Compilation method for parameterized numerical control machining program of marine propeller blade

Abstract

The invention relates to a programming method of a parameterized numerical control machining program of a marine propeller blade. The programming method comprises the following steps: S1, translating a coordinate system to drive a tool path; s2, completing development of a post-processing program in a post-processing builder Post Builder of Siemens NX, using a TCL language as a command language of the post-processing builder, using an original algorithm for a kinematic model of the numerical control machine tool, performing parameterized assignment on a height position adjustment value of a processing tool path in a processing program, performing automatic translation conversion on a processing coordinate system, and performing automatic translation conversion on the height position adjustment value of the processing tool path in the processing program; calculating and assigning the height adjustment value of the machining tool path in the area between the section radiuses; and S3, a tool machining track is generated in Siemens NX software according to the radius direction of the section of the blade, a post-processing program is used for being converted into a numerical control machining program, and the section needing to be adjusted is directly modified in a parameterized machining program according to the analysis condition of the blade blank.

Description

TECHNICAL FIELD

[0001] The present application relates to the field of ship propeller manufacturing, in particular, to a method for compiling a parameterized numerical control machining program of a ship propeller blade. BACKGROUND

[0002] The surface shape of the blade of a ship propeller is complex, and the shape of the blade blank cast is difficult to be consistent with the theoretical blade shape. Therefore, data measurement and analysis of the blade blank are required before machining the blade on a numerical control milling machine. Under the premise of meeting the ship propeller manufacturing standard (ISO484), the axial direction position value of the blade hub is adjusted according to the distribution of the blade blank allowance, and a three-dimensional model of the blade is reconstructed in a three-dimensional modeling software. According to the newly reconstructed three-dimensional model of the blade, a machining program of the blade is regenerated through a post-processing program matched with the machine tool, and the simulation machining of the blade is completed through a machining simulation software. After confirming that the machining program is correct, the machining program is transmitted to the numerical control machine tool for completing the machining of the corresponding blade.

[0003] The existing casting level and numerical control machining process method cannot make the blank state of each blade completely the same, so the adjustment results of the cross-sectional radius of each blade are also different. After analyzing the measurement data of the blade blank, the following work needs to be repeatedly completed: reconstructing the three-dimensional model of the blade, regenerating the machining program of the blade, and rechecking the machining program of the blade. These repetitive work consumes a lot of time, directly leading to low efficiency of the machining program compilation. SUMMARY

[0004] The purpose of the present application is to provide a method for compiling a parameterized numerical control machining program of a ship propeller blade, so as to solve the problems in the related art.

[0005] In order to achieve the above-mentioned purpose, the present application provides a method for compiling a parameterized numerical control machining program of a ship propeller blade, comprising:

[0006] Step S1: coordinate system translation to drive the tool path;

[0007] Step S2: developing a post-processing program in a post-processing constructor Post Builder of Siemens NX, using TCL language as its command language, using the original algorithm for the kinematic model of the numerical control machine tool, parameterizing and assigning the height position adjustment value of the machining tool path in the machining program, automatically translating the machining coordinate system, and calculating and assigning the height adjustment value of the machining tool path between the cross-sectional radii;

[0008] Step S3, the tool machining track is generated according to the radial direction of the blade section in the Siemens NX software, the post-processing program is used to convert into the numerical control machining program, and the section that needs to be adjusted is directly modified in the parameterized machining program according to the analysis of the blade blank.

[0009] Optionally, step S1 comprises:

[0010] Step S11, the axial position adjustment value of the blade section radius is received through the calculation of the R parameter, the machining program of the standard blade is not adjusted in the section radius position, so the adjustment value of each section radius is 0, and the R parameter corresponding to the section radius is valued as 0;

[0011] Step S12, if the position of a certain section radius needs to be adjusted, the R parameter corresponding to the section radius is directly valued, at this time, the adjustment value of each section radius of the blade is stored in the corresponding R parameter in the numerical control system;

[0012] Step S13, the machining coordinate system is translated and converted to drive the machining track corresponding to the section radius in the machining program to be machined according to the specified adjustment value.

[0013] Optionally, step S13 comprises:

[0014] Step S131, the automatic conversion is realized through the valuation of the frame variable, and the adjustment of each section radius of the blade is only reflected in the change of the Z axis direction in the workpiece coordinate system, so the Z axis of the frame variable is valued to complete the coordinate system translation conversion;

[0015] Step S132, the reference zero point coordinate system of the workpiece is kept as the reference of the workpiece machining without being changed, a frame specially used for coordinate system translation conversion is specified according to the settable frame use condition in the numerical control system;

[0016] Step S133, the reference zero point coordinate system data of the workpiece in the numerical control system and the adjustment value in the R parameter are calculated and then valued in the specified frame, so that the machining track corresponding to the section radius in the machining program is driven to be machined according to the adjustment value specified in the R parameter in the form of coordinate system translation conversion;

[0017] Step S134, the position data of the Z axis in the reference zero point coordinate system G54 of the workpiece is read through the frame variable instruction $P_UIFR[1,Z,FI].

