Machining design of flange

With the rapid development of science and technology and the increasingly fierce economic competition, the renewal speed of mechanical products is becoming faster and faster, and the proportion of multi-variety, medium and small batch production has increased significantly. At the same time, with the rapid growth of aviation industry, automobile industry and light industrial consumer goods production, there are more and more parts with complex shapes, and the accuracy requirements are also higher and higher. In recent decades, countries all over the world have attached great importance to the development of CNC machining technology that can effectively solve the processing of complex, precise and small batches of variable parts.
CNC machining technology is the basis for manufacturing industry to realize automation, flexibility and integration production. Modern CAD/CAM, FMS, CIMS, etc. are all based on CNC machining technology. Without CNC machining technology, advanced manufacturing technology will become rootless. The essence of the competition in mechanical manufacturing is the competition in numerical control technology.
CNC machine tool is a machine tool with CNC technology, or equipped with CNC system. In terms of application, CNC machine tools are used to express various operations and steps required by the processing process (such as spindle speed change, unclamp workpiece, feed and retreat, start and stop, select tool, supply cutting fluid, etc.) and the relative displacement between tool and workpiece with digital code. The digital information is sent to a special or general computer through the control medium, and the computer processes and calculates the input information, Send out various commands to control the servo system or other executive components of the machine tool, so that the machine tool can automatically process the required parts.
In modern production, in order to meet the requirements of multiple varieties, small batches, and fast product renewal cycle, the production line with single-function machine tools as the main body can no longer meet the increasing requirements of the mechanical manufacturing industry, so the equipment and production system with multi-function and certain flexibility have emerged one after another, which promotes the development of CNC technology to a higher level. Modern production systems mainly include flexible manufacturing cell (FMC), flexible manufacturing system (FMS) and computer integrated manufacturing system (CIMS).
CNC machine tool is a kind of high-efficiency automatic processing equipment. Compared with ordinary machine tools, it is characterized by good flexibility, strong adaptability, high accuracy, stable quality, high processing productivity, multi-function and high complexity control, reduced labor intensity, high reliability, good economy, and is conducive to the modernization of manufacturing system. These advantages have accelerated the penetration of CNC technology into various industrial fields, and the application scope has been expanding. CNC machine tools not only play a more and more important role in processing multiple varieties and small batches of parts, parts with complex structure and shape, parts that need frequent modification, parts that are expensive and not allowed to be scrapped, and urgent parts that need the shortest production cycle, but also have achieved good results in processing large batches and parts with less complex structure and shape.
The goal of the development of CNC system is to further reduce the price, increase the reliability, expand the function, improve the operation comfort, improve the integration, improve the flexibility and openness of the system, reduce the volume, and make the CNC machine tool have higher speed, higher accuracy, higher reliability and stronger function.

What is a flange?

Flange is a disk-shaped part, which is most common in pipeline system. Flanges are used in pairs. In pipeline system, flanges are mainly used for pipe connection. A flange shall be installed for the pipes to be connected. The threaded flange can be used for the low pressure pipes, and the welding flange can be used for the pressure above 4kg. Add sealing points between the two flanges and fasten them with bolts. Flanges with different pressures have different thicknesses and use different bolts. When pumps and valves are connected with pipes, parts of these equipment are also made into corresponding flange shapes, also known as flange connection. All connecting parts that are bolted and closed at the periphery of two planes are generally referred to as “flanges”, such as the connection of ventilation pipes. Such parts can be referred to as “flange”. But this kind of connection is only a part of the equipment, such as the connection between the flange and the water pump, so it is not easy to call the water pump “flange”. Smaller parts such as valves can be called “flange”.

1. Preparation of flange machining process specification

1.1 Determine production type

As shown in the figure, it is the flange of a product with an annual output of 10000 sets, with a spare parts rate of 25%, a machining scrap rate of 0.2%, and a quantity of 1 piece in each product. Now the machining process of the flange is formulated:

N=Q*n*(1+a%)*(1+b%)…………………（1.1）

=10000*1*(1+25%)*(1+0.2%)

=12525 pieces/year

The annual output of flange is 12525 pieces. It is now known that this product belongs to light machinery. According to the relationship between production type and production program, its production type is determined to be mass production.
Process characteristics of mass production:

• (1) Interchangeability of parts: it has extensive interchangeability, and a few assembly accuracy is relatively high, so group assembly method and adjustment method are adopted;
• (2) Manufacturing method and machining allowance of blank: metal die machine modeling, die forging or other efficient methods are widely used. High blank accuracy and small machining allowance;
• (3) Machine tool equipment and its layout form: efficient special machine tools and automatic machine tools are widely used and arranged according to the assembly line and automatic line;
• (4) Process equipment: efficient fixtures, composite tools, special measuring tools or automatic inspection devices are widely used to meet the accuracy requirements by adjustment;
• (5) Technical requirements for workers: high technical requirements for the adjustment workers, low technical requirements for the operators;
• (6) Process documents: there are process cards, and adjustment cards and inspection cards are required for key processes;
• (7) Cost: relatively low;
• (8) Production efficiency: high;
• (9) Working conditions of workers: good.

