A method for using a reference ball as a normal machining reference
By using a reference sphere as the normal machining reference in automotive stamping die manufacturing, the problems of difficulty in ensuring the accuracy of the reference surface, machining interference, and low tool setting efficiency are solved, achieving efficient and accurate normal machining and providing a means of accuracy verification.
Patent Information
- Authority / Receiving Office
- CN · China
- Patent Type
- Patents(China)
- Current Assignee / Owner
- 东风模具冲压技术有限公司
- Filing Date
- 2025-05-19
- Publication Date
- 2026-07-21
AI Technical Summary
In the manufacturing of automotive stamping dies, existing technologies suffer from problems such as difficulty in ensuring the accuracy of the reference surface, machining interference, low tool setting efficiency, and a lack of accuracy verification methods, which limit the efficiency and accuracy of complex die processing.
Using a reference sphere as the normal machining reference, the coordinates of the reference sphere's center are determined by machining a reference hole on the workpiece surface and installing the reference sphere. The reference is then aligned using contact measurement and a tool setter, enabling multi-axis CNC machining.
It eliminates datum transformation error, improves normal machining accuracy, simplifies the machining process, improves tool setting efficiency, and provides a means of verifying the accuracy of CNC milling equipment.
Smart Images
Figure CN120588018B_ABST
Abstract
Description
Technical Field
[0001] This invention relates to the field of machining in automobile manufacturing, and more specifically to a method for using a reference sphere as a normal machining reference. Background Technology
[0002] In the automotive stamping die manufacturing industry, dies are typically designed with working parts at various angles. These parts need to convert the up-and-down motion of the press into motion at arbitrary angles to meet product requirements. To machine the normal surfaces of these parts (i.e., directions not perpendicular to the bottom surface), the traditional method is to first mill three mutually perpendicular reference surfaces on the working part, namely the X, Y, and Z directions. Then, the CNC milling coordinate values are set using these reference surfaces, and corner machining is performed.
[0003] The existing technology has the following main problems:
[0004] 1. Difficulty in guaranteeing the accuracy of the datum surface: The accuracy of the milled datum surface directly affects the machining accuracy of the normal surface, but the machining accuracy of the datum surface is not easy to control, and there is a datum transformation error.
[0005] 2. Machining interference problem: When the mold structure is limited, the machining of the reference surface may require the disassembly of interfering parts, which makes the machining process cumbersome and time-consuming.
[0006] 3. Low tool setting efficiency: Traditional methods require aligning the reference planes in the X, Y, and Z directions separately, which takes a long time and is inefficient.
[0007] 4. Lack of accuracy verification methods: Existing technologies cannot effectively verify the accuracy of CNC milling equipment in normal machining, making it difficult to guarantee machining quality.
[0008] These problems limit the 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 the normal machining datum. Summary of the Invention
[0009] This invention provides a method for using a reference sphere as a normal machining reference, which overcomes the shortcomings of the prior art.
[0010] To achieve the above objectives, the present invention provides a method for using a reference sphere as a normal machining reference. The purpose of this invention is to provide a method for using a reference sphere as a normal machining reference, comprising the following steps:
[0011] S1. Machining 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. Install a reference ball: Install a reference ball inside the reference hole, and the exposed part of the reference ball forms a spherical measuring surface.
[0013] S3. Determine the coordinates of the reference ball's center: Determine the machine tool coordinates of the reference ball's center using contact measurement. Specifically, install a dial indicator on the machine tool spindle head, slide the dial indicator on the surface of the reference ball, and adjust the X and Y values of the CNC milling machine to determine the ball's center position, completing the X and Y axis reference alignment; adjust the Z-axis value until the highest point of the dial indicator contacts, completing the Z-axis reference alignment.
[0014] S4. Machining based on the ball center coordinates: Remove the dial indicator from the spindle, determine the position of the reference ball center relative to the machine tool origin, install the machining tool, and perform multi-axis CNC machining based on the ball center coordinates.
[0015] Preferably, in step S1, the diameter of the reference hole is D6H7 grade.
[0016] Preferably, in step S2, the reference ball is a standard reference ball, and the reference ball and the reference hole are interference-fitted with an interference amount of 0.005-0.008mm.
