Method for using reference ball as normal machining reference

Abstract

The invention discloses a method for using a reference ball as a normal machining reference, and belongs to the field of machining of automobile manufacturing. According to the method, a datum hole is machined in the surface of a to-be-machined workpiece, a datum ball is installed, contact type measurement is used for determining machine tool coordinate system coordinates of the center of the datum ball, and then multi-axis numerical control machining is conducted with the center coordinates as the machining datum. The specific operation comprises the steps that a reference hole perpendicular to the bottom plane is machined in the surface of a workpiece, then a reference ball is installed in the hole to form a spherical measuring face, then a dial indicator slides on the surface of the reference ball to complete reference alignment of the X axis, the Y axis and the Z axis, and finally multi-axis numerical control machining is conducted with the determined sphere center coordinates as the reference. The method can effectively eliminate the reference conversion error, improve the normal machining precision, simplify the machining process, reduce the machining interference risk, improve the tool setting efficiency and verify the normal machining precision of the numerical control milling equipment, and has remarkable beneficial effects.

Description

Technical Field

[0001] The present invention relates to the field of machining in automobile manufacturing, and in particular to a method using a reference sphere as a normal machining reference. Background Art

[0002] In the automotive stamping die manufacturing industry, dies are often designed with working parts at various angles. These parts need to convert the vertical motion of the press into arbitrary angles to meet product requirements. To machine the normal surfaces of these parts (i.e., directions that are not perpendicular to the bottom surface), the traditional method is to first mill three mutually perpendicular reference planes on the working part, namely the X, Y, and Z directions. Then, the tool is aligned with these reference planes and the coordinate values ​​of the CNC milling are set before the corner processing is carried out.

[0003] The existing technology has the following main problems:

[0004] 1. The accuracy of the reference surface is difficult to guarantee: the accuracy of the milled reference surface directly affects the machining accuracy of the normal surface, but the machining accuracy of the reference surface is difficult to control, and there is a reference conversion error.

[0005] 2. Machining interference problem: When the mold structure is limited, reference surface machining may require the disassembly of interfering parts, making the machining process cumbersome and time-consuming.

[0006] 3. Low tool setting efficiency: The traditional method requires alignment of the reference surfaces in the X, Y, and Z directions respectively, which takes a long time and is inefficient.

[0007] 4. Lack of precision verification means: Existing technologies cannot effectively verify the precision of CNC milling equipment in normal processing, making it difficult to ensure processing quality.

[0008] These problems limit the application efficiency and accuracy of existing technologies in complex mold processing, and there is an urgent need for a more efficient and accurate method for setting normal processing datums. Summary of the Invention

[0009] The present invention provides a method for using a reference sphere as a normal machining reference, which is used to overcome the shortcomings of the prior art.

[0010] To achieve the above-mentioned object, the present invention provides a method for using a reference sphere as a normal machining reference. The method comprises the following steps:

[0011] S1. Machining a reference hole: machining a reference hole on the surface of the workpiece to be machined, wherein the reference hole is perpendicular to the bottom plane of the workpiece.

[0012] S2. Installing the reference ball: installing the reference ball in the reference hole, with the exposed portion of the reference ball forming a spherical measuring surface.

[0013] S3. Determine the coordinates of the center of the reference ball: Determine the coordinates of the center of the reference ball in the machine tool coordinate system through contact measurement. The specific operation is: Install a dial indicator on the machine tool spindle head, slide it across the surface of the reference ball, adjust the X and Y values ​​of the CNC milling machine to determine the center position of the ball, and complete the X and Y axis reference alignment; adjust the Z axis value so that the highest point of the dial indicator contacts, completing the Z axis reference alignment.

[0014] S4. Processing based on the spherical center coordinates: Remove the dial indicator on the spindle, determine the position of the reference spherical center relative to the machine tool origin, install the processing tool, and perform multi-axis CNC processing based on the spherical center coordinates as the processing reference.

[0015] Preferably, in step S1, the diameter of the reference hole is D6H7.

[0016] Preferably, in step S2, the reference ball is a standard reference ball, and the reference ball and the reference hole are in interference fit, with the interference being 0.005-0.008 mm.

[0017] Preferably, in step S2, the diameter of the reference ball is 20 mm, the distance from the center of the ball to the mounting base is 20 mm, and the length of the bottom rod is 15 mm.

