The processing technology of CNC machine tools has many similarities with that of general machine tools, but the process regulations for processing parts on CNC machine tools are much more complicated than those for processing parts on general machine tools. Before CNC processing, the movement process of the machine tool, the process of the parts, the shape of the tool, the cutting amount, the tool path, etc., must be programmed into the program, which requires the programmer to have a multi-faceted knowledge base. A qualified programmer is the first qualified process personnel. Otherwise, it will be impossible to fully and thoughtfully consider the entire process of part processing and correctly and reasonably compile the part processing program.
2.1 Main contents of CNC processing process design
When designing the CNC machining process, the following aspects should be carried out: selection of CNC machining process content, CNC machining process analysis, and design of CNC machining process route.
2.1.1 Selection of CNC machining process content
Not all processing processes are suitable for CNC machine tools, but only a part of the process content is suitable for CNC processing. This requires careful process analysis of the part drawings to select the content and processes that are most suitable and most needed for CNC processing. When considering the selection of content, it should be combined with the actual equipment of the enterprise, based on solving difficult problems, overcoming key problems, improving production efficiency, and giving full play to the advantages of CNC processing.
1. Content suitable for CNC processing
When selecting, the following order can generally be considered:
(1) Contents that cannot be processed by general-purpose machine tools should be given priority; (2) Contents that are difficult to process with general-purpose machine tools and whose quality is difficult to guarantee should be given priority; (3) Contents that are inefficient to process with general-purpose machine tools and require high manual labor intensity can be selected when CNC machine tools still have sufficient processing capacity.
2. Contents that are not suitable for CNC processing
Generally speaking, the above-mentioned processing contents will be significantly improved in terms of product quality, production efficiency, and comprehensive benefits after CNC processing. In contrast, the following contents are not suitable for CNC processing:
(1) Long machine adjustment time. For example, the first fine datum is processed by the rough datum of the blank, which requires the coordination of special tooling;
(2) The processing parts are scattered and need to be installed and set at the origin multiple times. In this case, it is very troublesome to use CNC processing, and the effect is not obvious. General machine tools can be arranged for supplementary processing;
(3) The profile of the surface is processed according to a certain specific manufacturing basis (such as templates, etc.). The main reason is that it is difficult to obtain data, which is easy to conflict with the inspection basis, increasing the difficulty of program compilation.
In addition, when selecting and deciding the processing content, we should also consider the production batch, production cycle, process turnover, etc. In short, we should try to be reasonable in achieving the goals of more, faster, better, and cheaper. We should prevent CNC machine tools from being downgraded to general-purpose machine tools.
2.1.2 Analysis of CNC machining process
The CNC machining processability of the processed parts involves a wide range of issues. The following is a combination of the possibility and convenience of programming. Some of the main contents that must be analyzed and reviewed are proposed.
1. Dimensioning should conform to the characteristics of CNC machining. In CNC programming, the dimensions and positions of all points, lines, and surfaces are based on the programming origin. Therefore, it is best to directly give the coordinate dimensions on the part drawing or try to use the same reference to annotate the dimensions.
2. The conditions of geometric elements should be complete and accurate.
In program compilation, programmers must fully understand the parameters of the geometric elements that constitute the part contour and the relationship between each geometric element. Because all geometric elements of the part contour must be defined during automatic programming, and the coordinates of each node must be calculated during manual programming. No matter which point is unclear or uncertain, programming cannot be carried out. However, due to the lack of consideration or neglect by the part designers during the design process, incomplete or unclear parameters often occur, such as whether the arc is tangent to the straight line or whether the arc is tangent to the arc or intersecting or separated. Therefore, when reviewing and analyzing the drawings, it is necessary to calculate carefully and contact the designer as soon as possible if problems are found.
3. The positioning reference is reliable
In CNC machining, the machining procedures are often concentrated, and positioning with the same reference is very important. Therefore, it is often necessary to set some auxiliary references or add some process bosses on the blank. For the part shown in Figure 2.1a, in order to increase the stability of positioning, a process boss can be added to the bottom surface, as shown in Figure 2.1b. It will be removed after the positioning process is completed.