[0018] Optionally, step S13 further comprises:

[0019] Step S135, after the calculation of the Z axis data and the adjustment data in the R parameter, the calculation result is written into the Z axis data in the G509 specially used for coordinate conversion through the frame variable instruction $P_UIFR[9,Z,FI].

[0020] Step S136, running G509 instruction, the numerical control system will read the converted coordinate system data, at this time the completion of the coordinate system translation conversion function, the height of the subsequent machining tool path will be based on the position data of Z axis in G54, according to the adjustment value in R parameter for processing.

[0021] Optionally, step S2 comprises:

[0022] Step S21, the axial adjustment value of the machining tool path corresponding to the blade section radius is set as a parameter, and then the relative radius value of each machining tool path in the machining program to the blade is calculated in the post-processing program, and a unique R parameter is configured, and the relative radius value of all machining tool paths to the blade and the configured R parameter are recorded according to the machining order;

[0023] Step S22, the tool path source file contains the coordinate points (x, y, z) of the tool running track, and the coordinate value of the tool running is behind the "GOTO" instruction in the file, and the actual radius value of the machining tool path relative to the hub center can be calculated through the coordinate value;

[0024] Step S23, the machining tool path in the blade machining program can be divided into two types according to the different positions on the blade, one is located on the designed section radius of the blade, and the other is located between the designed section radii. The machining tool path located on the section radius can be adjusted according to the adjustment value specified for the corresponding section radius, while the machining tool path located between the section radii does not have a specified adjustment value. In order to ensure that the area between the section radii can still process a smooth surface, the adjustment value of the machining tool path in the area between the section radii needs to be calculated according to a certain algorithm.

[0025] Step S24, a special frame for coordinate system translation conversion is specified, which is used to complete the calculation of the reference zero point coordinate system of the workpiece and the different adjustment values in the R parameter. Each machining tool path reads the data in this special frame before machining, and performs coordinate system translation according to different adjustment values to automatically adjust the machining tool path to the expected adjustment value for machining.

[0026] Optionally, step S22 comprises:

[0027] Step S221, the machining tool path relative to the blade radius = the actual radius value of the machining tool path ÷ the radius value of the blade;

[0028] Wherein, the actual radius value of the machining tool path is directly calculated through the coordinate points in the tool path source file, and the radius of the blade needs to be input into the post-processing program according to the data in the design drawing. The radius value of the blade will directly affect the calculated machining tool path relative to the blade radius;

[0029] Step S222, after the machining tool path relative to the blade radius value is calculated, each machining tool path is configured with a unique corresponding R parameter according to the machining sequence, and in the post-processing constructor, these information can be uniformly stored in the form of a list by establishing a list through TCL language. The relative blade section radius value and the corresponding R parameter of the machining tool path can be searched out through the operation command of the list, and the blade design section radius value and the corresponding R parameter in the machining program are listed in the program header for use;

[0030] Step S223, record all machining tool path relative to the blade radius value and the corresponding R parameter, and the recorded results will be saved in the background in the form of a list. By searching the information in the list through the command, the R parameter corresponding to the design section radius of the blade can be found out, and these design section radius and the corresponding R parameter can be listed in the generated machining program header.

[0031] Optionally, step S23 includes:

[0032] Step S231, the method for estimating the function value of other unknown points by using linear interpolation method, the calculation formula is as follows:

[0033] ;

[0034] Wherein, Y is the value corresponding to the unknown data point to be estimated, and the X value of the point is a known value, X1 and Y1 are the first known data point, and X2 and Y2 are the second known data point;

[0035] When processing the adjustment value of the machining tool path in the region between the design section radius, the linear interpolation algorithm is used for calculation, the radius value and the axial adjustment value of the machining tool path are taken as a data point, and the radius value and the axial adjustment value of the two adjacent machining tool paths located on the design section radius are the known data points. The adjustment value of a machining tool path in the region between the design section radius can be calculated, and the calculation formula is as follows:

[0036] ;

[0037] Wherein, C is the adjustment value of a certain machining tool path to be calculated, the distance between the machining tool path and one of the adjacent section radius is H1, the adjustment value of this section radius is A, and the distance between the machining tool path and the other adjacent section radius is H2, the adjustment value of this section radius is B;

[0038] Step S232, first calculate the relative blade radius value of the machining tool path through the coordinate points in the tool path source file. If the machining tool path is located on the design section radius, directly use the adjustment value of the section radius. If the machining tool path is located between two design section radii, use the distance and adjustment value of the adjacent two design section radii as known data to calculate the adjustment value of a certain machining tool path according to the linear interpolation method. The transmission and calculation of the adjustment value are completed through the R parameter corresponding to the machining tool path.

[0039] The adjustment value of the machining tool path in the region between the blade section radii is the expression in which the R parameter participates in the calculation, which is embodied in the machining program. The Siemens numerical control system will calculate the adjustment value of each machining tool path according to the expression and save it in the unique R parameter.

[0040] Optionally, step S24 includes:

[0041] Step S241, according to the use of the frame set by the numerical control system, specify a frame dedicated to coordinate system translation conversion, and write the data in the reference zero point coordinate system of the workpiece into the frame dedicated to coordinate system translation conversion through the assignment instruction of the numerical control system;

[0042] Step S242, before running each machining tool path, the data in the dedicated frame need to be calculated and then read. In the machining program generated by the post-processing program, combined with the adjustment value saved in the R parameter and the data of the Z axis in the reference coordinate system, the data in the Z axis direction of the dedicated frame is calculated first, and then the data of the dedicated frame is read to complete the coordinate system translation.