1.2 Flange analysis

1.2.1 Analysis of parts

The flange is made of HT150 (gray cast iron). GB9439-88 is a ferritic and pearlitic gray cast iron. Its casting performance is good, the process is simple, the casting stress is simple, and it has certain mechanical strength and good vibration damping performance without artificial aging treatment. It is applicable to parts that bear large stress and require wear resistance.
The main machined surface of the part is Ф50.5 of the outer surface and Ф31 of the inner bore.
Ф26 hole with Ф50.5 coaxiality ø 0.01mm, and Ф31H7 hole coaxiality ø 0.05mm, and Ф50f7 coaxiality ø 0.1mm with the A circular runout 0.02mm, directly affect its installation accuracy, in processing them the best can be in a clamping of the two holes or two outer circle at the same time. In addition, the parallelism of D surface relative to C surface 0.1mm also affects the mounting accuracy.

1.2.2 Selection and manufacturing method of blank

According to the technical requirements, the part material is HT150, the blank is determined to be a casting, and the production program of the part is known to be 12525 pieces/year, the mass of the part is about 1kg, so the production type is mass production.
According to the material, production type, production program and the complexity of parts, the blank can be cast.
The reason for selecting blank casting: the shape of the casting is close to the part, which can reduce the amount of machining and thus reduce the casting cost.

1.3 Design of machining process procedures

1.3.1 Selection of positioning reference

When studying and analyzing the problem of workpiece positioning, the selection of positioning datum is the key. Generally speaking, once the positioning datum of the workpiece is selected, the positioning scheme of the workpiece is basically determined. The points, lines and planes used as the positioning datum can be actual or imaginary, such as the axis of outer circle and inner hole, symmetry plane, etc.
The selection of positioning reference is a very important issue in formulating process procedures. In the first process, only the raw blank surface on the workpiece can be used for positioning. This positioning datum is called coarse datum. In the later process, the processed surface can be used for positioning, and this positioning datum is called precision datum. In the flange machining process, a designated end face and outer circle of the flange are selected as the main base surface for most processes, and the large outer circle is used as the other base surface. This is due to the large area of the end face and relatively stable positioning.
Further study:

• (1) When rigid rough machining is performed on the left end, that is, in the first machining process, each surface of the workpiece is a blank surface, and the conditions for positioning and clamping are poor, while the machining allowance and cutting force are large. If the workpiece itself is poor again, the machining accuracy will be greatly affected. Therefore, the selection of the positioning and clamping method of the first process often has a profound impact on the machining accuracy of the entire process, Therefore, the right end face and outer circle of the flange are used as the locating surface and clamping surface. Carry out rough turning, then turn around and carry out rough machining on the other end. Use the large outer circle and the right end face for positioning and clamping.
• (2) When connecting holes and small holes are processed on the parts, special clamps are needed for processing, and the locating surface is still clamped with the outer circle surface and one side of the large outer circle.

1.3.2 Selection of flange surface machining method

The machined surfaces of this part are two end surfaces, small outer circle, outer circle (Φ50), outer circle of Φ50.5 and large outer surface, as well as hole of Φ31H7, hole of Φ26, two slots of right end and connecting hole and small hole. as well as Φ3 bevel hole.
Both end faces: dimensional tolerance is 31.5±0.05, and rough turning, semi-finish turning and finish turning are required.
Small outer circle: size tolerance Φ42±0.3, rough turning, semi-finish turning and finish turning are required
Outer circle of Φ50: Dimensional tolerance is Φ50f7, surface roughness is Rz7µm, rough turning, semi-finishing turning and finishing turning are required.

• Outer circle of Φ50.5: Dimensional tolerance is Φ50.5, surface roughness is Rz3.5, rough turning, semi-finishing turning and finishing turning are required.
• Large outer circle: the dimension tolerance is Φ73.5, rough turning, semi-finish turning and finish turning are required. And the distance between the two sides is 6.85±0.02, and the parallelism of one side surface relative to Φ another fixed base surface is 0.1, and rough turning, semi-finishing turning and finishing turning are required.

Hole of Φ31H7: tolerance grade is H7, surface roughness is Rz8.5µm, which can be machined by rough boring, semi-finish boring and finish boring.
Hole of Φ26H7: tolerance grade H7, surface roughness Rz8.5µm, can be machined by rough boring, semi-finish boring and finish boring.
A slot of 5mm width and Φ43 diameter and a slot of 2.4±0.1mm width and Φ47.65 diameter; rough and finish turning are used.
6﹡Φ6.5 hole: the position degree relative to Φ50.5 is Φ0.02, and drilling and reaming are adopted.
6﹡Φ10’s hole: using drilling.
Small hole of Φ2.8±0.1: drilling can be used.
Hole of Φ2.5: Drilling and reaming are adopted.
Diagonal hole of Φ3: Drilling is used.