4. Unified geometry and size:
It is best to use unified geometry and size for the shape and inner cavity of the parts, which can reduce the number of tool changes. Control programs or special programs may also be applied to shorten the program length. The shape of the parts should be as symmetrical as possible to facilitate programming using the mirror processing function of the CNC machine tool to save programming time.
2.1.3 Design of CNC Machining Process Route
The main difference between CNC machining process route design and general machine tool machining process route design is that it often does not refer to the entire process from blank to finished product, but only a specific description of the process of several CNC machining procedures. Therefore, in the process route design, it must be noted that since CNC machining procedures are generally interspersed in the entire process of part machining, they must be well connected with other machining processes.
The common process flow is shown in Figure 2.2.
The following issues should be noted in the design of the CNC machining process route:
1. Division of process
According to the characteristics of CNC machining, the division of the CNC machining process can generally be carried out in the following ways:
(1) One installation and processing is regarded as one process. This method is suitable for parts with less processing content, and they can reach the inspection state after processing. (2) Divide the process by the content of the same tool processing. Although some parts can process many surfaces to be processed in one installation, considering that the program is too long, there will be certain restrictions, such as the limitation of the control system (mainly the memory capacity), the limitation of the continuous working time of the machine tool (such as a process cannot be completed within one work shift), etc. In addition, a program that is too long will increase the difficulty of error and retrieval. Therefore, the program should not be too long, and the content of one process should not be too much.
(3) Divide the process by the processing part. For workpieces with many processing contents, the processing part can be divided into several parts according to its structural characteristics, such as an inner cavity, outer shape, curved surface, or plane, and the processing of each part is regarded as one process.
(4) Divide the process by rough and fine processing. For workpieces that are prone to deformation after processing, since the deformation that may occur after rough processing needs to be corrected, generally speaking, the processes for rough and fine processing must be separated.
2. Sequence arrangement The sequence arrangement should be considered based on the structure of the parts and the condition of the blanks, as well as the needs of positioning, installation, and clamping. The sequence arrangement should generally be carried out according to the following principles:
(1) The processing of the previous process cannot affect the positioning and clamping of the next process, and the general machine tool processing processes interspersed in the middle should also be considered comprehensively;
(2) The inner cavity processing should be carried out first, and then the outer shape processing; (3) Processing processes with the same positioning and clamping method or with the same tool are best processed continuously to reduce the number of repeated positioning, tool changes, and platen movements;
3. The connection between CNC machining technology and ordinary processes.
CNC machining processes are usually interspersed with other ordinary machining processes before and after. If the connection is not good, conflicts are likely to occur. Therefore, while being familiar with the entire machining process, it is necessary to understand the technical requirements, machining purposes, and machining characteristics of CNC machining processes and ordinary machining processes, such as whether to leave machining allowances and how much to leave; the accuracy requirements and form and position tolerances of positioning surfaces and holes; the technical requirements for the shape correction process; the heat treatment status of the blank, etc. Only in this way can each process meet the machining needs, the quality goals and technical requirements be clear, and there be a basis for handover and acceptance.
2.2 CNC machining process design method
After selecting the CNC machining process content and determining the parts processing route, the CNC machining process design can be carried out. The main task of the CNC machining process design is to further determine the processing content, cutting amount, process equipment, positioning and clamping method, and tool movement trajectory of this process so as to prepare for the compilation of the machining program.
2.2.1 Determine the tool path and arrange the processing sequence
The tool path is the movement trajectory of the tool in the entire processing process. It not only includes the content of the work step but also reflects the order of the work step. The tool path is one of the bases for writing programs. The following points should be noted when determining the tool path:
1. Seek the shortest processing route, such as the hole system on the part shown in the processing figure 2.3a. The tool path of Figure 2.3b is to process the outer circle hole first and then the inner circle hole. If the tool path of Figure 2.3c is used instead, the idle tool time is reduced, and the positioning time can be saved by nearly half, which improves processing efficiency.
2. The final contour is completed in one pass
In order to ensure the roughness requirements of the workpiece contour surface after machining, the final contour should be arranged to be continuously machined in the last pass.