[0043] Optionally, step S3 includes:

[0044] Step S31, in the machining module of Siemens NX software, use the variable profile milling method to generate five-axis milling machining tracks, take the blade surface as the cutting part, and use the section radius line of the blade surface as the driving line to generate the track line along the section radius direction of the blade;

[0045] Step S32, in Siemens NX software, take the theoretical design model of the blade as the cutting part, generate machining tracks along the section radius direction of the blade, generate the standard parameterized machining program of this type of blade, and need to be verified by simulation machining;

[0046] Step S33, according to the analysis of the blade blank data, the adjustment value of each section radius of the blade can be obtained. Modify the R parameter data corresponding to the section radius in the program header of the standard parameterized machining program of this type of blade, and the machining program can be compiled and directly used for machine tool machining.

[0047] Optionally, the step S1 further comprises a step S0 of analyzing a currently used propeller blade programming method and analyzing repetitive work.

[0048] The technical scheme provided by the embodiment of the present disclosure can include the following beneficial effects:

[0049] (1) The present scheme establishes a one-to-one correspondence between the design cross-sectional radius of the marine propeller blade and the machining track in the machining program, parameterizes the axial adjustment value of the machining track in the machining program, calculates the adjustment height of the regional machining track between the cross-sectional radii by linear interpolation, and drives the machining track to be machined according to the expected adjustment value through coordinate system translation conversion, thereby finally compiling a parameterized blade machining program.

[0050] (2) The parameterized numerical control machining program in the present scheme can avoid a large amount of repetitive work actually existing in the programming link of the propeller blade, and only needs to modify the adjustment value of each cross-sectional radius in the compiled parameterized program to complete the compilation of the blade machining program, thereby greatly improving the programming efficiency. BRIEF DESCRIPTION OF DRAWINGS

[0051] Figure 1 is a structural schematic diagram of a marine propeller according to an exemplary embodiment of the present disclosure.

[0052] Figure 2 is a marine propeller machining adjustment schematic diagram according to an exemplary embodiment of the present disclosure Figure One .

[0053] Figure 3 is a marine propeller machining adjustment schematic diagram according to an exemplary embodiment of the present disclosure Figure Two .

[0054] Figure 4 is an adjustment schematic diagram of a cross-sectional radius in a marine propeller blade parameterized numerical control machining program compilation method according to an exemplary embodiment of the present disclosure.

[0055] Figure 5 is a track line in a cross-sectional radius direction machining in a marine propeller blade parameterized numerical control machining program compilation method according to an exemplary embodiment of the present disclosure.

[0056] Figure 6 is an instruction diagram of machine tool machining in a marine propeller blade parameterized numerical control machining program compilation method according to an exemplary embodiment of the present disclosure.

[0057] Figure 7 is a flowchart of a marine propeller blade parameterized numerical control machining program compilation method according to an exemplary embodiment of the present disclosure Figure One .

[0058] Figure 8 is a flowchart of a method for preparing a parameterized numerical control machining program of a propeller blade of a ship according to an exemplary embodiment of the present disclosure Figure Two . DETAILED DESCRIPTION

[0059] The specific embodiments of the present disclosure will be described below in detail with reference to the accompanying drawings. It should be understood that the specific embodiments described herein are merely intended to illustrate and explain the present disclosure, and are not intended to limit the present disclosure.

[0060] In the present disclosure, the orientation words such as "up, down, front, back, left, right" are used for the convenience of description defined according to the drawing direction of the corresponding drawing, and "inner, outer" are defined according to the contour of the corresponding part itself. The terms such as "first, second" used in the present disclosure are used to distinguish one element from another element, and do not have sequentiality and importance. In addition, when the following description refers to the drawings, the same numbers in different drawings represent the same or similar elements unless otherwise indicated.

[0061] The present scheme aims at the problem of low efficiency of machining program preparation caused by a large amount of repetitive work in the process of numerical control machining program preparation of the propeller blade of a ship. Based on the in-depth analysis of the manufacturing tolerance of the propeller of a ship (ISO484), by integrating the programming technology of Siemens NX software, the post-processing program development technology and the advanced programming technology of Siemens numerical control system, the axial position value parameterization of the blade section radius in the machining program (i.e. the axial direction of the hub) is taken as the breakthrough point, a method for preparing a parameterized machining program of the propeller blade of a ship is researched, and a set of machine tool post-processing program capable of generating a parameterized machining program is developed in Siemens NX software. By directly modifying the axial position parameter of the blade section radius in the machining program, the preparation of different blade machining programs of the same type of propeller of a ship can be quickly completed, a large amount of repetitive work can be avoided in the process of blade machining program preparation, and the purpose of improving the programming efficiency of the propeller blade of a ship is finally achieved.

[0062] (1) The method for preparing a parameterized machining program in the present scheme can be applied to the machining of spatial curved surfaces similar to the surface of the propeller blade of a ship. Through this way, the preparation of the machining program can be quickly completed.