1.3.3 Process route

When the production batch is different, the process route of the parts will also have a large difference, when the parts have high processing quality requirements, the whole process should be divided into roughing stage, semi-finishing stage, finishing stage, and finishing stage. This can ensure the quality of processing, the reasonable use of machine tools, to adapt to the needs of heat treatment, in the roughing stage can be found defects, to facilitate even scrap or repair, the surface finishing arrangements at the end, so that these surfaces are less or not damaged.
The process route of flange mass production is listed in Table 2-1.

S/N	Operation name	Operation content
30	Rough turning	Rough machining the left end, rough turning the end face, rough turning Φ42 outer circle, Φ50 outer circle, and large outer circle.
	Boring	Rough boring Φ31 hole.
40	Rough Turning	Rough machining right end, rough turning end face, rough turning Φ50.5 outer circle.
	Boring	Rough bore Φ22.
50	Turning	Finish machining the left end face, semi-finish turning the end face, semi-finish turning the outer circle of Φ42, semi-finish turning the outer circle of Φ50 and the large outer circle.
	Boring	Semi-finish bore Φ31.
60	Boring	Finish turning the end face, finish turning the outer circle of Φ42, finish turning the outer circle of Φ50 and the large outer circle, and finish turning one side of the large outer circle.
	Boring	Fine-boring Φ31 hole. Turn the groove of width 3.9.
	Turning	Finish machining the right end face, semi-finish turning Φ50.5 outer circle.
		Finish turning Φ50.5 outer circle, finishing turning the other side of large outer circle, finishing turning groove of width 5 and 2.4.
		Fine-turn a groove of width 2.1 and depth 1.1 on one side of large outer circle.
		Semi-finish boring Φ26 hole, chamfering of semi-finish boring hole, finish boring hole and its chamfering.
70	Drill hole	Machining joint hole and small hole, drilling Φ6.5 through hole, then drilling Φ3 hole with Φ10 drill bit to 4.5mm deep.
		Drill Φ2.5 hole and ream the hole, and drill Φ2.8 hole.
75		Machining slant hole, drilling Φ2.5 slant hole as well as reaming.

1.3.4 Processing equipment and process equipment

Due to the type of production for mass production, so the processing equipment should be mainly general-purpose machine tools, supplemented by a small number of special machine tools. The production method to general-purpose machine tools plus special fixtures, supplemented by a small number of special machine tools in the production line. Workpiece clamping on each machine tool and the transfer between the machines are completed by hand.
① Select machine tools

• a. Process 30, 40 is rough turning, the part outline size is not large, accuracy requirements are not very high, choose CK200.
• b. Process 50, 60 belongs to the finishing molding, can be processed on the cutting center, choose MT2-200W.
• c. Process 70 can be processed by machining center, optional VTC-160A/16A.
• d. Process 75 can be processed on a drilling center, optional DTC510.

② Selection of fixture
This flange processing except for the processing of connection holes and small holes need to design fixtures, other processes can use general fixtures.
③ Choose tool

• a. Rough turning end face, outer circle and large outer circle: PCMNR2020-16 tool can be selected, where the shape of the insert is 80 ° diamond, rough boring tool can be selected micro-adjustment boring tool, insert for machine clamping type, M: M20 * 0.5, L = 64mm, l = 16mm boring tool.
• b. Process 50, semi-finish turning end face, Φ42 outer circle, Φ42 outer circle, Φ50 outer circle and large outer circle can use PCLN (L/R) 2525M-12 outer diameter turning tool, semi-finish boring Φ31 hole and chamfering, use S13R-SCLPROP-20E inner diameter boring tool. For finish turning end face, Φ42 outer circle, Φ51 outer circle and large outer circle, use MCLN (L/R) 2525M12M5 outer diameter turning tool; for finish boring Φ31 hole and its chamfer, use S16Q-SDUCL11-20E inner diameter boring tool. For turning a 3.9 width groove, an OD groove cutter KGML2525M-3 can be used.
• c. Process 60 semi-finish turning Φ50.5 outer circle, you can choose PCLNR2525M-12 outer diameter turning tool, semi-finish boring Φ26 hole, you can choose CNMG120408WQCA5025 inner diameter boring tool, finish turning end face, Φ50.5 outer circle and the other side of large outer circle, you can choose CPMHO90304HQCA5025 outer diameter boring tool, semi-finish boring Φ22 hole and For semi-finish boring Φ22 hole and chamfering, use WNMG080408WF4015 ID boring tool; for finish boring and chamfering, use TCMT110308PF4015 ID boring tool; for finish turning 5 wide slots, use VBGT110302R-YPR930 OD slotting tool; for finish turning 2.4 wide slots, use GMG3020-03MGPR930 OD slotting tool; for finish turning one side of large outer circle 2.1 wide and 1.1 deep groove GFVR2525M-201A end groove cutter.
• d. Drill Φ6.5 through-hole available straight-shank break twist drill, drill a deep 4.5 hole Φ10 with d = 10mm straight-shank twist drill, drill Ф3, Ф2.5 hole available straight-shank twist drill, drill Φ2.8 hole can be used d = 2.8mm straight-shank long twist drill.
• e. Drilling Ф2.5 oblique hole available diameter of 2.4 straight-shank twist drill, hole expansion available diameter of 2.5 straight-shank twist drill.