As shown in Figure 2.4a, the tool path for machining the inner cavity by line cutting, this tool path can remove all the excess in the inner cavity, leaving no dead angle and no damage to the contour. However, the line-cutting method will leave a residual height between the starting point and the endpoint of the two passes, and the required surface roughness cannot be achieved. Therefore, if the tool path of Figure 2.4b is adopted, the line-cutting method is used first, and then a circumferential cut is made to smooth the contour surface, which can achieve better results. Figure 2.4c is also a better tool path method.
3. Select the direction of entry and exit
When considering the tool's entry and exit (cutting in and out) routes, the tool's cutting out or entry point should be on the tangent along the part contour to ensure a smooth workpiece contour; avoid scratching the workpiece surface by cutting vertically up and down on the workpiece contour surface; minimize pauses during contour machining (elastic deformation caused by sudden changes in cutting force) to avoid leaving tool marks, as shown in Figure 2.5.
Figure 2.5 Extension of the tool when cutting in and out
4. Choose a route that minimizes the deformation of the workpiece after processing
For slender parts or thin plate parts with small cross-sectional areas, the tool path should be arranged by machining to the final size in several passes or by symmetrically removing the allowance. When arranging the work steps, the work steps that cause less damage to the rigidity of the workpiece should be arranged first.
2.2.2 Determine the positioning and clamping solution
When determining the positioning and clamping scheme, the following issues should be noted:
(1) Try to unify the design basis, process basis, and programming calculation basis as much as possible; (2) Try to concentrate the processes, reduce the number of clamping times, and process all the surfaces to be processed in
One clamping as much as possible ; (3) Avoid using clamping schemes that take up a long time for manual adjustment ;
(4) The point of action of the clamping force should fall on the part with better rigidity of the workpiece.
As shown in Figure 2.6a, the axial rigidity of the thin-walled sleeve is better than the radial rigidity. When the clamping claw is used for radial clamping, the workpiece will deform greatly. If the clamping force is applied along the axial direction, the deformation will be much smaller. When clamping the thin-walled box shown in Figure 2.6b, the clamping force should not act on the top surface of the box but on the convex edge with better rigidity or change to three-point clamping on the top surface to change the position of the force point to reduce the clamping deformation, as shown in Figure 2.6c.
Figure 2.6 Relationship between clamping force application point and clamping deformation
2.2.3 Determine the relative position of the tool and the workpiece
For CNC machine tools, it is very important to determine the relative position of the tool and the workpiece at the beginning of processing. This relative position is achieved by confirming the tool setting point. The tool setting point refers to the reference point for determining the relative position of the tool and the workpiece through tool setting. The tool setting point can be set on the part being processed or on a position on the fixture that has a certain size relationship with the part positioning reference. The tool setting point is often selected at the processing origin of the part. The selection principles
Of the tool setting point are as follows: (1) The selected tool setting point should make the program compilation simple;
(2) The tool setting point should be selected at a position that is easy to align and convenient to determine the processing origin of the part;
(3) The tool setting point should be selected at a position that is convenient and reliable to check during processing;
(4) The selection of the tool setting point should be conducive to improving the processing accuracy.
For example, when processing the part shown in Figure 2.7, when compiling the CNC processing program according to the illustrated route, select the intersection of the center line of the cylindrical pin of the fixture positioning element and the positioning plane A as the processing tool setting point. Obviously, the tool setting point here is also the processing origin.
When using the tool setting point to determine the machining origin, "tool setting" is required. The so-called tool setting refers to the operation of making the "tool position point" coincide with the "tool setting point." The radius and length dimensions of each tool are different. After the tool is installed on the machine tool, the basic position of the tool should be set in the control system. The "tool position point" refers to the positioning reference point of the tool. As shown in Figure 2.8, the tool position point of a cylindrical milling cutter is the intersection of the tool center line and the bottom surface of the tool; the tool position point of a ball-end milling cutter is the center point of the ball head or the vertex of the ball head; the tool position point of a turning tool is the tooltip or the center of the tooltip arc; the tool position point of a drill is the vertex of the drill. The tool setting methods of various types of CNC machine tools are not exactly the same, and this content will be discussed separately in conjunction with various types of machine tools.