[0018] Preferably, in step S3, the contact measurement includes the following steps:

[0019] S31. Call the spindle head of the machine tool, install a dial indicator on the spindle head, and use the dial indicator to straighten the reference surface on the workpiece so that the X or Y direction of the workpiece is parallel to the X or Y direction of the machine tool with an error within 0.01 mm.

[0020] S32. Quickly move the spindle to above the reference ball, manually fine-tune the spindle in the X, Y, and Z directions so that the dial indicator contacts the side surface of the reference ball. Manually rotate the spindle 360° to check the dial indicator runout value. Fine-tune the X and Y directions of the CNC milling until the dial indicator runout value is within 0.01mm. Record the current CNC milling X and Y coordinate values, which are the X and Y reference points of the machining.

[0021] S33. Fine-tune the Z-axis of the CNC milling machine so that the dial indicator slides across the top surface of the datum sphere until the apex of the datum sphere is found. Record the Z-axis coordinate value a. Rapidly move the spindle to the top of the shim on the workpiece bottom surface. Fine-tune the Z-axis so that the dial indicator contacts the shim surface until the dial indicator value matches the datum sphere apex. Record the Z-axis coordinate value b. The distance from the datum sphere center to the workpiece bottom surface = 1b - (ar) |, where r = the datum sphere radius. XYZ datum alignment is now complete.

[0022] Preferably, in step S4, the detailed steps for determining the position of the reference sphere center relative to the machine tool origin are as follows:

[0023] S41. Remove the dial indicator on the vertical milling spindle, install the processing tool, quickly move the vertical milling spindle to the top of the bottom iron pad of the workpiece, and place a standard tool setting instrument on the pad.

[0024] S42. Fine-tune the Z direction so that the tool tip contacts the tool setting surface until it reaches the tool setting standard value h. Set the Z value to 0, and the tool tip distance from the center of the reference sphere c = |b - (ar) | - h. Set the Z machining datum = 0 + c, and record the current Z coordinate value. This determines the machining X, Y, and Z datums.

[0025] Preferably, in step S4, the detailed steps of multi-axis CNC machining are as follows:

[0026] S43, remove the machining tool, operate the machine tool to input the spindle head change command, replace the vertical milling spindle head with a normal spindle head, and after replacing the normal spindle head, install the machining tool on the spindle.

[0027] S44. Operate the machine tool to input the spindle rotation command to rotate the five-axis head to the required processing angle, enter the coordinates of the center of the reference ball found in the previous step, and then the machine tool automatically converts it into a five-axis processing reference.

[0028] S45. Calibrate the normal spindle head.

[0029] S46, call NC program for processing.

[0030] Preferably, in step S45, the normal spindle head is calibrated;

[0031] S451. Attach the dial indicator stand to the tool handle and use a tape measure to measure the extended length of the stand. Use the measured extended length of the stand + 50mm as the tool length and enter it into the CNC milling tool length parameters.

[0032] S452. Operate the machine tool and move the spindle to the machining reference point, which is the center of the reference sphere, and stop. Then manually adjust the normal W axis so that the dial indicator needle lightly touches the side of the reference sphere. The W axis is equivalent to the Z axis in the three axes. The Z axis in the three axes moves vertically up and down, while the W axis of the normal spindle head moves in the normal direction.

[0033] S453. Manually rotate the machine tool spindle, causing the dial indicator to slide on the surface of the reference ball, and check the dial indicator value. If the dial indicator value fluctuates by more than 0.02mm, it means that an error occurred when the vertical axis rotated to the normal axis, and the coordinates need to be recalibrated. At this time, fine-tune the X, Y, and Z coordinate values ​​until the dial indicator value fluctuation is within the specified range;

[0034] Preferably, the step S45 further includes:

[0035] S454. Check the offset values ​​of the machine tool's X, Y, and Z coordinates after the previous operation, enter the offset values ​​into the machine tool's coordinate translation function, and the machine tool will automatically compensate to the processing base.

[0036] Preferably, the range specified in step S453 is less than or equal to 0.01 mm.