⑤ Choose a gauge
This part is a mass production, are generally used in general gauges. There are two ways to choose the gauge: one is to choose the uncertainty of the measuring instrument; the second is to choose the limit error of the measurement method according to the measuring instrument.

• a. Rough machining can be used vernier calipers, indexed to 0.02mm.
• b. Finishing processing hole with the gauge is the inside diameter micrometer, the index value of 0.001mm. processing outer circle with the gauge can choose the outside diameter micrometer, outer circle or inner hole step depth available height meter, the length of the workpiece or tolerance range of the larger hole or outer circle available 0.01mm digital display vernier calipers. Roughness and form tolerances or the operator’s own inconvenience measurement of the size available contour meter measurement. In addition, the appearance of the parts should be 100% inspected.

1.3.5 Machining process and cutting amount of calculation

The general method of determining the process size is to project forward from the last process of the machined surface, and the process size of the last process is marked according to the requirements of the part drawing. When there is no datum conversion, the process size of the same surface processed several times is only related to the machining allowance of the process (or work step). When there is a datum conversion, the process dimensions are solved by applying the process dimension chain.
Process 30➟Rough machining of the left end face, Process 50➟Finishing of the left end face.
Checking the relevant manual for the machining allowance table, we know that the left end face finishing allowance is 0.605mm, and the total left end face allowance is 1.525mm, so the roughing allowance is (1.525-0.605)=0.92mm.
As shown in the figure, finishing the left end of the process to the right end face and Ф50.5 of the outer circle positioning. Then the left end to the C surface of the process size that is the design size, X precision = (27.675 ± 0.025) mm, then the roughing process size X coarse = 28.28mm.
Check the textbook Table 3-16 plane processing method, the rough turning tolerance level is IT11-13, take IT11, its tolerance T fine = 0.10mm, so X coarse = (28.28±0.05) mm.
Calibrate the finish turning allowance Z fine.
Z fine min=X fine min-X fine max=[(28.28-0.05)-(27.675+0.025)]= 0.555mm, so the margin is enough.
Check the relevant manual, take the feed per revolution f=0.5mm/r for rough turning and f=0.1mm/r for finishing, take the spindle speed of 320r/min for rough turning and n=560r/min for finishing.
Process 50, finish machining forming
(1) (Rough turning – semi-finishing turning – finishing turning) The outer circle of each section is shown in Table 2-2.

Name	Machining allowance	Process dimensions and tolerances
Precision Turning Φ50	0.6	Φ50 -0.025 -0.05
Φ50.5	1.25	Φ50.5 -0.050 -0.058
Φ73.5	0.55	Φ73.50-0.1
Rough Turning Φ50	1.5	Φ50.6±0.1
Φ50.5	1.5	Φ51.75±0.1
Φ73.5	0.95	Φ74.05±0.1

Check the relevant manual, take the feed per revolution f=0.5mm/r for rough turning, f=0.3mm/r for semi-finishing turning and f=0.1mm/r for finishing turning; the spindle speed is 320r/min for rough turning and 560r/min for finishing turning.
(2) Rough boring – semi-finish boring – finish boring is shown in Table 2-3.

	Machining surface	Machining allowance	Tolerance class	Process size
Fine Boring	Φ26	0.2	IT7	Φ26+0.021-0
	Φ31	0.2	IT7	Φ31+0.025-0
Semi-finish Boring	Φ26	0.4	IT9	Φ25.8+0.052-0
	Φ31	0.4	IT9	Φ30.8+0.062-0
Rough Boring	Φ26	1	IT11	Φ25.4±0.1
	Φ31	1	IT11	Φ30.4±0.1

Check the relevant manual, take the feed per revolution f=0.5mm/r for rough boring, f=0.3mm/r for semi-finish boring, f=0.08mm/r for finish boring, take the rough boring ap=1mm, semi-finish boring ap=0.8mm, and finish boring ap=0.2mm.

1.3.6 Time quotas: Calculation of time quotas for process 70

Time quota is the time consumed to complete a process under certain production conditions. Time quota is the main indicator of labor productivity of a process, an important basis for production planning and costing, and the main information for calculating the number of equipment and personnel when designing or expanding a factory (or workshop).
The time quota of a process to complete a part is called time quota (TP), which consists of the following parts.
(1) Basic time ™ directly changing the size, shape, relative position, surface form or material properties of the production object and other process time consumed.
(2) It auxiliary time (ta) is the time consumed by the various auxiliary actions necessary to realize the process.
(3) Layout workplace time (ts) it is the time consumed to make the processing normal.
(4) Rest and physiological needs time (tr.n) it is the time consumed by the operator during working hours to restore physical strength and meet physiological needs, which can generally be calculated at 2% of the operating time.
① Maneuver time: reference to relevant information, to get the formula for drilling.

t_j=(l+l₁+l₂)/(f*n)
l₁=D*(cotk_r)/2+(l-2)

l₂=1 – 4,l₂=0 when drilling blind holes.

