Machining process of flange parts

With the continuous development of science and technology, the quality and productivity of mechanical products have been increasingly demanding. Automation of machining process is one of the most important measures to achieve the above requirements. It can not only improve the quality of products, increase production efficiency and reduce production costs, but also greatly reduce the labor intensity of workers. 

In recent years, due to the increasingly fierce competition in the market, in order to survive and develop in the competition, the production and processing enterprises not only to improve product quality, but also must continue to improve and shorten the production cycle to meet the changing needs of the market. Computer-controlled CNC machine tools of high precision, highly flexible and suitable for processing complex parts performance, just to meet the needs of today’s market fierce competition and process development. It can be said that the application of computer numerical control technology is a sign of advanced production technology in the machinery manufacturing industry, to a large extent, determines the success or failure of enterprises in the market competition.
In recent years, due to the increasingly fierce competition in the market, each production not only to improve the quality of products, but also to meet the changing needs of the market for frequent improvements. Therefore, even the mass production, but also to change the product long-term unchanging practice. This is the combination of machine tools, automated machine tools and automated production lines in mass production is also increasingly exposed to its shortcomings or shortcomings. In order to solve these problems, a new type of digital program-controlled machine tools came into being, it is extremely effective in solving the above series of production conditions restrictions, for single-piece, small batch production of precision and complex parts to provide automated processing means.
In recent years, the speed of development in China’s machinery manufacturing industry has been rapidly changing, especially the introduction of high-tech and the development of the application of CNC machine tools, the need for a large number of CNC programmers and process designers. For the application of CNC technology, employers need highly skilled CNC programming technical personnel, to become a qualified mechanical processing technicians, must master the machinery manufacturing process, can specify a qualified process protocol and qualified CNC program, how to develop a reasonable processing route and the parameters of processing directly affects the quality and efficiency of parts processing and cost.

Machining process of flange parts

Figure.1 shows the flange parts, the material is HT200. the flange parts in the CNC milling processing has a certain representative, processing, in the premise of ensuring quality, should try to improve productivity and reduce costs, so not necessarily all by CNC machine tools, simple surface by ordinary machine tools to complete.

20211013103502 37552 - Machining process of flange parts

Figure.1 Drawing of flange parts

Part drawing process analysis

For the process analysis of this part, the main aspects are structural shape, dimensions and technical requirements, positioning reference and blank material. The machined surface of the part consists of the tab plane, the central hole Φ40 and 2-Φ22 countersunk holes, and 2-Φ13 through holes: the dimensions are completely marked and the geometric conditions are adequate. The surface roughness of the Φ40 bore is Ra1.6um, the roughness of the two countersunk holes and the through-hole is Ra12.5um, and the roughness of the rest of the surface is Ra3.2um. Bring in the mechanical gap due to machine wear, processing to pay attention to the backlash compensation. In the CNC milling machine processing is a manual tool change, not only will reduce productivity, but also will add a lot of trouble to the programming, at the same time, because of the tool change increased the parts of the processing of the tool joint difference, thereby reducing the quality of parts processing. So try to reduce the number of tool changes. The material of the part is HT200, with good cutting performance.

The choice of CNC machining content

Compared with ordinary milling machine, CNC milling machine has the characteristics of high processing accuracy, complex shape of the processed parts, and wide processing range. However, the price of CNC milling machine is higher, the processing technology is complicated, and the manufacturing cost of the parts is higher. Therefore, it is necessary to correctly select the content suitable for CNC milling.
Ordinary machine tools can not be processed or processing difficulty, the quality of the content is difficult to ensure the priority of CNC machining as the content. For ordinary machine tools can be processed but the processing efficiency is low, and can be used in CNC machine tools when processing other surfaces incidental to the processing of the content of CNC machining. For example, the part on the two Φ 22 countersunk holes and two Φ except 13 through hole itself size and processing accuracy requirements are not high, but in order to reduce the process equipment, improve efficiency, can be in the CNC milling machine incidental processing completed. Except for the bottom surface, which is milled on the general machine tool, the rest of the machining parts need to be milled by CNC machine tool.

To determine the processing program

According to the above analysis, the center hole Φ40 of the flange part has a high surface roughness requirement, so it should be finished in two stages with rough and finish machining respectively. Φ40 hole is finished by three work steps: drilling – rough boring – finish boring method, and the upper surface profile of the part is finished by rough and finish milling. In addition, since the workpiece blank is a casting part, the machining allowance is large and the deformation in the machining is large, so the method of separate rough and finish machining is also suitable.