[0037] Beneficial effects of the present invention:

[0038] 1. Benchmark unification: eliminates benchmark conversion errors and improves normal machining accuracy;

[0039] 2. Simple processing: The mounting hole design of the reference ball simplifies the processing process and reduces interference problems;

[0040] 3. Efficient alignment: The benchmarks in the X, Y, and Z directions can be determined in one alignment, simplifying the tool setting process.

[0041] 4. Accuracy verification: The normal machining accuracy of the CNC milling equipment can be verified by detecting the surface of the reference ball in the spindle and normal direction. BRIEF DESCRIPTION OF THE DRAWINGS

[0042] Figure 1 is a flow chart of the method of the present invention;

[0043] Figure 2 is a flow chart of the steps of the present invention;

[0044] Among them: a is a schematic diagram of the reference ball mounting hole; b is a schematic diagram of step S31 in the embodiment; c is a schematic diagram of step S32 in the embodiment; d and e are schematic diagrams of step S33 in the embodiment; f is a schematic diagram of step S453 in the embodiment. DETAILED DESCRIPTION

[0045] In order to make the technical problems, technical solutions and beneficial effects to be solved by this application more clearly understood, this application is further described in detail below with reference to the accompanying drawings and embodiments. It should be understood that the specific embodiments described herein are only used to explain this application and are not intended to limit this application.

[0046] It should be noted that when an element is referred to as being “fixed on” or “disposed on” another element, it may be directly on the other element or indirectly on the other element. When an element is referred to as being “connected to” another element, it may be directly connected to the other element or indirectly connected to the other element.

[0047] It should be understood that the terms "length", "width", "up", "down", "front", "back", "left", "right", "vertical", "horizontal", "top", "bottom", "inside", "outside", etc., indicating the orientation or position relationship, are based on the orientation or position relationship shown in the accompanying drawings, and are only for the convenience of describing this application and simplifying the description, and do not indicate or imply that the device or element referred to must have a specific orientation, be constructed and operated in a specific orientation, and therefore cannot be understood as a limitation on this application.

[0048] Furthermore, the terms "first" and "second" are used for descriptive purposes only and should not be construed as indicating or implying relative importance or implicitly specifying the number of the technical features being referred to. Thus, a feature defined as "first" or "second" may explicitly or implicitly include one or more of the features. Throughout the description of this application, "plurality" means two or more, unless otherwise specifically defined.

[0049] References to "one embodiment" or "some embodiments" in this specification mean that a particular feature, structure, or characteristic described in conjunction with that embodiment is included in one or more embodiments of the present application. Thus, phrases such as "in one embodiment," "in some embodiments," "in other embodiments," and "in other embodiments" appearing in various places in this specification do not necessarily refer to the same embodiment, but rather mean "one or more but not all embodiments," unless otherwise specifically emphasized. The terms "including," "comprising," "having," and variations thereof all mean "including but not limited to," unless otherwise specifically emphasized.

[0050] The present invention will be further described below with reference to the accompanying drawings and specific embodiments.

[0051] Example

[0052] Assume that we want to perform five-axis CNC machining on a complex curved surface part. In order to ensure the machining accuracy, the method of the present invention is adopted to use the reference sphere as the normal machining reference.

[0053] Machining a reference hole (S1): On the surface of the workpiece to be machined, a reference hole with a diameter that meets the D6H7 level precision requirements is machined using the following machining steps: milling the plane - drilling the center hole - drilling the bottom hole - reaming the hole. This hole is ensured to be perpendicular to the bottom plane of the workpiece.

[0054] Install the reference sphere (S2): Select a standard reference sphere with a 20mm diameter, a 20mm distance from the center to the mounting base, and a 15mm base rod length. Install the reference sphere into the reference hole machined in step 1. Use an interference fit between the sphere and the hole, controlling the interference between 0.005-0.008mm. Ensure the reference sphere is securely installed and the exposed portion forms a spherical measuring surface.

[0055] Determine the coordinates of the center of the reference sphere (S3):

[0056] S31: Call the spindle head of the machine tool, install the dial indicator, and use the dial indicator to straighten the reference surface on the workpiece. By adjusting the X and Y axes of the machine tool, make the X or Y direction of the workpiece parallel to the X or Y direction of the machine tool, and control the error within 0.01mm.