[0017] Preferably, in step S2, the diameter of the reference ball is 20mm, the distance from the center of the ball to the mounting base is 20mm, and the length of the base rod is 15mm.
[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 0.01mm.
[0020] S32. Quickly move the spindle above the reference ball, manually fine-tune the X, Y, and Z directions of the spindle until the dial indicator contacts the side surface of the reference ball. Manually rotate the spindle 360° to observe 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 X and Y coordinate values of the CNC milling machine. These coordinate values are the X and Y reference points for machining.
[0021] S33. Fine-tune the Z-axis of the CNC milling machine so that the dial indicator slides on the top surface of the reference sphere until the vertex of the reference sphere is found. Record the Z-axis coordinate value a. Quickly move the spindle to the bottom surface of the workpiece above the shim. Fine-tune the Z-axis so that the dial indicator contacts the surface of the shim until the dial indicator value matches the value of the vertex of the reference sphere. Record the Z-axis coordinate value b. The distance between the center of the reference sphere and the bottom surface of the workpiece is |b-(ar)|, and r is the radius of the reference sphere. The XYZ reference 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 from the vertical milling spindle, install the machining tool, and quickly move the vertical milling spindle to the bottom of the workpiece above the shim. Place the standard tool setter on the shim.
[0024] S42. Fine-tune the Z-axis until the tool tip contacts the tool setter surface until the tool setter's standard value h is reached. Set the Z-axis value to 0, and the distance from the tool tip to the center of the reference sphere is c = |b - (ar)| - h. Set the Z-axis machining reference to 0 + c, and record the current Z-coordinate value, thus determining the machining X, Y, and Z-axis references.
[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, change the vertical milling spindle head to a normal spindle head, and after changing to the normal spindle head, install the machining tool on the spindle.
[0027] S44. Operate the machine tool and input the spindle rotation command to rotate the five-axis head to the required machining angle. Enter the coordinates of the datum ball center found in the previous steps, and then the machine tool will automatically convert to the five-axis machining datum.
[0028] S45, Correcting the normal spindle head.
[0029] S46. Call the NC program for processing.
[0030] Preferably, in step S45, the normal spindle head is corrected;
[0031] S451. Attach the dial indicator holder to the tool holder and measure the extended length of the holder using a tape measure. Use the measured extended length of the holder + 50mm as the tool length and enter it into the CNC milling tool length parameters.
[0032] S452. Operate the machine tool, move the spindle to the machining reference point (i.e., the center point of the reference ball) and stop. Then manually adjust the normal W-axis so that the dial indicator needle lightly touches the side of the reference ball. The W-axis is equivalent to the Z-axis in the three-axis system. The Z-axis is a vertical up-and-down movement, while the W-axis of the normal spindle head is a movement along the normal direction.
[0033] S453. Manually rotate the machine tool spindle to move the dial indicator across the reference ball surface and check the dial indicator reading. If the dial indicator reading fluctuates by more than 0.02 mm, it indicates an error in the rotation of the vertical spindle 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 reading fluctuates within the specified range.
[0034] Preferably, step S45 further includes:
[0035] S454. Check the offset values of the machine tool's X, Y, and Z coordinates after the previous operation, and enter the offset values into the machine tool's coordinate translation function. The machine tool will automatically compensate to the machining reference.
[0036] Preferably, the range specified in step S453 is less than or equal to 0.01 mm.
[0037] The beneficial effects of this invention are:
[0038] 1. Unified datum: Eliminates datum transformation errors and improves normal machining accuracy;
[0039] 2. Simple processing: The design of the mounting holes for the reference ball simplifies the processing and reduces interference problems;
[0040] 3. Highly efficient alignment: The reference points 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 using the spindle and the normal detection reference ball surface. Attached Figure Description
[0042] Figure 1 This is a flowchart of the method of the present invention;
[0043] Figure 2 This is a flowchart of the steps of the present invention;
[0044] Wherein: a is a simplified diagram of the mounting hole for the reference ball; 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 Implementation
[0045] To make the technical problems, technical solutions, and beneficial effects to be solved by this application clearer, the following detailed description is provided in conjunction with the accompanying drawings and embodiments. It should be understood that the specific embodiments described herein are merely illustrative and are not intended to limit the scope of this application.