Machining of the flat surface

Since the surface of the upper plane A is machined by removing the material, it is required to use two machining solutions of roughing and finishing to ensure the accuracy of standard tolerance IT8. Roughing and finishing milling because of the difference between roughing and finishing milling in the choice of inserts, two tools are used for roughing and finishing respectively. When roughing, try to use a larger feed, a larger back draft, and a higher cutting speed. In order to ensure the surface roughness and dimensional accuracy during finishing, smaller feed, smaller back draft and larger cutting speed should be used. To ensure the durability of the tool and surface roughness and reduce the processing temperature to use cutting fluid for cooling.

Processing of hole system

By analyzing the drawing of the part, we can see that the dimensional accuracy and position reading accuracy of the hole system in the drawing of the part are very strict, so we must use reasonable processing methods when machining to ensure both the dimensional accuracy and the position accuracy of the part.
When drilling the hole, the feed should be small, and only after the cutting part of the drill bit has entered the workpiece can it be drilled normally. When drilling small holes or deeper holes, the drill must often be withdrawn from clear cutting to prevent the drill bit from being “bitten” or broken due to chip blockage. When drilling steel, the cutting fluid must be fully poured to cool the drill bit to prevent the drill bit from annealing.

Blank size and material characteristics analysis

From the blank drawing, the parts to be processed are made of HT200 with 170 \110 \50mm, which is a good material with good processing performance.

Determine the positioning clamping program

The choice of positioning datum

In order to process all the surfaces to be machined in one clamping, in addition to following the principle of selecting the positioning datum, it is best to select the plane or hole that does not require CNC milling as the positioning datum, and pay attention to the selected positioning datum should be conducive to improving the rigidity of the workpiece. The lower surface B surface of the part is selected as the positioning reference surface.

The choice of fixture

The basic principle of selecting fixture
CNC machining characteristics of the fixture put forward two basic requirements: one is to ensure that the fixture coordinate direction and the machine tool coordinate direction relative fixed; second is to coordinate the size of the part and machine coordinate system relationship. In addition, the following points should be considered.

  • (1) When the parts are processed in small batches, should try to use the combination of fixtures, adjustable fixtures and other general-purpose fixtures to shorten production preparation time, save production costs.
  • (2) In batch production before considering the use of special fixtures, and strive to simple structure.
  • (3) The loading and unloading of parts should be fast, convenient, reliable, in order to shorten the machine downtime.
  • (4) Fixture on the parts should not prevent the machine tool to the parts of the surface processing, that is, the fixture to open, its positioning, clamping mechanism components can not affect the processing of the tool (such as collision, etc.).

Types of fixtures

CNC lathe fixture mainly has two types: one for disk or short shaft parts, the workpiece blank clamped in the chuck with adjustable jaws (three jaws, four jaws), by the chuck drive rotation; the other for shaft parts, the blank mounted on the spindle top and tailstock top between the workpiece by the spindle toggle chuck drive rotation.
CNC milling machine fixture, generally mounted on the table, its form according to the characteristics of the workpiece being processed can be a variety of. Such as: universal table vise, CNC indexing rotary table, etc..
According to the structural characteristics of the part to choose the vise fixture.

Selection of tools

The material of the part (cast iron) belongs to the general material, cutting performance is good. Selection of tool materials, rough machining is generally used high-speed steel, finishing alloy steel. General milling plane, in roughing to reduce the cutting force, the milling cutter diameter should be smaller, but not too small, so as not to affect the processing efficiency, in finishing to reduce the traces of the joint, the milling cutter diameter should be larger. Since the B surface is a rectangle of 160mm*100mm, the size is not large and there is a hole of φ60mm in the center, so the diameter of the rough and finish milling cutter should be greater than or equal to half of the width of the B surface, and the end mill with the diameter of φ50mm can be selected. When processing the center hole of 40H7, the scheme of drilling-rough boring-finishing boring is used, so φ3mm center drill, φ38mm twist drill, φ39.5mm rough boring cutter and φ40H7mm finishing boring cutter should be selected. Because it is a single-piece small batch production, the single-edge boring tool is chosen. The surface roughness of the drilled hole is Ra12.5mm, and the tolerance grade is about IT12, which is just in line with the roughness requirements of 2-φ13 and 2-φ22, so the drill is selected for processing these holes. The specific selected tools are shown in Table.3.