[0057] S32: Rapidly move the spindle to above the reference sphere and manually fine-tune the spindle's X, Y, and Z directions until the dial indicator contacts the side surface of the reference sphere. Then manually rotate the spindle 360°, observe the dial indicator runout, and fine-tune the CNC milling machine's X and Y directions until the dial indicator runout is within 0.01mm. At this point, record the current CNC milling machine's X and Y coordinates and determine them as the X and Y reference points for machining.

[0058] S33: Then fine-tune the Z direction of the CNC milling machine so that the dial indicator slides on the top surface of the reference sphere, find the vertex of the reference sphere, and record the Z coordinate value a at this time. Then quickly move the spindle to the top of the shim on the bottom surface of the workpiece, and continue to fine-tune the Z direction so that the dial indicator contacts the surface of the shim. When the dial indicator value is consistent with the vertex value of the reference sphere, record the Z coordinate value b. According to the formula: the distance between the center of the reference sphere and the bottom surface of the workpiece = |b-(ar)| (where r is the radius of the reference sphere), the position of the center of the sphere in the Z axis direction is calculated, and the base alignment of the three axes XYZ is now completed.

[0059] Processing based on the spherical center coordinates (S4):

[0060] S41: Remove the dial indicator from the vertical milling spindle and replace the machining tool. Quickly move the vertical milling spindle to the top of the workpiece bottom shim and place a standard tool setting gauge on the shim.

[0061] S42: Fine-tune the Z direction until the tool tip contacts the tool setter surface, reaching the tool setter standard value h. At this point, set the Z value to 0. Based on the previously measured data, calculate the distance c from the tool tip to the center of the reference sphere as |b-(ar)|-h. Then, set the Z machining reference as 0+c and record the current Z coordinate value, thus determining the X, Y, and Z references required for machining.

[0062] S43: Remove the machining tool and operate the machine tool to input the spindle head change command to replace the vertical milling spindle head with the normal spindle head. After the replacement is completed, install the tool for machining on the spindle.

[0063] S44: Operate the machine tool to input the spindle rotation command to rotate the five-axis head to the required machining angle. Enter the coordinates of the center of the reference ball measured in the previous step into the machine tool system, and the machine tool automatically converts it into a five-axis machining reference.

[0064] S45: Perform calibration of the normal spindle head. First, attach the dial indicator stand to the tool holder, use a tape measure to measure the extended length of the stand, and add 50mm to this length as the tool length and enter it into the CNC milling tool length parameter. Then, operate the machine tool to move the spindle to the processing reference point, which is the center point of the reference sphere, and stop. Manually adjust the normal W axis so that the dial indicator needle touches the side of the reference sphere. Next, manually rotate the machine tool spindle to drive the dial indicator to slide on the surface of the reference sphere and observe the dial indicator value. If the dial indicator value fluctuates by more than 0.02mm, it indicates that there is an error when the vertical axis is rotated to the normal axis, and the coordinates need to be recalibrated. At this time, fine-tune the X, Y, and Z coordinate values ​​until the dial indicator value fluctuation is controlled within 0.01mm. Finally, check the offset values ​​of the X, Y, and Z coordinates of the machine tool and enter these offset values ​​into the machine tool coordinate translation function. The machine tool automatically compensates for the processing reference.

[0065] S46: Call the NC program and start five-axis CNC machining of the workpiece according to the set machining parameters and trajectory.

[0066] By adopting the method of the present invention and using the reference sphere as the normal machining reference, the machining accuracy can be effectively improved, and the correct posture of the tool relative to the workpiece surface during multi-axis machining can be ensured, providing a reliable reference determination method for the precision machining of complex parts.

[0067] The process flow when the present invention works is described below in conjunction with the embodiments:

[0068] 1. Processing Preparation

[0069] Workpiece clamping: Clamp the workpiece to be processed steadily and firmly on the machine tool worktable, ensuring that the bottom plane of the workpiece is parallel to the worktable, providing a stable reference for subsequent processing.

[0070] Preparation of reference hole processing tools: According to the workpiece material and processing requirements, select appropriate drill bits, milling cutters, and reamer to ensure that the diameter of the tool meets the design requirements. At the same time, check the wear of the tool and replace it if necessary.

[0071] Preparation of tools for installing the reference ball: Prepare auxiliary tools for installing the reference ball, such as special installation fixtures, screwdrivers, etc., and ensure the integrity and applicability of the tools.

