When making process analysis, the programmer should have the machine tool instruction, programming manual, cutting scale, standard tools, fixture manual, etc., according to the material, contour shape and machining precision of the workpiece, a suitable machine tool is selected, and a machining plan is made to determine the machining sequence of the parts, the cutting tools, fixtures and cutting quantities used in each process. In addition, the programmer should sum up and accumulate practical experience in process analysis to write a high-quality CNC machining program.
1, Rational selection of machine tools
When machining parts on CNC machine tools, there are generally two situations, in the first case, we have a part drawing and blank material, which CNC machine tools should be chosen for the parts? In the second case, we already have numerical control machine tools, how to choose the parts that suit to process on this machine tool. In either case, the main factors to be considered are the material and class of the blank, the complexity of the contour shape of the part, the size, the machining accuracy, the number of parts, the heat treatment requirements, etc. . To sum up, there are three points:
(1) Suppliers need to ensure the technical requirements of processing parts and processing out of qualified products.
(2) Suppliers need to consider which factors are good for productivity.
(3) Suppliers try their best to reduce production costs (processing costs) as much as possible.
2, Technological analysis of CNC machining parts
The technological analysis of CNC machining involves a wide range of aspects, here we only from the possibility and convenience of CNC machining to be analyzed.
2.1 The dimension data on the part drawing should be given in accordance with the principle of convenient programming
The method of marking dimensions on part drawing should be adapted to the characteristic of CNC machining, the dimensions should be drawn on the same datum or the coordinate dimension should be given directly. This method is good for programming and coordination between dimensions. it would bring great convenience in keeping the consistency of the design datum, process datum, test datum and programming origin setting. Because the part designers usually take assembly and other characteristics into account in dimension marking, they have to adopt the part-dispersed marking method, which will bring a lot of inconvenience to process arrangement and CNC machining, because the precision of CNC machining and repeated positioning is very high, the operation characteristics will not be destroyed because of the large accumulated error, so we can change the local scattered method into the method with the same reference or giving the coordinate dimension directly.
At the same time, the geometrical elements forming the outline of the part shall be sufficient. In manual programming, you can calculate the base or node coordinates, but in automatic programming, all the geometric elements that make up the outline of a part are defined, therefore, when analyzing the part drawing, we should analyze whether the given conditions of the geometric elements are sufficient, such as arc and straight line, arc and arctangent in the drawing, but sometimes, according to the size given on the drawing, tangent became intersect or separated. Due to the insufficient conditions of component geometric elements, it is impossible to start programming, in this case, we need to discuss with the part designer to solve this problem.
2.2 The structure of the parts should suit the characteristics of CNC machining
The inside and outside of the part should adopt the uniform geometry type and size, which can reduce the tool specification and tool changing times, make the programming convenient, and improve the production efficiency;
The size of the inner groove fillet determines the size of the tool diameter, so the inner groove fillet radius should not be too small;
The radius R of the groove bottom fillet should not be too large when the part is milling the bottom plane;
Uniform benchmarking should be used. In CNC machining, if there is no uniform datum positioning, the position and size of the contour on the two surfaces after machining will be out of harmony because of the reinstallation of the workpiece. Therefore, a unified reference location should be adopted to avoid the above-mentioned problems and ensure the accuracy of the relative position after the two clamping processes.
It is best to have a suitable hole on the part as the positioning reference hole, if not, to set one hole as the positioning reference hole (such as on the blank to add lugs or set a hole on the margin which will be milled off in the subsequent process ). If the reference hole can't be made, at least make one fine finished surface as a unified standard to reduce the error caused by two times clampings.
In addition, it is necessary to analyze whether the machining accuracy and dimensional tolerance required by the parts can be guaranteed, whether there are any extra dimensions which cause contradiction or closed dimensions which influence the arrangement of the working procedure.