[0046] It should be noted that when a component is referred to as being "fixed to" or "set on" another component, it can be directly on or indirectly on that other component. When a component is referred to as being "connected to" another component, it can be directly connected to or indirectly connected to that other component.
[0047] It should be understood that the terms "length", "width", "upper", "lower", "front", "rear", "left", "right", "vertical", "horizontal", "top", "bottom", "inner", "outer", etc., indicate the orientation or positional relationship based on the orientation or positional relationship shown in the accompanying drawings. They 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, or be constructed and operated in a specific orientation. Therefore, they should not be construed as limitations 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 technical features indicated. Thus, a feature defined as "first" or "second" may explicitly or implicitly include one or more of that feature. In the description of this application, "multiple" means two or more, unless otherwise explicitly specified.
[0049] References to "one embodiment" or "some embodiments" as described in this specification mean that one or more embodiments of this application include a specific feature, structure, or characteristic described in connection with that embodiment. Therefore, the phrases "in one embodiment," "in some embodiments," "in other embodiments," "in still other embodiments," etc., appearing in different parts of 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 "comprising," "including," "having," and variations thereof 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] Suppose we want to perform five-axis CNC machining on a complex curved surface part. In order to ensure machining accuracy, we use the method of this invention to use a reference sphere as the normal machining reference.
[0053] Machining the reference hole (S1): On the surface of the workpiece to be machined, use the machining steps of milling the plane, drilling the center hole, drilling the bottom hole, and reaming to machine a reference hole with a diameter that meets the accuracy requirements of D6H7 grade, and ensure that the reference hole is perpendicular to the bottom plane of the workpiece.
[0054] Install the reference ball (S2): Select a standard reference ball with a diameter of 20mm, a distance of 20mm from the center of the ball to the mounting base, and a base rod length of 15mm. Install the reference ball into the reference hole processed in step 1. The reference ball and the reference hole should have an interference fit, with the interference controlled between 0.005-0.008mm, to ensure that the reference ball is installed securely and that the exposed part 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, use the dial indicator to straighten the reference surface on the workpiece, and adjust the X and Y axes of the machine tool to 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: Quickly move the spindle above the reference ball, manually fine-tune the X, Y, and Z directions of the spindle until the dial indicator contacts the side surface of the reference ball. Then manually rotate the spindle 360°, observe the dial indicator runout value, and fine-tune the X and Y directions of the CNC milling machine until the dial indicator runout value is within 0.01mm. At this point, record the current X and Y coordinate values of the CNC milling machine and determine them as the X and Y reference points for machining.
[0058] S33: Next, fine-tune the Z-axis of the CNC milling machine, allowing the dial indicator to slide on the top surface of the reference sphere to find its vertex. Record the Z-axis coordinate value 'a' at this point. Then, quickly move the spindle above the workpiece's bottom support and continue fine-tuning the Z-axis until the dial indicator contacts the support surface. When the dial indicator value matches the value at the vertex of the reference sphere, record the Z-axis coordinate value 'b'. Using the formula: distance from the center of the reference sphere to the bottom surface of the workpiece = |b - (ar)| (where r is the radius of the reference sphere), calculate the position of the sphere's center in the Z-axis direction. This completes the reference alignment for the X, Y, and Z axes.
[0059] Machining is performed using the sphere's center coordinates as a reference (S4):
[0060] S41: Remove the dial indicator from the end mill spindle and replace it with the machining tool. Quickly move the end mill spindle above the workpiece bottom support block and place a standard tool setter on the support block.
[0061] S42: Fine-tune the Z-axis until the tool tip contacts the tool setter surface until the tool setter's standard value h is reached. At this point, set the Z-axis value to 0. Based on the previously measured data, calculate the distance c = |b-(ar)|-h from the tool tip to the center of the reference ball. Then set the Z-axis machining reference = 0+c and record the current Z-coordinate value, thereby determining the X, Y, and Z-axis references required for machining.
[0062] S43: Remove the machining tool, input the spindle head change command into the machine tool, and replace the vertical milling spindle head with a normal spindle head. After the change is completed, install the machining tool on the spindle.
[0063] S44: Input the spindle rotation command into the machine tool to rotate the five-axis head to the required machining angle. Enter the coordinates of the reference sphere center obtained in the previous steps into the machine tool system, and the machine tool will automatically convert it into a five-axis machining reference.