[0072] Measuring tool preparation: Check the accuracy and sensitivity of the dial indicator to ensure it can accurately measure the position of the reference ball. Also, prepare measuring tools such as a tape measure and a standard tool setter, and calibrate them to ensure the reliability of the measurement results.

[0073] 2. Reference hole processing (S1)

[0074] Start the machine tool: Turn on the machine power, start the CNC system, initialize and reset the machine tool according to the operating procedures, and ensure that all axes of the machine tool are in a safe position.

[0075] Clamping the tool: Install the prepared tool on the machine tool spindle according to the processing steps, ensuring that the tool is clamped firmly and not loose. Adjust the tool extension length to meet the depth requirements of the processing reference hole.

[0076] Set machining parameters: Based on the workpiece material and tool specifications, set appropriate machining parameters such as cutting speed, feed rate, and cutting depth. Generally, the cutting speed can be selected based on empirical formulas or data provided by the tool manufacturer; the feed rate should be determined based on factors such as the tool diameter and the hardness of the workpiece material to ensure machining efficiency and hole quality; the cutting depth should be set based on the designed depth of the reference hole.

[0077] Machining the reference hole: Start the machine tool spindle, rotate the tool, and machine the reference hole according to the preset machining path and parameters. During machining, closely observe the machine tool's operating status, paying attention to changes in cutting force, cutting fluid supply, and workpiece machining accuracy. If any abnormalities are detected, such as excessive cutting force, machine vibration, or abnormal workpiece surface roughness, immediately suspend machining to inspect and correct the problem.

[0078] Inspecting the reference hole: After machining, use measuring tools to measure and inspect the reference hole's geometric parameters, including diameter, depth, and perpendicularity. Ensure that the reference hole's diameter meets D6H7 precision requirements and that the hole axis is perpendicular to the workpiece's bottom plane, with tolerances within the allowable range. If the inspection fails, analyze the cause and implement appropriate remedial measures, such as remachining or trimming the workpiece.

[0079] 3. Installation of reference ball (S2)

[0080] Cleaning the reference ball: Take the standard reference ball out of its packaging and use a clean soft cloth or air gun to remove dust, oil and other impurities from the surface of the sphere to ensure that the sphere surface is clean and free of stains to improve measurement accuracy.

[0081] Cleaning of reference hole: Use compressed air or special cleaning tools to clean the processed reference hole, remove the cutting fluid residue, iron filings and other debris in the hole, ensure that the inside of the reference hole is clean and dry, and provide good conditions for the installation of the reference ball.

[0082] Install the reference ball: Slowly insert the cleaned reference ball into the reference hole. Since the reference ball and the reference hole have an interference fit of 0.005-0.008mm, apply appropriate pressure during installation to ensure the ball is securely seated in the hole. Also, be careful to control the force required to avoid damaging the ball or hole with excessive force. After installation, inspect the exposed portion of the reference ball to ensure it forms a complete spherical measuring surface. The spherical surface should be free of scratches, dents, or other defects, and fit tightly into the hole without any looseness.

[0083] Verify the installation quality of the reference ball: Use measuring tools or visual inspection to verify that the reference ball is correctly installed, that the ball center is aligned with the axis of the reference hole, and that the fit between the reference ball and the reference hole meets the required accuracy. If any deviation or poor fit is found in the installation of the reference ball, it should be adjusted or reinstalled promptly until satisfactory installation quality is achieved. The reference ball is managed as a measuring tool and its accuracy is regularly tested using a three-dimensional coordinate system. Any reference ball with poor accuracy should be scrapped and replaced with a new one.

[0084] 4. Determine the coordinates of the center of the reference ball (S3)

[0085] Install the dial indicator: Call the spindle head of the machine tool, install the dial indicator on the spindle head, and ensure that the dial indicator head is in good contact with the surface of the reference ball. At the same time, ensure that the installation position of the dial indicator is stable without looseness or shaking, so as to improve the measurement accuracy and reliability.

[0086] Straighten the workpiece reference surface (S31): Use the dial indicator mounted on the spindle head to straighten the workpiece reference surface. Adjust the workpiece's X and Y axis position by operating the machine tool's handwheel or CNC system to ensure the workpiece's X or Y axis is parallel to the machine tool's X or Y axis, with an error within 0.01 mm. During this process, carefully observe the changes in the dial indicator reading and fine-tune the workpiece's position accordingly until the required parallelism is achieved.