3, Selection of processing method and determination of processing scheme
3.1 Selection of processing method
The selection principle of the machining method is to ensure the machining accuracy of the machined surface and the requirements of the surface roughness. Since there are many machining methods to obtain the same level of accuracy and surface roughness, the shape, size and heat treatment requirements of the parts should be considered in the actual selection. For example, boring, reaming, grinding and other machining methods can meet the precision requirements for IT7 precision holes, but the holes on the box body are generally boring or reaming rather than grinding. Generally, reaming is chosen for the common small size of the box hole, but when the hole diameter is larger, the boring process should be chosen. In addition, productivity and economic requirements, as well as plant production equipment and other practical circumstances should be taken into account. The precision and surface roughness of the commonly used processing methods can be found in the relevant technical manuals.
3.2 Principles for determining the processing plan
The more precise surface, often through rough processing, semi-finishing and fine finishing gradually achieved. It is not enough only to select the corresponding final processing method base on the quality requirements for these surfaces, but also to correctly determine the processing scheme from the blank to the final forming
When determining the processing scheme, the processing method required to meet these requirements shall be initially determined in accordance with the accuracy of the main surface and the requirements of the Surface roughness. For example, for IT7 class accuracy holes with a small aperture, when the final machining method takes the precision reaming, the precision reaming hole usually has to be processed through drilling, reaming and coarse reaming.
4, Division of working procedure and working step
4.1 division of work processes
Machining parts with CNC, working procedures can be relatively centralized, complete most or all of the working procedures as far as possible in one clamping. First of all, according to the part drawing, we should consider whether the part can be processed on one machine, if not, we should decide which part can be processed on this machine, and which part is processed on another machine, that is, divide the processing procedures for the part, there are several ways to divide the general working.
4.2 division of work steps
The division of working steps is mainly considered from machining accuracy and efficiency, it often needs to use different tools and cutting parameters to machine different surface. In order to facilitate the analysis and description of the more complex process, the process is subdivided into steps. The following is an example of a machining centre to illustrate the principle of step division:
4.2.1 the same surface is finished by roughing, semi-finishing and fine-finishing, or all the surfaces are finished by roughing first and fine finishing separately.
4.2.2 for parts with both milling and boring holes, do milling first and then boring. The precision can be improved according to this method. Because the workpiece would be deformation due to the large cutting force when milling. Milling the surface before boring the hole, so that it has a period of time to restore, reduce the deformation and improve the accuracy of the hole.
4.2.3 divide the work step according to the cutting tool. The turning time of some machine tool worktables is shorter than the time of changing the cutting tool. Divide the work step according to the cutting tool to reduce the time of changing the cutting tool and improve the efficiency of the machine.
In a word, the division of working procedures and working steps should be considered comprehensively according to the structural characteristics and technical requirements of specific parts.
5, Parts installation and fixture selection
5.1 basic principles of positioning and installation
1) strive to make the design, process and program computing benchmark unity.
2) to minimize the number of clamping, as far as possible in a location after clamping, processing all the surfaces.
3) avoid the manual adjustment of occupying machine in order to give full play to the efficiency of CNC machines.
5.2 basic principles of selecting fixtures
The characteristics of CNC machining put forward two basic requirements for the fixture: One is to ensure that the coordinate direction of the jig and the machine is relatively fixed; the other is to coordinate the relations of the coordinate system of parts and machine, after that, there are four other things to consider,
1) when the batch of parts processing is not large, we should use modular jigs, adjustable jigs and other general jigs as far as possible to shorten the production preparation time and save production costs.
2) only consider using special jigs in batch production, and strive for simple structure.
3) the loading and unloading of parts should be fast, convenient and reliable to shorten the machine pause time.
4）jigs should not interfere with the machining of the surface of the part, that is, the jig should open its positioning, and the clamping device components should not affect the machining tool (such as collision)
6, Selection of cutting tools and determination of cutting parameters
6.1 selection of cutting tools
Tool selection is one of the important contents in CNC machining. It not only affects the machining efficiency but also directly affects the machining quality. When programming, the selection of cutting tools usually needs to consider the machining capacity of machine tools, process content, workpiece materials and other factors.