Table.3 CNC machining tool card

Work step No

Tool number

Tool name

Tool handle model

Diameter/mm

Tool radius compensation number

1

T01

End mill φ20mm

BT40-XM33-75

φ20

H01

2

T02

Flat end milling cutter in φ 50 mm

BT40-TQC50-180

φ50

 

3

T03

Center drill φ 3 mm

BT40-TQC50-180

φ3

 

4

T04

Drilling bit φ38

BT40-TW50-140

φ38

 

5

T05

Drilling bit φ13 mm

BT40-Z10-45

φ13

 

6

T06

Rough boring cutter φ39.5 mm

BT40-M1-45

φ39.5

 

7

T07

Fine boring cutter φ40 mm

BT40- M1-45

φ40

 

8

T08

Flat bit φ22 mm

BT40-MW2-55

φ22

Determine the machining order

The machining sequence is determined according to the principle of primary then secondary, coarse then fine. Therefore, the external contour size used as the positioning reference, the lower bottom surface used as the positioning reference and the 2-22 countersunk holes and 2-13 through holes are machined first to provide a stable and reliable positioning reference for CNC machining. The specific machining sequence is shown in the table.
Table.1 CNC machining process card

 

NC machining process card

Product name or code

Part name

Material

Part drawing No

 

 

 

Flamge

HT200

 

Operation No

Program number

Fixture name

Fixture No

Use equipment

Workshop

 

 

Bench clamp

 

 

 

Work step No

Work step content

Machining surface

Tool number

Tool specification / mm

Spindle speed / (r / mm)

Feed rate/(mm/min

Back cut/mm

Note

1

Rough milling surface B outer contour to dimension

Outer contour

T01

20

800

150

First 10, second 8

 

2

Milling boss

Boss

T02

50

800

150

First, second 8, third 2

 

3

Drill Φ 40h7 center hole, 2* Φ 22 * 10mm hole, center hole

 

 

Central hole

 

 

T03

3

800

100

 

 

3

 

4

Drill Φ 40h7 hole to 38

Drilling

T04

35

600

80

 40

 

5

Drill Φ 13 holes

Drilling

T05

13

800

80

 22

 

6

Rough boring Φ 40h7 to 39.5

Boring

T06

38

800

80

 40

 

7

Fine boring Φ 40h7 hole

Boring

T07

39.5

800

50

 40

 

8

Spot facer 2* Φ 22 * 10 holes

Spot facer

T08

22

800

100

 10

Table.2 Flange parts mechanical machining process

Serial number

Process name

Process content

Equipment and tooling

1

Casting

The blank shall be made with a unilateral allowance of 3-5mm for each part except the surrounding sides

 

2

Clamp

Mark the whole line and check it

 

3

Milling

Rough and finish milling face a; No allowance is left for rough milling surface B

Ordinary milling machine

4

NC machining

Finish milling surface B and machining each hole

Vertical CNC milling machine

5

Clamp

Deburring

 

6

Test

 

The selection of the cutting amount

The selection of the cutting amount should be fully considered the machining accuracy of the part, surface roughness and tool strength, rigidity and machining efficiency and other factors. Cutting amount is an important parameter that indicates the size of the main motion and feed movement of the machine tool. Choose a good cutting amount, so that the depth of cut, spindle speed and feed rate between the three can coordinate with each other, mutual adaptation, in order to form the best cutting parameters.

The depth of cut is determined

When the rigidity of the process system allows, as far as possible to choose a larger depth of cut, in order to reduce the number of tool walking, improve productivity. Rough machining, after leaving the finishing, semi-finishing margin, as far as possible, a tool will be removed the remaining margin. The first cutter as large as possible, so that the cutter in the inner cutting, to avoid the surface of the workpiece is not flat and have a hard skin castings and forgings.