[0087] Rapidly move the spindle to above the reference sphere (S32): Operate the machine tool's rapid traverse function to rapidly move the spindle above the reference sphere. Manually fine-tune the spindle position in the X, Y, and Z directions until the dial indicator needle lightly touches the side surface of the reference sphere. Then manually rotate the spindle 360° while observing the dial indicator runout. Based on the runout, fine-tune the position of the CNC milling machine in the X and Y directions until the dial indicator runout is within 0.01 mm. At this point, record the current X and Y coordinates of the CNC milling machine; these coordinates serve as the X and Y reference points for machining.

[0088] Fine-tune the spindle position to determine the Z coordinate of the center of the ball (S33): Fine-tune the Z direction of the CNC milling machine so that the dial indicator slides on the top surface of the reference sphere to find the apex of the reference sphere. When the dial indicator needle touches the apex of the reference sphere, record the Z coordinate value a at this time. Next, quickly move the spindle to the top of the shim on the bottom surface of the workpiece, and fine-tune the Z direction so that the dial indicator needle touches the surface of the shim. Adjust the Z position until the dial indicator reading is consistent with the reading at the apex of the reference sphere. At this time, record the Z coordinate value b. Calculate the distance between the center of the reference sphere and the bottom surface of the workpiece according to the formula: |b-(ar)| (where r is the radius of the reference sphere). At this point, the reference alignment of the three axes XYZ is completed.

[0089] 5. Processing based on spherical center coordinates (S4)

[0090] Remove the dial indicator and clamp the tool (S41-S42): Remove the dial indicator on the vertical milling spindle and install the machining tool. Quickly move the vertical milling spindle to above the shim on the bottom surface of the workpiece, and place a standard tool setter on the shim. Fine-tune the Z direction so that the tip of the tool contacts the surface of the tool setter until the standard value h of the tool setter is reached. At this time, set the Z direction value to 0. Based on the previously measured data, calculate the distance c = |b-(ar)|-h from the center of the reference sphere, and set the Z-direction machining reference = 0+c. Record the current Z coordinate value to determine the X, Y, and Z-direction references required for machining.

[0091] Spindle head replacement and tool installation (S43): Remove the machining tool and input the spindle head replacement command on the machine tool to replace the vertical milling spindle head with a normal spindle head. After the replacement is completed, install the tool for machining on the spindle and ensure that the tool is firmly clamped and not loose. At the same time, check whether the tool extension length and installation position meet the machining requirements.

[0092] Normal spindle head angle adjustment and datum conversion (S44): The machine tool inputs the spindle rotation command to rotate the five-axis head to the desired machining angle. The coordinates of the datum ball center measured in the previous step are entered into the machine tool system, which automatically converts them into a five-axis machining datum, ensuring that the tool accurately cuts in the set normal direction during machining.

[0093] Correction of normal spindle head (S45):

[0094] Measuring and Setting Tool Length (S451): Attach the dial indicator holder to the tool handle and use a tape measure to measure the extended length of the indicator holder. This extended length plus 50mm is used as the tool length and entered into the CNC milling tool length parameters to ensure the machine tool can accurately identify the tool length information and provide a basis for subsequent machining compensation.

[0095] Adjust the normal W axis (S452): Operate the machine tool so that the spindle moves to the machining reference point (the center of the reference sphere) and stops. Then manually adjust the normal W axis so that the dial indicator needle lightly touches the side of the reference sphere. The W axis is equivalent to the Z axis in the three-axis, but its direction of movement is along the normal direction. Therefore, during the adjustment process, pay attention to the W axis's motion accuracy and contact with the reference sphere.

[0096] Check and adjust the dial indicator values ​​(S453): Manually rotate the machine spindle, sliding the dial indicator across the surface of the reference sphere, and check for fluctuations in the dial indicator values. If the dial indicator value fluctuates by more than 0.02mm, it indicates an error in the vertical axis rotation to the normal axis, and the coordinates need to be recalibrated. Fine-tune the X, Y, and Z coordinate values ​​until the dial indicator value fluctuations are within 0.01mm to ensure the relative position accuracy between the tool and the reference sphere.