[0063] (2) The method for preparing a parameterized post-processing program in the present scheme completed in Siemens NX can also be applied to the post-processing preparation process of other CAM (Computer Aided Manufacturing) software.

[0064] (3) The method of machining tool path coordinate system translation in the Siemens CNC system in this scheme can also be applied to other CNC systems.

[0065] Referring to Figures 1 to 8 The method for preparing a parameterized numerical control machining program of a marine propeller blade provided by the embodiment of the present disclosure comprises the following steps:

[0066] Step S1: coordinate system translation is used to drive the tool path.

[0067] Step S2: the development of a post-processing program is completed in the Post Builder of the Siemens NX, TCL language is used as the command language thereof, the kinematic model of the numerical control machine tool uses the original algorithm, the height position adjustment value of the machining tool path in the machining program is parameterized and assigned, the machining coordinate system is automatically translated and converted, and the height adjustment value of the machining tool path in the region between the cross-sectional radii is calculated and assigned.

[0068] Step S3: the tool machining path is generated in the Siemens NX software according to the direction of the blade cross-sectional radius, the post-processing program is converted into a numerical control machining program, and the cross-sections that need to be adjusted are directly modified in the parameterized machining program according to the analysis of the blade blank.

[0069] It can be understood that the Siemens NX (formerly Unigraphics) is an integrated CAD / CAE / CAM digital product development system developed by Siemens PLM Software, which covers the whole life cycle from product conceptual design, engineering simulation to manufacturing. (1) The present scheme establishes a one-to-one correspondence between the design cross-sectional radius of the marine propeller blade and the machining path in the machining program, parameterizes the axial adjustment value of the machining path in the machining program, calculates the adjustment height of the machining path in the region between the cross-sectional radii by using the linear interpolation method, drives the machining path to be machined according to the expected adjustment value through coordinate system translation conversion, and finally prepares a parameterized blade machining program.

[0070] (2) The parameterized numerical control machining program in the present scheme can avoid a large amount of repetitive work actually existing in the programming link of the propeller blade, and only needs to modify the adjustment values of the cross-sectional radii in the prepared parameterized program to complete the preparation of the blade machining program, thereby greatly improving the programming efficiency.

[0071] In an embodiment, step S1 comprises the following steps:

[0072] Step S11: the axial position adjustment value of the blade cross-sectional radius is received through calculation of the R parameter, the machining program of the standard blade is generated without adjustment of the cross-sectional radius position, so the adjustment value of each cross-sectional radius is 0, and the R parameter corresponding to the cross-sectional radius is assigned as 0.

[0073] Step S12, if it is necessary to adjust the radius of a certain section, directly assign the R parameter corresponding to the radius of the section, at this time the adjustment value of each section radius of the blade has been stored in the corresponding R parameter in the numerical control system;

[0074] Step S13, the machining coordinate system is translated and converted to drive the machining trajectory corresponding to the radius of the section in the machining program to process according to the specified adjustment value.

[0075] In an embodiment, step S13 includes:

[0076] Step S131, automatic conversion is realized by assigning the frame variable, and the adjustment of each section radius of the blade only reflects the change in the Z axis direction in the workpiece coordinate system, so assigning the Z axis of the frame variable can complete the coordinate system translation conversion;

[0077] Step S132, the reference zero point coordinate system of the workpiece is kept as the reference for workpiece machining without being changed, and a frame specially used for coordinate system translation conversion is specified according to the frame usage that can be set in the numerical control system;

[0078] Step S133, the reference zero point coordinate system data of the workpiece in the numerical control system and the adjustment value in the R parameter are calculated and then assigned to the specified frame, so that the machining tool path corresponding to the radius of the section in the machining program is driven to process according to the adjustment value specified in the R parameter in the form of coordinate system translation conversion;

[0079] Step S134, the position data of the Z axis in the reference zero point coordinate system G54 of the workpiece is read through the frame variable instruction $P_UIFR[1,Z,FI].

[0080] In an embodiment, step S13 further includes:

[0081] Step S135, after the Z axis data and the adjustment data in the R parameter are calculated, the calculation result is written into the Z axis data in the G509 specially used for coordinate conversion through the frame variable instruction $P_UIFR[9,Z,FI];

[0082] Step S136, the G509 instruction is run, and the numerical control system will read the converted coordinate system data, at this time the translation conversion function of the coordinate system is completed, and the height of the subsequent machining tool path will be processed according to the adjustment value in the R parameter based on the position data of the Z axis in the G54.

[0083] In an embodiment, step S2 includes:

[0084] Step S21, after setting the axial adjustment value of the machining tool path corresponding to the blade section radius as a parameter, the relative radius value of each machining tool path to the blade is calculated in the post-processing program, and a unique corresponding R parameter is configured, and the relative radius value of all machining tool paths to the blade and the configured R parameter are recorded in the order of machining;

[0085] Step S22, the tool path source file contains the coordinate points (x, y, z) of the tool running track, and the coordinate value of the tool running is behind the "GOTO" instruction in the file. The actual radius value of the machining tool path relative to the hub center can be calculated through the coordinate value;

[0086] Step S23, the machining tool paths in the blade machining program can be divided into two types according to the different positions on the blade. One is located on the designed section radius of the blade, and the other is located between the designed section radii. The machining tool path located on the section radius can be adjusted according to the adjustment value specified for the corresponding section radius, while the machining tool path located between the section radii does not have a specified adjustment value. In order to ensure that the area between the section radii can still process a smooth surface, the adjustment value of the machining tool path in the area between the section radii needs to be calculated according to a certain algorithm.