Compared with the traditional machining method, CNC machining requires a higher demand for the cutting tool. It not only requires high precision, good rigidity, and high durability but also requires stable size and convenient installation and adjustment. This requires the use of new high-quality materials manufacturing CNC machines and tool parameters optimization.
When selecting the cutting tool, the size of it should be adapted to the surface size and shape of the workpiece to be processed. In the production, the plane parts peripheral contour processing, often uses the vertical milling cutter. When milling flat surface, should choose carbide insert milling cutter; when processing boss, groove, choose high-speed steel end milling cutter; when processing blank surface or rough machining hole, can choose carbide insert corn milling cutter. It is recommended to select the relevant parameters of the cutting tool according to the experience data when selecting the end milling cutter. The ball-end milling cutter is often used in surface machining, but when the surface is flat, the cutting condition of the cutter is poor, so the annular cutter should be used. In single-piece or small-batch production, in order to replace the multi-coordinate linkage machine tool, the drum-shaped cutter or the cone-shaped cutter is often used to process the plane parts with the tooth-inlaid milling cutter, it is suitable for machining some spherical surfaces on a five-axis CNC machine. Its efficiency is nearly ten times higher than that of a ball-end milling cutter, and it can obtain good machining precision.
On CNC, all kinds of cutting tools are installed on the tool magazine, according to the procedure at any time to select and change the cutting tools. Therefore, it is necessary to have a set of connecting rods to connect common cutting tools, so that the standard cutting tools used in drilling, boring, expanding, reaming, milling, etc. . As a programmer, you should know the structure and size of the toolbar used on the machine tool and the adjustment method, so as to determine the radial and axial dimensions of the tool. At present, the TSG tool system is used on CNC in our country. Its shank has the straight shank(three specifications) and taper shank(four specifications), including 16 kinds of knives with different uses
6.2 determination of cutting parameters
Cutting parameters include spindle speed (cutting speed), back to eat the amount of knife, and feed. For different processing methods, it needs to choose different cutting parameters and should be programmed into the list.
The principle of reasonable selection of cutting quantity is that in rough machining, productivity is generally increased, but economy and processing cost should also be taken into account; in semi-finish machining and finishing machining, under the premise of guaranteeing the processing quality, give consideration to cutting efficiency, economy and processing cost. The specific value should be based on the machine tool instruction, cutting quantity manual, and the combination of experience.
7, Determination of tool setting point and tool changing point
During the process of programming, the position of "tool setting point" and "tool changing point" should be selected correctly. "tool setting point" is the starting point of the movement of the tool relative to the workpiece when machining the part on the CNC machines. Because the program section is executed from this point, the tool setting point is also called "program starting point" or "starting point".
The selection principle of tool setting point is as follows,
1) To facilitate the use of digital processing and simplified programming;
2) Easy to find on the machine tool, easy to check-in processing;
3) The machining error is small.
The tool setting point can be selected on the workpiece or outside the workpiece (for example, on the jig or the machine tool), but must have a certain size relationship with the positioning datum of the part.
In order to improve the machining accuracy, the tool setting point should be selected as far as possible on the part design or process data, such as the workpiece with hole location, and the centre of the optional hole as the tool setting point. The position of the cutter is adjusted by the hole so that the "cutter location point" and "Cutter Location Point" coincide. The factory commonly used method is to set the dial gauge on the machine tool spindle, and then turn the machine tool spindle, so that the "Cutter location point" and the cutter location point. The better the consistency, the higher the accuracy of the tool setting. The so-called "Cutter location point" refers to the turning tool, boring tooltip; drill point; End Mill, milling cutter head bottom centre, and Ball Head Milling Cutter Center.