Programming

Machining process

  • 1. Rough and finish milling of the upper surface;
  • 2. Rough and finish milling 60 outer circle and its steps;
  • 3. Drill the center hole
  • 4. Drilling 40 bottom hole;
  • 5. Rough boring 40 bore;
  • 6. Drill 2*13 holes;
  • 7. Rough and finish milling outer contour;
  • 8. Countersink 2*22 holes.                                        

Procedure

Rough milling outer contour

G54 G00 X0 Y0 Z50 //Enter the machining coordinate system
M03 S800 T1 //Spindle start, select Φ20mm end mill
G90 G17 X-90 Y20 //From the starting point to the starting point of machining
Z0 //Down cutter to the upper surface of the part
G01 Z-10 F150 //Down cutter depth -10mm
G42 G01 X-80 Y0 F200 H01 //Start tool radius compensation
G03 X-69.245 Y-17.735 R20 //Mill outer contour R20 (third quadrant)
G01 X-13.867 Y-46.602 //Milling straight lines (third quadrant)
G03 X13.867 Y-46.602 R30 //Milling outer contour R30 (fourth quadrant)
G01 X69.245 Y-17.735 //Milling straight line (fourth quadrant)
G03 X69.245 Y17.735 R20 //Milling outer contour R20 (first quadrant)
G01 X13.867 Y46.602 //Milling a straight line (first quadrant)
G03 X-13.867 Y-46.602 R30 //Milling outer contour R30 (second quadrant)
G01 X-69.245 Y17.735 //Milling a straight line (second quadrant)
G03 X-80 Y0 R20 //Milling outer contour R20 (third quadrant)
G01 X-80 Y-10 //Cut out the part
G01 G40 X-90 Y20 //Cancel tool compensation
G00 Z50 //Z-direction tool lift
X50 Y50 M02 //Return to the origin of the machining coordinate system, end

Rough and finish milling Φ60mm outer circle and cams

G54 X0 Y0 Z50 //Enter the machining coordinate system
T2 //Select Φ50mm flat bottom tool
M03 S800 //Start the spindle. 
G90 G01 Z-8 F150 //Z downward tool depth 8mm
G03 X-80 Y-10 I0 F200 //Rough milling Φ60mm outer circle and tab
G00 Z50 //Lift tool
G01 Z-16 F200 //Second cutting depth 8mm
G03 X-80 Y-10 F200 //Rough milling Φ60mm outer circle and boss
G00 Z50 //Lift tool
G01 Z-18 F200 //Down cut 2mm, start finish machining     
G03 X-80 Y-10 //Finish milling Φ60mm outer circle and boss
G00 Z50 //Z-direction tool lift
X0 Y0 M02 //Return to the origin of the machining coordinate system, end

To perform hole machining

G54 G90 X0 Y0 Z0 F200 //Enter the machining coordinate system
T3                               
M08 //Cutting fluid open 
M03 S800 //Spindle start
G98 G81 X0 Y0 Z-3 F100 //Drill center hole
X60 Y0 //Drill center hole
X-60 Y0 //Drill center hole
G01 Z100 // Lift tool
M09 // Chip fluid off
X100 Y100 // Back up to the tool change point 
TO4 // Select Φ38 drill bit
M03 S800 // Spindle start
M08 // Chip fluid on 
G99 G73 X0 Y0 Z-45 R10 Q5 F80 //Select high-speed deep hole drilling method for Φ40 hole
G01 Z100 // Tool lifting
M09 // Chip fluid off
X100 Y100 //return to the tool change point 
T5 //Change to tool T5 (Φ13 drill bit)
M03 S800 // Spindle start
M08 //Chip fluid on
G98G73 X-60Y0Z-45R10F80 //Select high-speed deep hole drilling method for Φ13 hole 1
G73 X60 Y0 Z-45R10F80 //Select high speed deep hole drilling method for Φ13 hole2
G01 Z100 // Return to the starting point of Z-direction  
M09 // Chip fluid off 
X100 Y100 //return to the tool change point
T6 // change to tool T6 (Φ39.5 boring tool)
M03 S800 // Spindle start
M08 //Chip fluid on
G99 G86 X0 Y0 Z-42 R10 F80 //Select rough boring method for 40 holes
G01 Z100 // Tool lift
M09 // Chip fluid off 
X100 Y100 //Return to tool change point
T7 //Change to T7 (Φ40 boring tool)
M03 S800 // Spindle start
M08 //Chip fluid on
G76 X0 Y0 Z-42R10 Q2 F50 //Finish machining Φ40 hole 
G01 Z100 // Tool lifting
M09 // Chip fluid off 
X100 Y100 // Retreat to the tool change point
T8 //Change to tool T8 (Φ22 flat drill bit)
M03 S800 // Spindle start
M08 //Chip fluid on
G99 G81 X-60 Y0 Z-30 R10 Q3 F100 // Machining Φ22 hole (right side)
G98 G81 X60 Y0 Z-30 R10 Q3 F100 //Machining hole of Φ22 (left side)
G00 Z100 // Lift the tool
M09 // Chip fluid off
G00 X100 Y100 // Return to tool change point 
M05 M30 // Spindle stop, end of program