[0087] Step S24, a frame specially used for coordinate system translation conversion is specified, which is used to calculate the reference zero point coordinate system of the workpiece and the different adjustment values in the R parameter. Each machining tool path reads the data in this special frame before machining, and performs coordinate system translation conversion according to different adjustment values to realize automatic adjustment of different machining tool paths to the expected adjustment value for machining.

[0088] In an embodiment, step S22 includes:

[0089] Step S221, the relative radius of the machining tool path to the blade = the actual radius value of the machining tool path ÷ the radius value of the blade;

[0090] Wherein, the actual radius value of the machining tool path is directly calculated through the coordinate points in the tool path source file, and the radius of the blade needs to be input into the post-processing program according to the data in the design drawing. The radius value of the blade will directly affect the calculated relative radius of the machining tool path to the blade;

[0091] Step S222, after the relative radius value of the machining tool path to the blade is calculated, a unique corresponding R parameter is configured for each machining tool path according to the order of machining. In the post-processing constructor, these information can be stored uniformly through the list established by TCL language. Through the operation command of the list, the relative radius value of the machining tool path to the blade and the corresponding R parameter can be searched out, and the blade design section radius value and the corresponding R parameter in the machining program are listed in the program header for use.

[0092] Step S223, record all processing cutter track relative to the blade radius value and the corresponding R parameter, record the results will be in the form of a list saved in the background, through the command to retrieve the list of information, you can find the blade design cross-sectional radius corresponding to the R parameter, in the generated processing program header can be listed these design cross-sectional radius and the corresponding R parameter.

[0093] In an embodiment, step S23 includes:

[0094] Step S231, using linear interpolation method to estimate the function value of other unknown points, the formula is as follows:

[0095] ;

[0096] Wherein, Y is to be estimated unknown data point corresponding value, and the point of X value is known value, X1 and Y1 is the first known data point, X2 and Y2 is the second known data point;

[0097] In the processing of the adjustment value of the processing cutter track located between the design cross-sectional radius, according to the linear interpolation algorithm for calculation, the radius value and axial adjustment value of the processing cutter track as a data point, the adjacent two located on the design cross-sectional radius of the processing cutter track radius value and axial adjustment value is the known data point, can calculate the adjustment value of a processing cutter track between the design cross-sectional radius, the formula is as follows:

[0098] ;

[0099] Wherein, C is to calculate the adjustment value of a processing cutter track, the distance between the processing cutter track and one of the adjacent cross-sectional radius is H1, the adjustment value of this cross-sectional radius is A, the distance between the processing cutter track and the other adjacent cross-sectional radius is H2, the adjustment value of this cross-sectional radius is B, see the following Figure 4 ;

[0100] Step S232, first calculate the relative blade radius value of the processing cutter track through the coordinate point in the cutter location track source file, if the processing cutter track is located on the design cross-sectional radius, directly use the adjustment value of this cross-sectional radius; if the processing cutter track is located between two design cross-sectional radius, the distance and adjustment value of the adjacent two design cross-sectional radius as the known data, according to the linear interpolation method to calculate the adjustment value of a processing cutter track, the adjustment value of the transmission and calculation is completed through the corresponding R parameter of the processing cutter track;

[0101] The adjustment value of the machining tool path of the region between the blade section radii is expressed in the machining program by the R parameter participating in the calculation, and the Siemens numerical control system calculates the adjustment value of each machining tool path according to the expression and saves it in the unique R parameter.

[0102] In an embodiment, the step S24 comprises:

[0103] In step S241, a frame dedicated to coordinate system translation conversion is specified according to the use of the numerical control system, and data in the reference zero point coordinate system of the workpiece is written into the frame dedicated to coordinate system translation conversion through the assignment instruction of the numerical control system.

[0104] In step S242, the data in the dedicated frame needs to be calculated before running each machining tool path, and then read. In the machining program generated by the post-processing program, the adjustment value saved in the R parameter and the data of the Z axis in the reference coordinate system are combined to calculate the data in the Z axis direction of the dedicated frame first, and then read the data of the dedicated frame to complete the coordinate system translation.

[0105] In an embodiment, the step S3 comprises:

[0106] In step S31, the variable profile milling method is used under the machining module of the Siemens NX software to generate a five-axis milling machining path, the blade surface is taken as the cutting component, and the section radius line of the blade surface is taken as the driving line to generate a track line along the section radius direction of the blade. See the following Figure 5 ;

[0107] In step S32, the theoretical design model of the blade is taken as the cutting component in the Siemens NX software to generate a machining path along the section radius direction of the blade, generate a standard parameterized machining program of this type of blade, and need to be verified by simulation machining.