[0064] S45: Perform normal spindle head calibration. First, attach the dial indicator holder to the tool holder, measure the extension length of the holder with a tape measure, and add 50mm to this length as the tool length, recording it in the CNC milling tool length parameters. Then, operate the machine tool to move the spindle to the machining reference point, i.e., the center point of the reference ball, and stop. Manually adjust the normal W-axis so that the dial indicator needle lightly touches the side of the reference ball. Next, manually rotate the machine tool spindle, causing the dial indicator to slide on the surface of the reference ball, and observe the dial indicator reading. If the dial indicator reading fluctuates more than 0.02mm, it indicates an error in the vertical spindle rotation to the normal axis, requiring recalibration of the coordinates. At this time, fine-tune the X, Y, and Z coordinate values until the dial indicator reading fluctuation is controlled within 0.01mm. Finally, check the offset values of the machine tool's X, Y, and Z coordinates and record these offset values in the machine tool's coordinate translation function; the machine tool will automatically compensate for the machining 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 employing the method of this invention, using a reference sphere as the normal machining reference, machining accuracy can be effectively improved, ensuring the correct orientation of the tool relative to the workpiece surface during multi-axis machining, and providing a reliable reference determination method for the precision machining of complex parts.
[0067] The following describes the process flow of the present invention in conjunction with embodiments:
[0068] I. Processing Preparation
[0069] Workpiece clamping: The workpiece to be processed is clamped stably and securely on the machine tool worktable, ensuring that the bottom plane of the workpiece is parallel to the worktable, so as to provide a stable reference for subsequent processing.
[0070] Preparation of tools for machining reference holes: Select appropriate drills, milling cutters, and reamers according to the workpiece material and machining requirements, ensure that the diameter of the tools meets the design requirements, and check the wear of the tools, replacing them if necessary.
[0071] Preparation of reference ball installation tools: Prepare auxiliary tools for installing the reference ball, such as dedicated installation clamps, screwdrivers, etc., and ensure that the tools are intact and suitable.
[0072] Preparation of measuring tools: Check the accuracy and sensitivity of the dial indicator to ensure it can accurately measure the position of the reference ball. At the same time, prepare measuring tools such as tape measures and standard tool setters, and calibrate them to ensure the reliability of the measurement results.
[0073] II. Machining of the reference hole (S1)
[0074] Start the machine tool: Connect the machine tool power supply, start the CNC system, and perform the initialization and zeroing operation of the machine tool according to the operating procedures to ensure that each axis of the machine tool is in a safe position.
[0075] Tool clamping: Install the prepared tools onto the machine tool spindle in sequence according to the machining steps, ensuring that the tools are firmly clamped and there is no looseness. Adjust the tool extension length to meet the depth requirements of machining the reference hole.
[0076] Setting machining parameters: Based on the workpiece material and tool specifications, set appropriate machining parameters such as cutting speed, feed rate, and depth of cut. 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 depth of cut should be set according to the design 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, the supply of cutting fluid, and the machining accuracy of the workpiece. If any abnormalities are found, such as excessive cutting force, machine tool vibration, or abnormal workpiece surface roughness, machining should be stopped immediately to check and troubleshoot the problem.
[0078] Inspecting the reference hole: After machining, use measuring tools to measure and inspect the geometric parameters of the reference hole, such as its diameter, depth, and perpendicularity. Ensure that the diameter of the reference hole meets the D6H7 accuracy requirement, and that the hole's axis is perpendicular to the bottom plane of the workpiece, with the error within the allowable range. If the inspection fails, analyze the cause and take corresponding remedial measures, such as remachining or repairing the workpiece.
[0079] III. Installation of the reference ball (S2)
[0080] Reference ball cleaning: Remove the standard reference ball from the packaging and use a clean soft cloth or air gun to remove dust, oil and other impurities from the surface of the ball to ensure that the surface is clean and free of stains, so as to improve the accuracy of the measurement.
[0081] Reference hole cleaning: Clean the machined reference hole with compressed air or a special cleaning tool to remove cutting fluid residue, iron filings and other debris from the hole, ensuring that the inside of the reference hole is clean and dry, providing good conditions for the installation of the reference ball.