[0097] Coordinate offset value entry and compensation (S454): Check the offset values ​​of the machine tool's X, Y, and Z coordinates after the previous operation, and enter these offset values ​​into the machine tool's coordinate translation function. The machine tool automatically compensates the machining base to eliminate the influence of coordinate deviation on machining accuracy.

[0098] Calling the NC program for machining (S46): After confirming that all preparatory work and calibration operations are complete, the pre-programmed NC machining program is called and the machine tool is started to perform multi-axis CNC machining according to the set machining parameters and tool paths. During the machining process, the machine tool's operating status, tool wear, and workpiece machining quality are closely monitored, and any abnormalities that may arise, such as tool breakage, abnormal cutting forces, or workpiece surface roughness that does not meet requirements, are promptly addressed. Furthermore, tools are replaced and cutting fluids are replenished in a timely manner based on machining progress and needs to ensure smooth machining.

[0099] 6. Cleaning and inspection after processing

[0100] Clean cutting fluid and iron chips: After processing is completed, turn off the machine tool spindle and CNC system, and cut off the power supply. Use special cleaning tools to remove cutting fluid residue and iron chips on the workpiece surface and machine tool worktable to keep the processing environment tidy and the workpiece surface clean.

[0101] Remove the reference ball: Carefully remove the reference ball installed in the reference hole, taking care not to damage the reference hole and the reference ball. Clean the removed reference ball and store it properly for next use.

[0102] Workpiece Inspection: Using various measuring tools and testing equipment, such as coordinate measuring machines and roughness meters, the finished workpiece is thoroughly inspected for geometric dimensions, shape accuracy, positional accuracy, and surface roughness. Based on the inspection results, the workpiece is judged to determine whether it meets design requirements and machining accuracy standards. If machining errors or defects are found, the cause is analyzed and appropriate remedial measures are implemented, such as trimming, rework, or adjustment of machining parameters.

[0103] Recording and Feedback: The process parameters, measurement results, problems encountered, and solutions for this processing are recorded in detail in the process documents and quality record sheets to provide a reference for subsequent processing and process improvements. At the same time, problems and suggestions encountered during the processing are fed back to the process department and relevant departments to continuously optimize the process and improve the processing quality.

[0104] The above process flow is for reference only and can be appropriately adjusted and optimized according to actual processing equipment, workpiece characteristics and process requirements to ensure the efficiency, stability and reliability of the processing process.

[0105] The above-described embodiments are only used to illustrate the technical solutions of the present application, rather than to limit them. Although the present application has been described in detail with reference to the aforementioned embodiments, those skilled in the art should understand that they can still modify the technical solutions described in the aforementioned embodiments, or make equivalent replacements for some of the technical features therein. These modifications or replacements do not deviate the essence of the corresponding technical solutions from the spirit and scope of the technical solutions of the various embodiments of the present application, and should all be included in the scope of protection of the present application.

Claims

1. A method using a reference sphere as a normal machining reference, characterized in that: The steps include: S1. Processing a reference hole on the surface of a workpiece to be processed, wherein the reference hole is perpendicular to the bottom plane of the workpiece; S2. Installing a reference ball in the reference hole, wherein the exposed portion of the reference ball forms a spherical measuring surface; S3. Determine the machine tool coordinate system coordinates of the center of the reference ball by contact measurement: Install a dial indicator on the machine tool spindle head, slide the dial indicator on the surface of the reference ball, adjust the X and Y values ​​of the CNC milling to determine the position of the ball center, complete the X and Y axis reference alignment, and adjust the Z axis value so that the highest point of the dial indicator contacts, complete the Z axis reference alignment; S4. Remove the dial indicator on the spindle, determine the position of the reference sphere center relative to the machine tool origin, install the machining tool, and perform multi-axis CNC machining using the sphere center coordinates as the machining reference.

2. The method of using a reference sphere as a normal machining reference according to claim 1, wherein: In the step S1: the diameter of the reference hole is D6H7.

3. The method of using a reference sphere as a normal machining reference according to claim 1, wherein: In the step S2: the reference ball is a standard reference ball, and the reference ball and the reference hole are interference fit, with the interference being 0.005 to 0.008 mm.

4. The method of using a reference sphere as a normal machining reference according to claim 1, wherein: In step S2: the diameter of the reference ball is 20 mm, the distance from the center of the ball to the mounting base is 20 mm, and the length of the bottom rod is 15 mm.