[0108] In step S33, according to the analysis of the blade blank data, the adjustment value of each section radius of the blade can be obtained, and the R parameter data corresponding to the section radius is modified in the program header of the standard parameterized machining program of this type of blade, so that the machining program is compiled and directly used for machine tool machining. See the following Figure 6 The R parameters corresponding to the section radii of 0.3R to 0.8R are listed in the machining program header, and the axial adjustment value of the 0.8R section radius is in the R100 parameter. If the 0.8R section radius needs to be adjusted by 5mm along the axial position, the R100 parameter is directly assigned to 5.

[0109] In an embodiment, the step S1 further comprises a step S0 before the step S1, and the step S0 comprises: analyzing the currently used propeller blade programming method and analyzing the repetitive work.

[0110] Marine propeller is usually 4 to 6 blades evenly connected around the hub. The surface of the blade is a complex spatial surface connected by a set of spatial curves. The set of spatial curves that constitute the blade is divided into different cross-sectional radii according to the position of the entire blade radius, generally including the following design cross-sectional radii (referred to as cross-sectional radius) in the drawing: 1.0R, 0.975R, 0.95R, 0.9R, 0.8R, 0.7R, 0.6R, 0.5R, 0.4R, 0.3R, 0.25R, 0.2R. See the following Figure 1 .

[0111] Existing numerical control processing program preparation method of blade

[0112] The existing numerical control processing program preparation method of the blade is usually to analyze the blade blank data according to the manufacturing tolerance (ISO484) of the blade, then to rebuild the three-dimensional model of the blade in the Siemens NX software and to regenerate the processing program according to the analysis result of the blade blank, and finally to simulate the processing verification of the processing program in the simulation software.

[0113] Analysis of blade blank and use of manufacturing tolerance

[0114] The surface shape of the marine propeller blade is complex, and the blade is a cantilever structure. The blade is affected by various deformation factors during casting, so the shape of the blade blank formed by casting is difficult to keep consistent with the theoretical blade shape. In order to ensure that each part of the outer surface of the blade has a margin for processing, it is usually necessary to adjust the shape of the blade according to the requirements of the marine propeller manufacturing tolerance (ISO484), and the commonly used adjustment method is to adjust the axial (i.e. the axis direction of the hub, see Figure 1 ) position value of the cross-sectional radius of the blade. When analyzing the data of the blade blank, if the measured cross-sectional radius of the blank shape can completely wrap the theoretical shape of the cross-sectional radius, that is, there is enough margin for processing, the axial position value of the cross-sectional radius does not need to be adjusted, otherwise the axial position value of the cross-sectional radius needs to be adjusted until the cross-sectional radius of the blank shape can completely wrap the theoretical shape of the cross-sectional radius. See the following Figure 2 , the thick line is the cross-sectional radius of the blank shape, the thin line is the theoretical shape of the cross-sectional radius, figure A does not need to adjust the axial position value of the cross-sectional radius, figure B needs to adjust the axial position value of the cross-sectional radius.

[0115] Reconstruction of blade model

[0116] When measuring the data of the blade blank, the shape data of each cross-sectional radius of the blade is usually measured, and then the blade blank data is analyzed, that is, a comparative analysis process of the blank shape and the theoretical shape of the cross-sectional radius. Within the requirements of the marine propeller manufacturing tolerance (ISO484), it is ensured that there is sufficient allowance for processing at each part of the cross-sectional radius surface, and finally the axial position adjustment value of each cross-sectional radius is analyzed. According to these adjustment values, the position of each cross-sectional radius is adjusted in the Siemens NX software, and the blade model for processing is reconstructed according to the adjusted cross-sectional radius. See the following Figure 3 .

[0117] Generation of blade processing program

[0118] The blade processing program is completed in the processing module environment of the Siemens NX software. In the multi-axis milling state, the processing tool relies on the blade surface as the driving surface to complete the editing of the processing tool path, and at the same time, the tool path source file can be generated. The post-processing program matched with the machine tool converts the tool path source file, and finally generates the blade processing program that can be recognized by the machine tool numerical control system.

[0119] Simulation inspection of blade processing program

[0120] The blade processing program generated by the post-processing program is a five-axis linkage processing program, which cannot be directly read by artificial to judge the safety and correctness of the processing program. The safety and correctness of the processing program must be verified by simulation processing in professional numerical control machining simulation software. First, the virtual machine tool processing environment is constructed according to the actual numerical control machine tool structure, machine tool numerical control system, processing tool and processing workpiece, and then the blade processing program is called for simulation and simulation processing, which is used to verify whether the collision occurs between the numerical control machine tool and the workpiece, and whether the shape of the processed blade is accurate. Only the processing program that passes the simulation verification can be transmitted to the numerical control machine tool for actual processing, otherwise the processing program needs to be modified and improved in the Siemens NX software, and the modified processing program needs to be simulated and processed again until the processing program passes the simulation verification.

[0121] In the Siemens NX software, the processing tool path can be generated according to the direction of the blade cross-sectional radius. Through the one-to-one correspondence between the blade cross-sectional radius and the processing tool path in the processing program, the axial position adjustment value of the blade cross-sectional radius is kept consistent with the axial position adjustment value of the corresponding processing tool path in the processing program, and finally the axial adjustment value of the processing tool path corresponding to the blade cross-sectional radius in the processing program is determined as a modifiable parameter. According to the analysis results of the blade blank, only the adjustment parameter of the processing tool path corresponding to the blade cross-sectional radius in the processing program needs to be directly modified, and the blade processing program can be compiled.