[0082] Installing the reference ball: Slowly insert the cleaned reference ball into the reference hole. Since the reference ball and reference hole use an interference fit (0.005-0.008mm), appropriate pressure needs to be applied during installation to ensure the reference ball is securely installed. Simultaneously, carefully control the installation force to avoid damaging the reference ball or reference hole due to excessive force. After installation, check whether the exposed part of the reference ball forms a complete spherical measuring surface. The spherical surface should be free of scratches, dents, or other defects, and should fit tightly with the reference hole without any looseness.
[0083] Inspect the installation quality of the reference ball: Use measuring tools or visual inspection to check whether the installation position of the reference ball is correct, whether the center of the ball is located on the axis of the reference hole, and whether the fit between the reference ball and the reference hole meets the requirements. If any deviation or poor fit is found in the installation of the reference ball, it should be adjusted or reinstalled in time until satisfactory installation quality is achieved. The reference ball is managed as a measuring tool; its accuracy is periodically checked using a three-coordinate measuring machine. Reference balls with accuracy exceeding the tolerance are discarded and replaced with new ones.
[0084] IV. Determine the coordinates of the center of the reference sphere (S3)
[0085] Install the dial indicator: Take 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 any looseness or shaking, in order to improve the accuracy and reliability of the measurement.
[0086] Straightening the workpiece reference surface (S31): Use a dial indicator mounted on the spindle head to straighten the reference surface on the workpiece. Adjust the workpiece's position in the X and Y axes by operating the machine tool's handwheel or CNC system, ensuring the workpiece's X or Y axis is parallel to the machine tool's X or Y axis, with the error controlled within 0.01mm. During this process, carefully observe the dial indicator readings and fine-tune the workpiece's position based on the readings until the parallelism requirement is met.
[0087] Rapidly move the spindle above the reference ball (S32): Use the machine tool's rapid traverse function to quickly move the spindle above the reference ball. Manually fine-tune the spindle's position in the X, Y, and Z directions until the dial indicator needle lightly contacts the side surface of the reference ball. Then, manually rotate the spindle 360° while observing the dial indicator's runout. Fine-tune the CNC milling machine's position in the X and Y directions based on the runout until the dial indicator runout is within 0.01mm. At this point, record the current X and Y coordinate values of the CNC milling machine; these coordinate values are the X and Y reference points for machining.
[0088] Fine-tuning the spindle position to determine the Z-coordinate of the sphere center (S33): Fine-tune the Z-axis of the CNC milling machine, allowing the dial indicator to slide on the top surface of the reference sphere to find its vertex. When the dial indicator needle touches the vertex of the reference sphere, record the Z-axis coordinate value 'a' at this point. Next, quickly move the spindle above the workpiece's bottom support and fine-tune the Z-axis until the dial indicator needle touches the support surface. Adjust the Z-axis position until the dial indicator reading matches the reading at the vertex of the reference sphere; record the Z-axis coordinate value 'b' at this point. Calculate the distance from the center of the reference sphere to the bottom surface of the workpiece using the formula: |b-(ar)| (where r is the radius of the reference sphere). This completes the reference alignment of the X, Y, and Z axes.
[0089] V. Machining based on the coordinates of the sphere's center (S4)
[0090] Disassembling the dial indicator and clamping the tool (S41-S42): Remove the dial indicator from the end mill spindle and install the machining tool. Quickly move the end mill spindle above the workpiece bottom support block and place a standard tool setter on the block. Fine-tune the Z-axis until the tool tip contacts the tool setter surface until the tool setter's standard value h is reached. At this point, set the Z-axis value to 0. Based on the previously measured data, calculate the distance c = |b-(ar)|-h from the tool tip to the center of the reference ball, and set the Z-axis machining reference = 0+c. Record the current Z-coordinate value to determine the required X, Y, and Z-axis references for machining.
[0091] Spindle head replacement and tool installation (S43): Remove the machining tool, operate the machine tool and input the spindle head replacement command to replace the vertical milling spindle head with a normal spindle head. After replacement, install the machining tool on the spindle, and ensure that the tool is firmly clamped without any looseness. 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 operator inputs a spindle rotation command to rotate the five-axis head to the required machining angle. The coordinates of the datum sphere center measured in the previous steps are entered into the machine tool system, and the machine tool automatically converts it to a five-axis machining datum, ensuring that the tool can accurately cut according to the set normal direction during machining.
