

3. The CNC machining method for integral machining of fillet corners and draft angles based on macros, as described in claim 1 or 2, is characterized in that: In step 2, the range of the first fluctuation value is 0-1mm.

4. A CNC machining method for integral machining of fillet corners and draft angles based on macros, as described in claim 1 or 2, characterized in that: In step 3, the range of depth value h1 is 1mm ≤ h1 ≤ 2mm, and the range of depth value h2 is 1mm ≤ h2 ≤ 2mm.

5. A CNC machining method for integral machining of fillet corners and draft angles based on macros, as described in claim 1 or 2, characterized in that: Step 4 includes the following sub-steps: Step 4.1: Determine the starting point of the CNC machining program: Use the determined tool entry point a as the program starting point; Step 4.2: Determine the tool length compensation method: Use a square shoulder tool with carbide inserts to achieve tool length compensation; Step 4.3: Use the WHILE-DO loop command to set the variable parameters of the fillet surface and the draft angle, respectively. The variable parameters of the fillet surface and the draft angle are determined in step 3. Step 4.4: Set the circumferential cutting tool path and circumferential cutting sequence determined in Step 2; Step 4.5: Determine macro variables #5 and #8; When machining the rounded corner surface, macro variable #5 causes the tool to return from the current layer's cutting end point q to the starting point a, and then cycle into the next layer of cutting, starting from the zero point of the Z-axis coordinate until the point where the rounded corner and the draft slope are tangent; When machining the draft slope, macro variable #8 causes the tool to return from the current layer's cutting end point q to the starting point a, and then cycle into the next layer of cutting, starting from the point where the rounded corner and the draft slope are tangent downwards until the bottom surface of the part ends.

6. The CNC machining method for integral machining of fillet corners and draft angles based on macros according to claim 5, characterized in that: Step 5 includes the following sub-steps: Step 5.1: Perform rounded corner machining: Start the CNC machine tool, move the tool to the starting point a outside the cuboid blank, and the tool moves along the designed circumferential 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 mode to complete the cutting of the current layer. The tool exits from the current layer point q and returns to the entry point a; then it proceeds to the next layer of cutting by decreasing a depth h1 along the Z-axis. For each depth h1 the tool descends, the distance D from the tool tip to the rounded corner surface changes accordingly. K+1 The cutting tool cuts in a cyclic manner until the rounded corner surface is tangent to the draft angle; thus completing the machining of the rounded corner surface. Step 5.2: Machining the draft angle: After the tool exits, it is lifted back to the initial entry point a. The tool then moves along the designed circumferential cutting path in the order of a﹣b﹣c﹣d﹣e﹣f﹣g﹣h﹣i﹣j﹣k﹣l﹣m﹣n﹣p﹣q in a center trajectory to complete the cutting of the current layer. The tool exits from the current layer point q and returns to the next cutting point a; then it proceeds to the next layer of cutting by decreasing a depth h2 along the Z-axis. For each depth h2 the tool descends, the distance D from the tool tip to the draft angle changes accordingly. L+1 The cutting tool cuts in a cyclic manner, starting from the point where the rounded corner arc and the draft angle are tangent and cutting downwards until the bottom surface of the part is reached, thus completing the machining of the draft angle.

Images