Operation points and analysis

Operation points

  • 1. The part is clamped by ordinary precision flat vise.
  • 2. Before machining, the part must be corrected by using a percentage table in the vice.
  • 3. The workpiece must be mounted in the vise to reveal the vise more than 25mm.
  • 4. In the clamping to be in the lower plane of the vise on the pad of two equal height pad iron, to prevent damage to the vise drill or boring tool when punching. And no debris is allowed on the contour pads to ensure parallel to the table.
  • 5. Choose a large diameter disc milling cutter to process the upper surface of the part to improve processing efficiency.
  • 6. When processing each hole, you should first choose the center drill for positioning, not directly with a drill to hit the bottom hole, and then in the choice of a suitable drill to hit the bottom hole, for the strict requirements of dimensional accuracy but also reaming and reaming, the location of high requirements but also boring processing.
  • 7. Be able to use trigonometric functions or plane geometry to calculate the nodes.
  • 8. Wipe clean the surface of the toolholder when changing the tool without chips.

Analysis of the main points

  • 1. The processing of this part requires only single-sided processing.
  • 2. Use a large diameter disc milling cutter to improve efficiency.
  • 3The purpose of using small diameter milling cutter and spiral groove milling cutter is to increase the speed so as to ensure the surface roughness and prevent tool interference.
  • 4. Rough machining as far as possible to use the reverse milling, finishing as far as possible to use the way of milling.
  • 5. Choose the correct tool setting point and correct tool setting method to minimize the positioning error and ensure the position accuracy.
  • 6. Complete all machining with one tool setting.
  • 7. The tool setting instrument should be accurate in measuring the tool length.

Conclusion

This design is aimed at applying as much knowledge as possible and applying advanced automatic production technology, so we have been strict with ourselves from the very beginning, put a lot of effort and treated it with a serious and rigorous attitude. Since any negligence or mistake in the design will affect the processing of the actual parts, we insisted on determining the size of each structure, calculating the data and selecting the parameters as accurately and reasonably as possible, and asked the teachers and factory workers to check and correct them, and proposed our own design solutions to discuss with our classmates to make them more reasonable and reliable.
I am deeply aware that this design has an extremely important role for us to go to work in society:

  • 1. Cultivate our comprehensive use of the knowledge we have learned, the ability to solve practical problems, so that their knowledge to consolidate and improve.

  • 2. Basically mastered the operation of general CNC machine tools and cultivated our ability to complete tasks independently and work together with classmates.

  • 3. Have a systematic summary and application of the knowledge learned during school. Clearly understand the tasks and skills as a CNC technician, and have a clear understanding of the whole CNC technology. From the site observation, access to information, drawing assembly diagrams to processing workpieces and other links have a certain personal experience for the future work laid a good foundation.

  • 4. Cultivated my own hard-working spirit and careful and rigorous working attitude. In this design, the time is tight, the task is heavy, we dare not have the slightest slack, every point, every place to strive to achieve accurate and reasonable. Through this personal design, I deeply appreciate that in order to be a real CNC technician, we must be careful, serious, rigorous and humble, because any little negligence or slackness may bring great trouble to the production and cause great loss to the enterprise.

In addition, due to our limited ability, it is impossible to do perfection, and there are inevitably unreasonable or unsatisfactory places in this design. Therefore, we sincerely ask for your criticism and guidance, so that we can be able to do our best in the actual production activities in the future.

Source: China Flange Manufacturer – Yaang Pipe Industry (www.steeljrv.com)

(Yaang Pipe Industry is a leading manufacturer and supplier of nickel alloy and stainless steel products, including Super Duplex Stainless Steel Flanges, Stainless Steel Flanges, Stainless Steel Pipe Fittings, Stainless Steel Pipe. Yaang products are widely used in Shipbuilding, Nuclear power, Marine engineering, Petroleum, Chemical, Mining, Sewage treatment, Natural gas and Pressure vessels and other industries.)

If you want to have more information about the article or you want to share your opinion with us, contact us at sales@steeljrv.com
Please notice that you might be interested in the other technical articles we’ve published:

Related News

العربيةБългарски简体中文繁體中文DanskNederlandsEnglishFrançaisDeutschBahasa IndonesiaItaliano日本語한국어LatinPortuguêsРусскийEspañolதமிழ்ไทยTürkçe