Tool change points are set for machine tools such as machining centers and CNC lathes that use multiple tools for processing because these machine tools need to automatically change tools during the processing process. For CNC milling machines with manual tool change, the corresponding tool change position should also be determined. In order to prevent damage to parts, tools, or fixtures during tool change, tool change points are often set outside the contour of the processed parts, and a certain safety margin is left.
2.2.4 Determine cutting parameters
For efficient metal-cutting machine tool processing, the material being processed, the cutting tool, and the cutting amount are the three major factors. These conditions determine the processing time, tool life, and processing quality. Economical and effective processing methods require a reasonable selection of cutting conditions.
When determining the cutting amount for each process, programmers should choose according to the durability of the tool and the provisions in the machine tool manual. The cutting amount can also be determined by analogy based on actual experience. When selecting the cutting amount, it is necessary to fully ensure that the tool can process a part or ensure that the tool's durability is not less than one work shift, at least not less than half a work shift. The back-cutting amount is mainly limited by the rigidity of the machine tool. If the rigidity of the machine tool allows, the back-cutting amount should be equal to the processing allowance of the process as much as possible so as to reduce the number of passes and improve processing efficiency. For parts with high surface roughness and precision requirements, sufficient finishing allowance should be left. The finishing allowance of CNC machining can be smaller than that of general machine tool machining.
When programmers determine the cutting parameters, they should consider the workpiece material, hardness, cutting state, back-cutting depth, feed rate, and tool durability, and finally, select the appropriate cutting speed. Table 2.1 is the reference data for selecting cutting conditions during turning.
Table 2.1 Cutting speed for turning (m/min)
|
Name of cutting material |
Light Cutting |
Generally, the cutting |
Heavy cutting |
||
|
High-quality carbon structural steel |
Ten # |
100 ～ 250 |
150 ～ 250 |
80 ～ 220 |
|
|
45 # |
60 ～ 230 |
70 ～ 220 |
80 ～ 180 |
||
|
alloy steel |
σ b ≤750MPa |
100 ～ 220 |
100 ～ 230 |
70 ～ 220 |
|
|
σ b >750MPa |
70 ～ 220 |
80 ～ 220 |
80 ～ 200 |
||
2.3 Fill in CNC machining technical documents
Filling in the special technical documents for CNC machining is one of the contents of the CNC machining process design. These technical documents are not only the basis for CNC machining and product acceptance but also the procedures that operators must follow and implement. The technical documents are specific instructions for CNC machining, and their purpose is to make the operator more clear about the content of the machining program, the clamping method, the tools selected for each machining part, and other technical issues. The main CNC machining technical documents include the CNC programming task book, workpiece installation, origin setting card, CNC machining process card, CNC machining tool path map, CNC tool card, etc. The following provides common file formats, and the file format can be designed according to the actual situation of the enterprise.
2.3.1 CNC programming task book It explains the technical requirements and process description of the process personnel for the CNC machining process, as well as the machining allowance that should be guaranteed before CNC machining. It is one of the important bases for programmers and process personnel to coordinate work and compile CNC programs; see Table 2.2 for details.
Table 2.2 NC programming task book
|
Process Department |
CNC programming task book |
Product Parts Drawing Number |
Mission No. |
||||||||
|
Parts Name |
|||||||||||
|
Use CNC equipment |
common Page Page |
||||||||||
|
Main process description and technical requirements: |
|||||||||||
|
Programming received date |
moon day |
Person in charge |
|||||||||
|
prepared by |
Audit |
programming |
Audit |
approve |
|||||||
2.3.2 The CNC machining workpiece installation and origin setting card (referred to as the clamping diagram and part setting card)
It should indicate the CNC machining origin positioning method and clamping method, the machining origin setting position and coordinate direction, the name and number of the fixture used, etc. See Table 2.3 for details.