For drilling 6 – Φ6.5mm:

l₁=[6.5*cot(118°/2)/2+1.5]=3.45mm

l=70mm,take l₂=3mm.

The above data and the previous have been selected f and n into the formula, we get:

t_j=(70+3.45+3)/(0.4*630)=0.30mm
6t_j=4*0.30min=1.2min

For drilling 6 – Φ10mm:

l₁=[10*cot(118°/2)/2+1.5]mm=3mm
l=100mm,l₂=0

Substituting the above data and the previously selected f and n into the formula, we get:

t_j=(100+3)/(0.3*1000)=0.34min

6t_j=0.34*6=2.06min

For drilling Φ2.8 mm:

l₁=[2.8*cot(118°/2)/2+1.5]mm=2.34mm
Take l=100mm,l₂=0mm
t_j=(100+2.34)/(0.4*230)=0.41min

For drilling Ф3 holes:

l₁=[3*cot(118°/2)/2+1.5]=2.4mm
Take l=10mm,l2=0mm,
t_j=(10+2.4)/(0.035*45)=7.87min

For drilling Ф2.4:

l₁=[2.4*cot(118°/2)/2+1.5]=2.22mm

Take l=10mm,l2=0mm

t_j=(10+2.22)/(23*0.5)=1.1min

Referring to the relevant information, the formula for calculating the bottom of the reamed hole is

t_j=(l+l1+l2)/(f*n)
l₁=(D-d)*(cotk_r)/2+(l-2)

When reaming blind holes, l₂=0mm.
For reaming Ф2.5:

l₁=[(2.5-2.4)*cot(118 ° / 2)/2+1.5)=1.53mm
t_j=(10+1.53+0)/(0.25*15)=3.07min

① Time t_j:

t_b=(1.2+2.06+0.41+7.87+1.1+3.07)=15.71min

1.3.7 Machining process cards

① Comprehensive process card
Briefly write each process, as production management use.
② Craft card
Detailed description of the entire process, as a guide to workers and help managers and technicians to master the entire parts processing process of a process document, in addition to the content of the process, should also fill in the cutting amount used in the process and the name of the tooling equipment, code, etc..
③ Process card
More detailed process documents used to guide workers in the production of key parts in mass production of the key processes are used.

• (1) The sketch can be scaled down and expressed in as few projected views as possible. Sketch can also be drawn only with the processing part of the local view, in addition to the processing surface, positioning surface clamping surface, the main contour surface, the rest of the line can be omitted, to the extent necessary, clear.
• (2) The surface to be processed with a thick solid line (or red line), the rest are fine solid line.
• (3) Should indicate the process dimensions, tolerances and roughness requirements of the process.
• (4) Positioning, clamping surface should be marked with the specified symbols.

2. The machining program of flange

CNC programming, that is, the preparation of CNC machine tool machining programs, it is the most important part of the use of CNC machine tools. It is divided into manual programming and automatic programming. CNC program to the parts processing process, process parameters (feed rate and spindle speed, etc.), displacement data (geometry and geometry size, etc.) and switching commands (tool change, cutting fluid on/off and workpiece loading and unloading, etc.) and other information with the CNC system to specify the function code and format according to the processing order written into a processing program sheet, and recorded on the information carrier.
CNC lathe is one of the most widely used CNC machine tools at present. CNC lathes are mainly used for processing rotary parts such as shafts and discs. Through the operation of CNC machining program, it can automatically complete the cutting and processing of internal and external cylindrical surface, conical surface, forming surface, thread and end face, etc. It can also carry out grooving, drilling, reaming and reaming, etc. The turning center can complete more machining procedures in one clamping, improve machining accuracy and productivity, and is especially suitable for the machining of complex-shaped rotary parts. As the machining object of CNC lathe is mostly rotary body, general three-jaw chuck fixture is used.
Programming characteristics of CNC lathe:

• ① Absolute size and incremental size G90 and G91 instructions correspond to absolute position data input and incremental position data input respectively.
• ② Machining coordinate system machining coordinate system should be consistent with the coordinate direction of the machine tool coordinate system, X-axis corresponds to radial, Z-axis corresponds to axial, C-axis (spindle) movement direction is to look from the machine tailstock to the spindle, counterclockwise for +C direction, clockwise for -C direction.
• ③ Diameter programming method and radius programming using the diameter size programming and the size of the part drawing marked the same, so as to avoid the size of the conversion process may cause errors, to bring great convenience in programming.
• ④ In and out of the way cutting starting point is determined with the size of the workpiece blank margin, should be the tool quickly go to the point when the tool tip does not collide with the workpiece as the principle.
• ⑤ Cycle function CNC system has different forms of cycle function to reduce the programming workload.
• ⑥ Constant cutting speed control in order to ensure the quality of the machined surface, the use of constant cutting speed control function, the CNC system can be based on the X coordinate value where the tool tip is located, as the diameter of the workpiece value to calculate the spindle speed.

Whether manual programming or automatic programming are to go through the drawing analysis, auxiliary preparation, the development of processing technology, mathematical processing, filling out the program sheet, the preparation of control media, program verification steps and then machine tool processing. Manual programming is suitable for processing parts with relatively simple shapes. In the future when automatic programming is developing at a high speed, the status of manual programming is still very important and is the basis of automatic programming.
CNC system functions.