5. The method of using a reference sphere as a normal machining reference according to claim 1, wherein: In step S3, the contact measurement includes the following steps: S31, calling the spindle head of the machine tool, installing a dial indicator on the spindle head, and using the dial indicator to straighten the reference surface on the workpiece so that the X or Y direction of the workpiece is parallel to the X or Y direction of the machine tool with an error within 0.01 mm; S32. Quickly move the spindle to above the reference ball, manually fine-tune the spindle in the X, Y, and Z directions until the dial indicator contacts the side surface of the reference ball. Manually rotate the spindle 360° to check the dial indicator runout value. Fine-tune the X and Y directions of the CNC milling machine until the dial indicator runout value is within 0.01mm. Record the current CNC milling X and Y coordinate values, which are the X and Y reference points for machining. S33. Fine-tune the Z-axis of the CNC milling machine so that the dial indicator slides across the top surface of the datum sphere until the apex of the datum sphere is found. Record the Z-axis coordinate value a. Rapidly move the spindle to the top of the shim on the workpiece bottom surface. Fine-tune the Z-axis so that the dial indicator contacts the shim surface until the dial indicator value matches the datum sphere apex. Record the Z-axis coordinate value b. The distance from the datum sphere center to the workpiece bottom surface = |b - (ar)|, and r = the datum sphere radius. XYZ datum alignment is now complete.

6. The method of using a reference sphere as a normal machining reference according to claim 1, wherein: In step S4, the detailed steps for determining the position of the reference sphere center relative to the machine tool origin are as follows: S41. Remove the dial indicator from the vertical milling spindle, install the machining tool, quickly move the vertical milling spindle to the top of the shim on the bottom surface of the workpiece, and place a standard tool setting instrument on the shim. S42. Fine-tune the Z direction so that the tool tip contacts the tool setting surface until it reaches the tool setting standard value h. Set the Z value to 0, and the tool tip distance from the center of the reference sphere c = |b - (ar) | - h. Set the Z machining datum = 0 + c, and record the current Z coordinate value. This determines the machining X, Y, and Z datums.

7. The method of using a reference sphere as a normal machining reference according to claim 1, wherein: In step S4, the detailed steps of multi-axis CNC machining are as follows: S43, remove the machining tool, operate the machine tool to input a spindle head change command, replace the vertical milling spindle head with a normal spindle head, and after replacing the normal spindle head, install the machining tool on the spindle; S44. Operate the machine tool to input a spindle rotation command to rotate the five-axis head to the required machining angle, enter the coordinates of the center of the reference ball found in the previous step, and then the machine tool automatically converts to a five-axis machining reference; S45, calibrate the normal spindle head; S46, call NC program for processing.

8. The method of using a reference sphere as a normal machining reference according to claim 7, wherein: In the step S45, the normal spindle head is corrected; S451. Attach the dial indicator stand to the tool handle and use a tape measure to measure the extended length of the stand. Use the measured extended length of the stand + 50mm as the tool length and enter it into the CNC milling tool length parameters. S452. Operate the machine tool, move the spindle to the machining reference point (the center of the reference sphere), and stop. Then manually adjust the normal W axis so that the dial indicator needle lightly touches the side of the reference sphere. The W axis is equivalent to the Z axis in the three axes. The Z axis moves vertically up and down, while the W axis moves along the normal direction. S453. Manually rotate the machine tool spindle, causing the dial indicator to slide across the surface of the reference ball. Check the dial indicator value. If the dial indicator value fluctuates by more than 0.02mm, it indicates an error in the vertical axis rotation to the normal axis, and the coordinates need to be recalibrated. Then, fine-tune the X, Y, and Z coordinate values ​​until the dial indicator value fluctuation is within the specified range.

9. The method of using a reference sphere as a normal machining reference according to claim 8, wherein: The step S45 further includes: S454. Check the offset values ​​of the machine tool's X, Y, and Z coordinates after the previous operation, enter the offset values ​​into the machine tool's coordinate translation function, and the machine tool will automatically compensate to the processing base.

10. The method of using a reference sphere as a normal machining reference according to claim 8, wherein: The range specified in step S453 is 0.01 mm.

Images