[0122] The present application is described by way of examples, and it is to be understood that various alterations and / or equivalents can be apparent to those skilled in the art without departing from the spirit and scope of the present application. In addition, it is to be understood that the features and embodiments described herein can be modified to adapt to specific situations and materials without departing from the spirit and scope of the present application. Therefore, the present application is not limited to the specific embodiments disclosed herein, and all embodiments falling within the scope of the claims of the present application are to be included in the scope of the present application.

Claims

1. A method for compiling a parametric CNC machining program for marine propeller blades, characterized in that, include: Step S1: The coordinate system is translated to drive the toolpath; Step S2: After completing the development of the post-processor program in the Post Builder of Siemens NX, TCL language is used as its command language. The kinematic model of the CNC machine tool uses the original algorithm to parameterize the height position adjustment value of the machining toolpath in the machining program, automatically translate the machining coordinate system, and calculate and assign the height adjustment value of the machining toolpath in the area between the cross-sectional radii. Step S3: In Siemens NX software, a tool machining trajectory is generated according to the radius direction of the blade section. The post-processing program is used to convert it into a CNC machining program. Based on the analysis of the blade blank, the cross section that needs to be adjusted is directly modified in the parametric machining program.

2. The method for compiling a parametric CNC machining program for marine propeller blades according to claim 1, characterized in that, Step S1 includes: Step S11: Calculate the axial position adjustment value of the blade section radius by receiving the R parameter. The machining program generated by the standard blade does not adjust the position of the section radius, so the adjustment value of each section radius is 0, and the R parameter of the corresponding section radius is assigned to 0. Step S12: If it is necessary to adjust the position of a certain cross-section radius, the R parameter of the corresponding cross-section radius is directly assigned a value. At this time, the adjustment values ​​of each cross-section radius of the blade have been stored in the corresponding R parameter in the CNC system. Step S13: Transform the machining coordinate system by translation to drive the machining trajectory corresponding to the cross-sectional radius in the machining program to perform machining according to the specified adjustment value.

3. The method for compiling a parametric CNC machining program for marine propeller blades according to claim 2, characterized in that, Step S13 includes: Step S131: Automatic conversion is achieved by assigning values ​​to the frame variables. The adjustment of the radius of each section of the blade is only reflected in the change of the Z-axis in the workpiece coordinate system. Therefore, the coordinate system translation conversion can be completed by assigning values ​​to the Z-axis of the frame variables. Step S132: Keep the workpiece's reference zero coordinate system as the reference for workpiece machining without changing it, and specify a frame specifically for coordinate system translation transformation according to the frame usage that can be set in the CNC system. Step S133: Calculate the reference zero point coordinate system data of the workpiece in the CNC system together with the adjustment value in the R parameter and then assign it to the specified frame. Drive the machining tool path corresponding to the cross section radius in the machining program to perform machining according to the adjustment value specified in the R parameter by means of coordinate system translation transformation. Step S134: Read the Z-axis position data stored in the workpiece's reference zero-point coordinate system G54 through the frame variable instruction $P_UIFR[1, Z, FI].

4. The method for compiling a parametric CNC machining program for marine propeller blades according to claim 2, characterized in that, Step S13 also includes: Step S135: After calculating the Z-axis data and the adjustment data in the R parameter, the calculation result is written into the Z-axis data in the G509 specifically used for coordinate transformation through the frame variable instruction $P_UIFR[9, Z, FI]. In step S136, the G509 command is executed, and the CNC system will read the converted coordinate system data. At this time, the coordinate system translation conversion function is completed. The height of the subsequent machining toolpath will be based on the Z-axis position data in G54 and the machining will be performed according to the adjustment value in the R parameter.

5. The method for compiling a parametric CNC machining program for marine propeller blades according to claim 2, characterized in that, Step S2 includes: Step S21: After setting the axial adjustment value of the machining toolpath corresponding to the blade section radius as a parameter, calculate the radius value of each machining toolpath relative to the blade in the post-processing program, and configure a unique corresponding R parameter. At the same time, record the radius values ​​of all machining toolpaths relative to the blade and the configured R parameters in the machining order. Step S22: The tool path source file contains the coordinates (x, y, z) of the tool path. The coordinates of the tool path are after the "GOTO" command in the file. The actual radius of the machining tool path relative to the center of the hub can be calculated using these coordinates. Step S23: The machining toolpaths in the blade machining program can be divided into two types according to their position on the blade. One type is located exactly on the design cross-sectional radius of the blade, and the other type is located between the design cross-sectional radii. The machining toolpaths located on the cross-sectional radius can be adjusted according to the adjustment value specified for the corresponding cross-sectional radius. However, the machining toolpaths located in the area between the cross-sectional radii do not have a specified adjustment value. In order to ensure that the area between the cross-sectional radii can still be machined into a smooth surface, it is necessary to calculate the adjustment value of the machining toolpaths in the area between the cross-sectional radii according to a certain algorithm. Step S24: Specify a frame specifically for coordinate system translation transformation. This frame is used to calculate the reference zero point coordinate system of the workpiece and different adjustment values ​​in the R parameter. Before machining, each machining toolpath reads the data in this special frame and performs coordinate system translation transformation according to different adjustment values, so as to realize that different machining toolpaths are automatically adjusted to the expected adjustment values ​​for machining.