[0093] Correcting the normal spindle head (S45):
[0094] Measuring and setting the tool length (S451): Attach the dial indicator holder to the tool holder and use a tape measure to measure the extension length of the holder. Enter the measured holder extension length + 50mm as the tool length into the CNC milling tool length parameters to ensure the machine tool can accurately identify the tool length information, providing a basis for subsequent machining compensation.
[0095] Adjusting the normal W-axis (S452): Operate the machine tool to move the spindle to the machining reference point, i.e., the center point of the reference ball, and then manually adjust the normal W-axis until the dial indicator needle lightly touches the side of the reference ball. The W-axis is equivalent to the Z-axis in the three axes, but its direction of movement is along the normal direction. Therefore, during the adjustment process, attention should be paid to the movement accuracy of the W-axis and its contact state with the reference ball.
[0096] Checking and adjusting the dial indicator reading (S453): Manually rotate the machine tool spindle to slide the dial indicator on the surface of the reference ball and observe the fluctuation of the dial indicator reading. If the fluctuation of the dial indicator reading is greater than 0.02mm, it indicates an error in the rotation of the vertical spindle 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 fluctuation of the dial indicator reading is within 0.01mm to ensure the relative positional accuracy between the tool and the reference ball.
[0097] Coordinate offset value entry and compensation (S454): View 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 will automatically compensate for the machining reference to eliminate the impact of coordinate deviation on machining accuracy.
[0098] Calling the NC program for machining (S46): After confirming that all preparations and calibration operations are completed correctly, call the pre-programmed NC machining program and start the machine tool for multi-axis CNC machining according to the set machining parameters and toolpath. During machining, closely observe the machine tool's operating status, tool wear, and workpiece machining quality, and promptly handle any abnormalities, such as tool breakage, abnormal cutting force, or workpiece surface roughness not meeting requirements. Simultaneously, according to the machining progress and needs, promptly replace tools and replenish cutting fluid to ensure the smooth progress of the machining process.
[0099] VI. Cleaning and Inspection After Processing
[0100] Cleaning away cutting fluid and metal shavings: After machining, shut down the machine tool spindle and CNC system, and disconnect the power. Use a dedicated cleaning tool to remove any remaining cutting fluid and metal shavings from the workpiece surface and machine tool table, keeping the machining environment clean and the workpiece surface tidy.
[0101] Removing the reference ball: Carefully remove the reference ball installed in the reference hole, taking care not to damage the reference hole or the reference ball. Clean and properly store the removed reference ball for future use.
[0102] Workpiece inspection: Using various measuring tools and testing equipment, such as coordinate measuring machines and surface roughness testers, a comprehensive inspection is performed on the machined workpieces to check their geometric dimensions, shape accuracy, positional accuracy, and surface roughness. Based on the inspection results, it is determined whether the workpiece meets the design requirements and machining accuracy standards. If machining errors or defects are found, the causes should be analyzed and corresponding remedial measures should be taken, such as trimming, rework, or adjusting machining process parameters.
[0103] Recording and Feedback: Detailed records of the processing parameters, measurement results, problems encountered, and solutions are kept in the process documents and quality record sheets to provide a reference for subsequent processing and process improvement. Simultaneously, problems and suggestions encountered during processing are fed back to the process department and relevant departments to continuously optimize the process flow and improve processing quality.
[0104] The above process flow is for reference only. It can be appropriately adjusted and optimized according to the actual processing equipment, workpiece characteristics and process requirements to ensure the efficiency, stability and reliability of the processing.
[0105] The above-described embodiments are only used to illustrate the technical solutions of this application, and are not intended to limit them. Although this application has been described in detail with reference to the foregoing embodiments, those skilled in the art should understand that modifications can still be made to the technical solutions described in the foregoing embodiments, or equivalent substitutions can be made to some of the technical features. Such modifications or substitutions do not cause the essence of the corresponding technical solutions to deviate from the spirit and scope of the technical solutions of the embodiments of this application, and should all be included within the protection scope of this application.