• S function (1) constant line speed control G96S – where the number after S indicates the constant line speed in m/min. (2) constant line speed cancellation G97S – where the number after S indicates the spindle speed after constant line speed control cancellation, if S is not specified, the final value of G96 will be retained.
• T function programming format T – where T is usually followed by two digits indicating the selected tool number. However, there are also four digits used after T. The first two are the tool number, the last two are the tool length compensation number, and again the tool tip radius compensation number.
• M function M00: program pause; M3: spindle clockwise rotation; M04: spindle counterclockwise rotation; M05: spindle rotation stop; M08: coolant on; M09: coolant off; M30: program stop, program reset to the starting position.
• G function G00 fast point positioning; G01 linear interpolation instruction; G02 for clockwise circular interpolation at the specified feed rate; G03 for counterclockwise circular interpolation at the specified feed rate.

The tool radius compensation instruction is often inconsistent with the center trajectory of the tool and the part contour due to the tool radius size when milling the part contour. In order to avoid the calculation of the tool center trajectory, directly according to the contour size on the part drawing programming, the CNC system provides the tool radius compensation function. Among them, G41 is the left offset tool radius compensation, G42 is the right offset tool radius compensation, and G40 is the undo tool radius compensation instruction.
Subroutine call: M98P – where: P indicates the subroutine call. 8 digits after P, the first four digits are the number of calls, omitted when called once; the last four digits are the number of the subroutine called. m99 indicates the end of the subroutine and returns to the main program in which the subroutine was called.
Determine the tool route and arrange the processing sequence should pay attention to the following points:

• 1). Seek the shortest processing route;
• 2). The final contour of a single tool to complete; 3, choose a reasonable cut-in and cut-out direction.

Roughing endface and finishing forming procedures

Left end face

O01683

G00  G40  T0000;

M1100;

M1300;

#2601=0（Z  AXIS  WORKSIFT）;

G28  W0;

G28  U0;

G00  G97  T100  S300;

G30  U0  W0;

M305（OD  MEATUR）;

;

M307（ID  MEATUR）;

;

T0000;

M1100;

T0;

T0000;

M1300;

T0;

M205;

M00;

;

N1  M105;

M80;

M68;

M60;

M69;

/9  M99  P200;

/8  M99  P200;

;

/ M00;;

N10（OD  ROUGH  NR=0.8）;

G00  G97  T0199  S500  M03;

G00  G96  X47.22  S220  M08;

G00  Z43.0;

G01  Z41.9  F0.3;

G01  X51.0  Z40.111;

G01  Z21.2  F0.35  M15;

M16;

G00  G97  X75.0  Z100.0  M09  S1000;

G00  T0188;

/ M00;

;

N20 (ID  ROUGH  NR=0.4);

G00  G97  X31.563  T0299  S1000  M03;

G00  G96  Z44.0  S220  M08;

G01  Z41.9  F0.3;

G01  X30.6  Z39.17  F0.3;

G01  Z24.7  F0.2;

G01  X25.75  F0.3;

G01  Z0.5  M15;

M16;

G00  G97  X22.0  Z60.0  S1000;

G00  T0288;

/ M00;

;

N30 (OD  FINISH  NR=0.4);

G00  G97  X52.0  T0399  S1000  M03;

G00  G96  Z41.7  S360  M08;

G01  X30.0  F0.16;

G00  X45  Z43;

G42  G01  Z41.71  F0.2;

X48.774;

G04  U0.01;

G03  X49.161  Z41.552  R0.2  F0.06;

G04  0.01;

G01  X49.963  Z40.06  F0.12;

G04  U0.2;

G40  G01  Z20.875  F0.08;

G00  X73.045  W0.5;

G42  G01  Z20.875  F0.3;

G03  X73.445  Z20.675  R0.2  F0.08;

G40  G01  Z13.0  F0.18;

G00  X74.0  Z21.0;

G01  Z20.875  F0.3;

G04  U0.01;

G01  X49.963  F0.15  M15;

M16;

G00  G97  X75.0  Z100.0  S1000  M09;

G00  T0388;

/ M00;

;

N40 (OD  GROOVE  T=3.0  NR=0.3);

G00  G97  X52.0  T0599  S1000  M03;

G00  G96  Z33.9  S160  M08;

G01  X50.2  F0.3;

;

G65  P9005  X45.619  I1.0  F0.1  U0.2;

G01  U0.2  F0.3;

G01  X45.419  F0.05  M15;

M16;

G00  X51.0;

G04  U0.01;

G00  Z32.8;

G04  U0.01;

G01  X49.963  F0.2;

G02  X48.763  Z33.4  R0.6  F0.05;

G01  X45.369  F0.12;

G04  U0.1;

G00  X51  Z33.6;

G04  U0.01;

G00  Z35;

G04  U0.01;

G01  X49.963  F0.2;

G03  X48.713  Z34.4  R0.6  F0.05;