6. The method for compiling a parametric CNC machining program for marine propeller blades according to claim 5, characterized in that, Step S22 includes: Step S221, the relative radius of the machining toolpath to the blade = the actual radius of the machining toolpath ÷ the radius of the blade; The actual radius of the machining toolpath is calculated directly from the coordinates in the toolpath source file, while the blade radius needs to be input into the post-program based on the data in the design drawings. The blade radius value will directly affect the calculated machining toolpath relative to the blade radius. Step S222: After calculating the relative blade radius value of the machining toolpath, assign a unique corresponding R parameter to each machining toolpath according to the machining sequence. In the post-processor constructor, this information can be uniformly stored by creating a list using TCL language. The relative blade section radius value and corresponding R parameter of the machining toolpath can be searched by the operation command of the list. The blade design section radius value and corresponding R parameter in the machining program are listed in the program header for use. Step S223: Record the relative blade radius values ​​of all machining toolpaths and the corresponding R parameters. The recorded results will be saved in the background in the form of a list. By retrieving the information in the list by command, the R parameters corresponding to the design section radius of the blade can be found. These design section radii and corresponding R parameters can be listed in the generated machining program header.

7. The method for compiling a parametric CNC machining program for marine propeller blades according to claim 5, characterized in that, Step S23 includes: Step S231, using linear interpolation to estimate the function values ​​at other unknown points, the calculation formula is as follows: ； Where Y is the value corresponding to the unknown data point to be estimated, and the X value of the point is a known value, X1 and Y1 are the first known data points, and X2 and Y2 are the second known data points; When processing the adjustment value of machining toolpaths located within the design section radius, a linear interpolation algorithm is used for calculation. The radius value and axial adjustment value of the machining toolpath are taken as a data point. The radius values ​​and axial adjustment values ​​of two adjacent machining toolpaths located on the design section radius are known data points. Thus, the adjustment value of a certain machining toolpath within the design section radius can be calculated, resulting in the following calculation formula: ； Where C is the adjustment value of a certain machining toolpath to be calculated, the adjustment value of the toolpath at a distance of H1 from one of its adjacent cross-sections is A, and the adjustment value of the toolpath at a distance of H2 from another adjacent cross-section is B. Step S232: First, the relative blade radius value of the machining toolpath is calculated using the coordinate points in the toolpath source file. If the machining toolpath is exactly located on the design section radius, the adjustment value of this section radius is used directly. If the machining toolpath is located between two design section radii, the distance and adjustment value of the two adjacent design section radii are used as known data, and the adjustment value of a certain machining toolpath is calculated using the linear interpolation method. The transfer and calculation of the adjustment value are completed through the R parameter corresponding to the machining toolpath. The adjustment value of the machining toolpath in the region between the blade cross-section radii is reflected in the machining program by an expression that involves the R parameter. The Siemens CNC system will calculate the adjustment value of each machining toolpath according to the expression and save it in the unique corresponding R parameter.

8. The method for compiling a parametric CNC machining program for marine propeller blades according to claim 6, characterized in that, Step S24 includes: Step S241: Based on the usage of the CNC system setting frame, specify a frame dedicated to coordinate system translation transformation, and write the data in the workpiece's reference zero coordinate system into the frame dedicated to coordinate system translation transformation through the assignment instructions of the CNC system. Step S242: Before running each machining toolpath, the data in the dedicated frame needs to be calculated and then read. In the machining program generated by the post-processor, the adjustment value saved in the R parameter and the Z-axis data in the reference coordinate system are combined to first calculate the data in the Z-axis direction of the dedicated frame, and then read the data of the dedicated frame to complete the coordinate system translation.

9. The method for compiling a parametric CNC machining program for marine propeller blades according to claim 5, characterized in that, Step S3 includes: Step S31: In the machining module of Siemens NX software, a five-axis milling machining trajectory is generated using variable profile milling. The blade surface is used as the cutting part, and the cross-sectional radius line of the blade surface is used as the driving line to generate a machining trajectory line along the cross-sectional radius direction of the blade. Step S32: In Siemens NX software, using the theoretical design model of the blade as the cutting component, generate the machining trajectory along the cross-sectional radius of the blade, generate the standard parametric machining program for this type of blade, and verify it through simulation machining. Step S33: Based on the analysis of the blade blank data, the adjustment value of the radius of each section of the blade can be obtained. The R parameter data corresponding to the section radius can be directly modified in the program header of the standard parametric machining program for this type of blade to complete the machining program compilation, which can be directly used for machine tool machining.

10. The method for compiling a parametric CNC machining program for marine propeller blades according to claim 1, characterized in that, Before step S1, there is also step S0, which involves analyzing the currently used propeller blade programming method and analyzing repetitive tasks.

Images