Table 2.3 Workpiece installation and origin setting card
|
Part Number |
J30102-4 |
CNC machining workpiece installation and origin setting card |
Process No. |
||||
|
Parts Name |
Planet carrier |
Number of clamping |
|||||
|
|
|||||||
|
3 |
Trapezoidal slot bolts |
||||||
|
2 |
Pressure plate |
||||||
|
1 |
Boring and milling fixture plate |
GS53-61 |
|||||
|
Prepared by (date) Reviewed by (date) |
Approved (date) |
Page |
|||||
|
Total Pages |
Serial number |
Fixture Name |
Fixture drawing number |
||||
2.3.3 CNC machining process card
There are many similarities between CNC machining process cards and ordinary machining process cards. The difference is that the programming origin and tool setting point should be indicated in the process diagram, and a brief programming description (such as machine tool model, program number, tool radius compensation, mirror symmetry processing method, etc.) and cutting parameters (i.e., spindle speed, feed rate, maximum back cutting amount or width, etc.) should be selected. See Table 2.4 for details.
Table 2.4 CNC machining process card
|
unit |
CNC machining process card |
Product name or code |
Parts Name |
Part Number |
||||||||||
|
Process diagram |
car between |
Use equipment |
||||||||||||
|
Process No. |
Program Number |
|||||||||||||
|
Fixture Name |
Fixture No. |
|||||||||||||
|
Step No. |
work step do Industry |
Processing surface |
Tool No. |
knife repair |
Spindle speed |
Feed speed |
Back |
Remark |
||||||
|
prepared by |
Audit |
approve |
Year Month Day |
common Page |
No. Page |
|||||||||
2.3.4 CNC machining tool path diagram
In CNC machining, it is often necessary to pay attention to and prevent the tool from accidentally colliding with the fixture or workpiece during movement. For this reason, it is necessary to try to tell the operator about the tool movement path in the programming (such as where to cut, where to lift the tool, where to cut obliquely, etc.). In order to simplify the tool path diagram, it is generally possible to use unified and agreed symbols to represent it. Different machine tools can use different legends and formats. Table 2.5 is a commonly used format.
Table 2.5 CNC machining tool path diagram
|
CNC machining tool path map |
Part Number |
NC01 |
Process No. |
Step No. |
Program number |
O 100 |
||||
|
Machine model |
XK5032 |
Segment number |
N10 ～ N170 |
Processing content |
Milling contour perimeter |
Total 1 page |
No. Page |
|||
 |
||||||||||
|
programming |
||||||||||
|
Proofreading |
||||||||||
|
Approval |
||||||||||
|
symbol |
||||||||||
|
meaning |
Lift the knife |
Cut |
Programming origin |
Cutting point |
Cutting direction |
Cutting line intersection |
Climbing a slope |
Reaming |
Line cutting |
|
2.3.5 CNC tool card
During CNC machining, the requirements for tools are very strict. Generally, the tool diameter and length must be pre-adjusted on the tool setting instrument outside the machine. The tool card reflects the tool number, tool structure, tail handle specifications, assembly name code, blade model and material, etc. It is the basis for assembling and adjusting tools. See Table 2.6 for details.
Table 2.6 CNC tool card
|
Part Number |
J30102-4 |
number control knife Tool Card piece |
Use equipment |
|||||
|
Tool name |
Boring tool |
TC-30 |
||||||
|
Tool number |
T13006 |
Tool changing method |
automatic |
Program Number |
||||
|
knife Tool Group become |
Serial number |
serial number |
Tool name |
Specification |
quantity |
Remark |
||
|
1 |
T013960 |
Pull nail |
1 |
|||||
|
2 |
390, 140-5050027 |
Handle |
1 |
|||||
|
3 |
391, 01-5050100 |
Extension rod |
Φ50×100 |
1 |
||||
|
4 |
391, 68-03650 085 |
Boring bar |
1 |
|||||
|
5 |
R416.3-122053 25 |
Boring cutter components |
Φ41-Φ53 |
1 |
||||
|
6 |
TCMM110208-52 |
blade |
1 |
|||||
|
7 |
2 |
GC435 |
||||||
 |
||||||||
|
Remark |
||||||||
|
prepared by |
Proofreading |
approve |
Total Pages |
Page |
||||
Different machine tools or different processing purposes may require different forms of CNC processing special technical files. In work, the file format can be designed according to the specific situation.
Post time: Dec-07-2024