G01  X45.369  F0.12;

G04  U0.1;

G01  Z33.4  F0.1;

G04  U0.1;

G00  G97  X80  Z33.6  S1000;

G00  Z100  M09;

G00  T0588;

;

N50 (ID  FINISH  NR=0.2);

G00  G97  X33  T0699  S1000  M03;

G00  G96  Z43  S300  M08;

G41  G01  Z41.7  F0.2;

X32.037;

G02  X31.871  Z41.655  R0.1  F0.04;

G01  X31.755  Z41.568  F0.06;

G02  X21.471  Z41.204  R0.95  F0.05;

G01  X0.5  Z38.445  F0.08;

G40  G00  X30.4  Z40.5;

G01  X31.013  F0.3;

G04  U1;

G01  Z30  F0.08;

G41  G00  X28.931  Z37.379;

G01  X31.4  Z35.4  F0.06;

G04  U0.2;

G01  Z30  F0.08;

G04  U0.2;

G01  X30.492  Z29.199  F0.03;

G40  G01  Z34  F0.3;

G01  X31.013  F0.3;

G04  U2;

G01  Z24.9  F0.08;

G00  X25  W0.3;

G01  Z24.3  F0.3;

G01  X31.013  F0.1;

G01  Z25  F0.08;

G00  X26.411  W0.3;

G41  G01  Z24.3  F0.3;

G02  X26.011  X24.1  R0.2  F0.06;

G40  G01  X25.5  Z23.645  F0.1;

G00  G97  X24  Z100  S200;

G04  U5.0;

G00  X150  M09;

G00  T0688;

T100;

M81;

G30  U0  W0  T100  M05;

M80;

M10;

N200;

M01;

M99  P1;

%

Right end face

O02683

G00  G40  T0000;

M1100;

M1300;

#2601=0 (Z  AXIS  WORKSIFT);

G28  W0;

G28  U0;

G00  G97  T300  S300;

G30  U0  W0;

;

;

;

;

T0003;

M1101;

T0;

T0004;

T0;

M1301;

T0;

M205;

M00;

;

N1  M105;

M68;

M60;

M69;

/9  M99  P200;

/8  M99  P200;

;

G65  P9031  A0.2  B0.1  I1.0;

/ M00;

;

N10 (OD  FINISH  NR=0.4);

G00  G97  X53.0  T0399  S1500  M03;

G00  G96  Z41.4  S250  M0.8;

G01  X34.0  F0.2;

G00  X47  Z43;

G42  G01  Z41.41  F0.2;

X49.603;

G03  X49.989  Z41.251  R0.2  F0.08;

G01  X50.6  Z40.111  F0.1;

G40  G01  Z41  F0.5;

G01  X50.445  F0.3;

G04  U0.2;

G01  Z38.4  F0.05;

G01  Z36.0  F0.2;

G01  Z33.6  F0.05;

G01  X51.25  F0.3;

G01  Z27.675  F0.3;

G00  X73  W0.6;

G42  G01  Z27.675  F0.3;

G03  X73.4  Z27.457  R0.2  F0.08;

G40  G00  X74.0  Z28.0;

G01  Z27.675  F0.3;

G04  U0.01;

G01  X51.25  F0.3  M15;

M16;

G00  G97  X80.0  Z90.0  S1000  M09;

G00  T0388;

/ M00;

;

N20 (ID  FINISH  NR=0.4);

G00  G97  X24.0  T0499  S1000  M03;

G00  G96  Z42.2  S230  M08;

G01  Z40.4  F0.2;

G01  X35.0  F0.15  M15;

M16;

G01  X41.5  F0.3;

G00  X26.854;

G41  G01  Z40.4  F0.3;

G02  X26.467  Z40.251  R0.2  F0.08;

G01  X26.055  Z39.483  F0.1;

G02  X26.011  Z39.314  R0.65  F0.06;

G40  G01  Z16.0  F0.08;

G00  G97  X25.0  Z26.0  S200;

G04  U1.0;

G00  G97  X24.0  Z80.0  S1000;

G00  T0488  M09;

/ M00;

;

;

N30 (ID  FINISH  GROOVE  NR=0.2);

G00  G97  X37  T0699  S1000  M03;

G00  G96  S200  Z43.5  M08;

G41  G01  Z41.4  F0.3;

X35.55;

G02  X35.15  Z41.2  R0.2  F0.05;

G40  G01  Z40.2  F0.07  M15;

M16;

G01  X35.0  Z40.6  F0.3;

G01  X32.688  F0.2;

G01  X35.15  Z40.2  F0.08;

G04  U0.1;

G01  X35.0  Z40.7  F0.5;

G00  G97  X34.0  Z100.0  S1000  M09;

G00  T0688;

/ M00;

;

N40  (OD  GROOVE  T=3.0  NR=0.3  38.9);

G00  G97  X55.0  T0899  M03;

G00  G96  S160  Z30.575  M08;

G00  X53.0;

G01  X52.0  F0.3;

;

G65  P9005  X43.15  I1.0  F0.1  U0.2;