After the parts are installed, there is a definite dimension relationship between the workpiece coordinate system and the machine coordinate system. After the workpiece coordinate system is set, the coordinate value of the first program segment starting from the tool setting point is (X0, Y0). When programming by absolute value, regardless of whether the tool-setting point and the origin of the workpiece coincide, is X2, Y2; when programming by incremental value, the coordinates of the first program segment are X2 and Y2 when they coincide with the origin of the workpiece, and X1+ X2 and Y1 + Y2 when they do not coincide.
The tool setting point is not only the beginning point but also the endpoint of the program. Therefore, the repeated accuracy of the tool setting point should be considered in batch production, which can be checked by the coordinate value (X0, Y0) between the tool setting point and machine tool origin.
The so-called "machine tool origin" refers to a fixed machine tool on the limit point. For example, a lathe refers to the lathe spindle rotation centre and the head Chuck endpoint of the intersection.
When the tool change is needed in the processing, the tool change point should be specified. The so-called "tool change point" is the position of the tool change when the tool holder changes position. The point can be either a fixed point (such as a machining centre machine tool, where the position of the tool changing manipulator is fixed) or an arbitrary point (such as a lathe). The tool change point shall be located outside the workpiece or fixture, and the workpiece and other parts shall not be touched when the tool holder is rotated. The set value can be determined by the actual measurement method or calculation.
8, Determination of processing routes
In CNC machining, the path of cutter position relative to the movement of workpiece is called machining path. When programming, the main principles of determining the processing route are the following,
1) the processing route shall ensure the accuracy and surface roughness of the parts to be processed and shall be of high efficiency.
2) make numerical calculations simple to reduce the amount of programming effort.
3) the processing route should be kept to a minimum, which can reduce both the number of program segments and the tool-free time and so on, to determine whether one feed or multiple feeds to complete the processing and the milling process is to use forward milling or reverse milling, etc.
For point-to-point CNC machine tools, the positioning accuracy is high, the positioning process is as fast as possible, and the path of the tool relative to the workpiece is irrelevant. In addition, the axial motion size of the tool should be determined, which is mainly determined by the hole depth of the part to be machined, but some auxiliary dimensions should be considered, such as the tool lead-in distance and overshoot.
When turning threads on CNC machines, the z-direction feed along the pitch direction should maintain a strict speed ratio with the rotation of the machine tool spindle, so cutting during the acceleration or deceleration of the feed mechanism should be avoided. Therefore, it is necessary to introduce distance δ1 overstep distance δ2 and the values are related to the dynamic characteristics of the drive system of the machine, also the pitch of the thread and the precision of the thread. It is generally 2 - 5mm, for large pitch and high precision thread, it needs to take a large value, generally taking about 1/4. If there is no back groove at the end of the thread, the shape of the back end is related to the CNC system, generally press 45° to finish.
When milling plane parts, the side edge of the end milling cutter is usually used. In order to reduce the tool marks and ensure the surface quality of parts, the cutting and cutting procedures need to be carefully designed. When milling the outline of the external surface, the point of cut-in and cut-out should be cut in and out of the surface of the part along the lengthening line of the outline curve of the part, and should not be cut in the normal direction directly to avoid scratches on the surface of the part, make sure the outline of the part is smooth.
When milling the surface of the inner contour, the cut-in and cut-out can not be extended, then the cutter can cut in and out along the normal direction of the contour of the part, and the cut-in and cut-out point can be selected at the intersection of two geometric elements of the contour of the part, in the process of machining, when the system of the workpiece, cutter, fixture and a machine tool is in the state of equilibrium elastic deformation, the cutting force is reduced when the feed is stopped, which will change the equilibrium state of the system, the tool will leave scratches on the surface of the part where the feed stops, so feed stops should be avoided in contour machining.
When the surface is curved, the ball-end cutter is often used to cut the surface by the "line cutting method". The so-called line-cutting method means that the cutting point locus of the tool and the contour of the part is one line, and the distance between the lines is determined according to the requirement of the precision of the part.
This article gives a general guideline on how to analyse the process of CNC machining. Xu Feng has rich experience in CNC machining, so if you have such need, kindly contact us for the details, and any questions can be welcomed.