Claims
1. A method for using a reference sphere as a normal machining reference, characterized in that: Includes the following steps: S1. A reference hole is machined on the surface of the workpiece to be processed, and the reference hole is perpendicular to the bottom plane of the workpiece; S2. Install a reference ball inside the reference hole, and the exposed part of the reference ball forms a spherical measuring surface; S3. Determine the machine tool coordinates of the center of the reference ball through 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 machine to determine the position of the ball center, complete the X and Y axis reference alignment, adjust the Z axis value so that the highest point of the dial indicator contacts, and complete the Z axis reference alignment. S4. Remove the dial indicator from the spindle, determine the position of the reference ball center relative to the machine tool origin, install the machining tool, and perform multi-axis CNC machining with the ball center coordinates as the machining reference. In step S3, the contact measurement includes the following steps: 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 0.01mm. S32. Quickly move the spindle above the reference ball, manually fine-tune the X, Y, and Z directions of the spindle until the dial indicator contacts the side surface of the reference ball. Manually rotate the spindle 360° to observe 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 X and Y coordinate values of the CNC milling machine. These coordinate values are the X and Y reference points for machining. S33. Fine-tune the CNC milling Z-axis to make the dial indicator slide on the top surface of the reference ball until the vertex of the reference ball is found; Record the Z-coordinate value a. Quickly move the spindle to the top of the workpiece bottom shim. Fine-tune the Z-coordinate so that the dial indicator contacts the surface of the shim until the dial indicator value matches the value of the datum ball vertex. Record the Z-coordinate value b. The distance between the center of the datum ball and the bottom surface of the workpiece is |b-(ar)|, and r is the radius of the datum ball. The XYZ datum alignment is now complete. 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, and quickly move the vertical milling spindle to the bottom of the workpiece on the pad. Place the standard tool setter on the pad. S42. Fine-tune the Z-axis until the tool tip contacts the surface of the tool setter until the tool setter's standard value h is reached. Set the Z-axis value to 0, and the distance from the tool tip to the center of the reference ball is c = |b-(ar)|-h. Set the Z-axis machining reference = 0+c, and record the current Z coordinate value, thus determining the machining X, Y, and Z-axis references. 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 the spindle head change command, change the vertical milling spindle head to a normal spindle head, and after changing to the normal spindle head, install the machining tool on the spindle. S44. Operate the machine tool and 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 found in the previous steps, and then the machine tool will automatically convert to the five-axis machining reference. S45, Correcting the normal spindle head; S46. Call the NC program for machining; In step S45, the normal spindle head is corrected; S451. Attach the dial indicator holder to the tool holder and use a tape measure to measure the extension length of the indicator holder. Use the measured extension length of the indicator holder + 50mm as the tool length and enter it into the CNC milling tool length parameter. S452. Operate the machine tool, move the spindle to the machining reference point, i.e., the center point of the reference ball, and stop. Then manually adjust the normal W-axis so that the dial indicator needle lightly touches the side of the reference ball. The W-axis is equivalent to the Z-axis in the three axes. The Z-axis in the three axes is vertical up and down movement, while the W-axis is movement along the normal direction. S453. Manually rotate the machine tool spindle to make the dial indicator slide on the surface of the reference ball and check the dial indicator value. If the dial indicator value fluctuates by more than 0.02 mm, it indicates that there is an error when the vertical spindle rotates 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 fluctuates within the specified range.
2. The method for using a reference sphere as a normal machining reference according to claim 1, characterized in that: In step S1: the diameter of the reference hole is D6H7 grade.
3. The method for using a reference sphere as a normal machining reference according to claim 1, characterized in that: In step S2: the reference ball is a standard reference ball, and the reference ball and the reference hole are interference-fitted with an interference amount of 0.005~0.008mm.
4. The method for using a reference sphere as a normal machining reference according to claim 1, characterized in that: In step S2: the diameter of the reference ball is 20mm, the distance from the center of the ball to the mounting base is 20mm, and the length of the base rod is 15mm.
5. The method for using a reference sphere as a normal machining reference according to claim 1, characterized in that: Step S45 further includes: S454. Check the offset values of the machine tool's X, Y, and Z coordinates after the previous operation, and enter the offset values into the machine tool's coordinate translation function. The machine tool will automatically compensate to the machining reference.
6. The method for using a reference sphere as a normal machining reference according to claim 1, characterized in that: The range specified in step S453 is less than or equal to 0.01 mm.