G01  U0.2  F0.3;

G01  X42.95  F0.05  M15;

M16;

G00  X52.0;

G04  U0.01;

G00  X29.025;

G04  U0.01;

G01  X51.15  F0.2;

G02  X50.15  Z29.525  R0.5  F0.08;

G01  X42.9  F0.12;

;

G00  X51.0  Z29.725;

G04  U0.01;

G00  Z32.125;

G04  U0.01;

G01  X50.445  F0.2;

G03  X49.445  Z31.625  R0.5  F0.08;

G01  X42.9  F0.12;

;

G01  Z29.525  F0.1;

G00  X90.0  Z29.725;

G00  G97  Z80.0  S1000  M09;

G00  T0888;

/ M00;

;

N50   (OD  GROOVE  T=2.0  NR=0.2  47.6);

G00  G97  T0999  M03;

G00  G96  X55.0  Z37.225  S160  M08;

;

G00  X51.0;

;

G65  P9005  X47.875  I0.6  F0.1  U0.2;

G01  U0.2  F0.3;

G01  X47.675  F0.05  M15;

M16;

G00  X51.0;

G04  U0.01;

G00  X36.675;

G04  U0.01;

G01  X50.445  F0.2;

G02  X49.645  Z37.075  R0.4  F0.08;

G01  X47.825  F0.1;

G03  X47.625  Z37.175  R0.1  F0.04;

;

G00  X51.0  Z37.375;

G04  U0.01;

G00  Z37.875;

G04  U0.01;

G01  X50.445  F0.2;

G03  X49.645  Z37.475  R0.4  F0.08;

G01  X47.825  F0.1;

G02  X47.625  Z37.375  R0.4  F0.04;

;

G01  Z37.175  F0.1;

G00  G97  X100.0  Z37.375  S1000;

G00  Z100.0  M09;

G00  T0988;

/ M00;

;

N60 (FACE  GROOVE  T=2.0  NR=0.2);

G00  G97  T1099  M03  S1000;

G00  G96  X51.35  S160  M08;

G00  Z42.5;

G01  Z28.0  F1.0;

G01  Z27.2  F0.1;

G01  W0.2  F0.3;

G01  Z26.9  F0.1;

G01  W0.2  F0.3;

G01  Z26.55  F0.1  M15;

M16;

G00  Z30.5;

G04  U0.01;

G01  Z26.54  F0.8;

;

G00  X51.25  Z28.5;

G04  U0.01;

G00  X52.15;

G04  U0.01;

G01  Z27.675  F0.2;

G02  X51.55  Z27.375  R0.3  F0.05;

G01  Z26.54  F0.08;

G01  X51.15  F0.05;

;

G00  Z50.0  X51.35;

G00  G97  X100.0  Z100.0  S700  M09;

G00  T1088;

G30  U0  W0  T300  M05;

M10;

;

N200;

;

N200;

M01;

M99  P1;

%

Macro Programs

O9031

N10 (FORMAT);

#500=6.85 (T3Z);

#116=#0;

#110=#0;

N20 (LHECK-BLANK);

IF [#508  NE  #0] GOTO 30;

#100=1;

#508=#500;

N30 (CHECK-BLANK);

IF [#100  NE  1] GOTO 50;

#508=#0;

M99;

N50 (CALUCULATION);

#116=#500－#508 (T3Z);

N60 (CHUCK-OFFSET  LIMIT);

IF [ABS [#116  GT  #1] GOTO 3000];

N400 (TRANS-OFFSET);

#2103=#2103+#116*#4 (T3Z);

#2104=#2104+#116*#4 (T4Z);

#2106=#2106+#116*#4 (T6Z);

#2108=#2108+#116*#4 (T8Z);

#2110=#2110+#116*#4 (T10Z);

#508=#0;

M99;

N3000 (ALARM);

#3000=1 (6.85  LIMIT  OVER);

M02;

%

3. Summary

This paper is about the design of flange manufacturing process and the programming of CNC machining flanges, with the purpose of introducing the design method, focusing on strengths and trying to achieve complete and detailed content. The article firstly introduces the analysis of the part and determines the manufacturing form of the blank and the size of the blank according to the processing requirements of the part drawing. Next, the selection of the datum surface is carried out to determine the rough and fine datum in the machining process, and the process route is developed in accordance with the selected datum. Determine the geometry, dimensional accuracy and positional accuracy of the part to achieve the required process. Finally, according to the selected process route to select the equipment, tools, fixtures and preparation of parts processing procedures. The basic requirements, contents, methods and steps of machine manufacturing process design and the discussion of how to prepare the program of CNC lathe, and the program of flange. The size of the machining allowance not only affects the size of the blank of mechanical parts, but also affects the size of the process equipment, the adjustment of equipment, the consumption of materials, the selection of cutting dosage, the number of machining hours. Therefore, the correct determination of machining allowance, for saving metal materials, reduce tool loss, reduce man-hours, thereby reducing product manufacturing costs, to ensure the quality of processing is of great importance.

Source: China Flanges Manufacturer – Yaang Pipe Industry (www.epowermetals.com)