Machining Audit

Printer-friendly versionSend by emailPDF version

Manufacturing components as per drawing at a lesser lead time and reduced cost is essential to ensure competitive production costs, improved quality, performance and longevity of machines.

Reduction in cycle time, competitive production costs, improved quality, performance and longevity of machines, is an important role in enhancing productivity especially in large volume production and need based high value batch production. In the highly competitive market scenario, customers determine the price of a product and entrepreneurs need to continuously fine tune the costs to realize profits. Machine utilization has a major impact in reducing the manufacturing cost of components. Although the material cost cannot be reduced, the cycle time & machining cost can be reduced drastically. For increasing machine on time and improving productivity requires adopting best machining practices. This training course will help CNC users to machine the parts intelligently, problem solving techniques, train and lead people.

In mass production, small inefficiencies pull down the productivity. Only periodic reviewing and revamping of the programs and processes can eliminate the accumulated inefficiencies. These inefficiencies are no reflection on your in-house machining skills and your capability to remedy them.

As we are aware, to produce more and to meet customer expected quantity, need to add more machines which calls for an investment, place, accessories and added man power.

First choice:

Find a machine in a machine: Weed out wasteful tool motions and re-sequence machining operations with the existing state of things. This does not call for any investments. What it needs is a close hard look at the existing state of things and a little course correction.

Ace Micromatic firmly believe in being close to you and assist at various stages during the complete life cycle of your CNC machines.

We understand that your biggest challenge is to continuously improve productivity, efficiency and quality of your end products, so as to remain cost competitive. In our endeavour to address these challenges, the Ace Micromatic Group would like to help you, make the best use of your CNC machines. With expertise and experience, we will show you how to use effectively your machines to maximize productivity and remain competitive.

Our focus is to "help you and making a positive contribution to your Business” to increase productivity & OEE.

As you are aware Ace Micromatic Group is manufacturer of Turning Centres, Machining Centres and CNC Grinding. Each products are used for its unique application capabilities.

Most common application on Turning Centers are:

General Turning

  • External
  • Internal

Grooving

  • OD grooving
  • ID grooving
  • Face grooving

Threading

  • External
  • Internal

Drilling

In this edition we will talk about Threading on Turning Centres and factors influencing the following:

Tool life Less than recommended Insert breakage / Chip off Abnormal wear
Cycle time Run time for a given component, cycle start to M30 But average cycle time of a batch may not be actual cycle time a single part machined. You need to look in to that, which factors are contributing in reducing total efficiency and take action plan to eliminate/improve.
Quality and aesthetic of part produces Machining part as per drawing dimensions. Even though dimensions are with in limit but aesthetically may not be good. You need to look in to that, which factors are affecting the quality and aesthetic of part and take action plan to eliminate/improve.
Operators interventions Operator's interventions in production is the major cause of reducing productivity and morale of operators. Insert breakages Chip breaking issues Frequent/unscheduled insert change GD & T repeatability problems Accidents due to improper cutting methods You need to relook on the process/method which can eliminate operator's intervention in production activities.
Machine, cutting tool and work hols abuse Improper tool entry/exit. Input material stock/size variations Improper cutting tools

Purpose

Peripheral

  1. Enable us to visualize the:
    • Existing process
    • Machining techniques
    • Resources (cutting tools, work holding, machines)
  2. 2. Provide us the inputs for:
    • Improvements
      • Bench mark the cycle time
      • Best utilization to cutting tools & machines
      • Man power efficiency
      • Machine shop capacity
      • Quality of parts machined
      • Safety
      • On time delivery
  3. 3. Help you to prepare road map for continual improvements

Our worksheets and method of analysing data collected from existing machining will help you to audit the existing machining method and make necessary correction if there is scope for improvements.

Auditing data collected from existing process

Tool life in threading applications:

Inserts life determined by contact time, cutting method and cutting parameters used, if machining is under ideal conditions. We need suitable grade of inserts, anvil and ID or OD insert to perform the threading operation. Unnoticed small inefficiencies will pull down production and increase cost per part because of increased down time and high tool consumption.

Thread choice:

 

 

Full profile thread

Partial profile thread

Preparation:

Before doing threading operation we need to prepare OD/ID for External/internal thread.

Thread height and major/minor diameter of external/internal thread in full profile thread controlled by insert as shown in the picture. Hence control of pre turned diameter in external thread and pre bore diameter in internal thread is very important.

Excess material left on OD/ID will rubbed or peeled by full profile insert hence produce sharp edge or burr on thread also reduces tool life.

Solution:

  • Pre turned diameter must be maintained with in ±0.02.

  • Periodically checked and corrected.

  • Difference of major diameter and minor must be equal to thread height as per insert for the given thread.

  • Control X offset of threading tool.

Preparation:

During partial thread major diameter in external thread and minor diameter in internal thread are having a wider tolerance.

For external thread major diameter will be lessor than nominal diameter.

For internal thread minor diameter will be bigger than nominal diameter.

Example: M20 x 2 pitch

Solution:

  • Find average Diameter for major & minor diameter and fix tolerance of ±0.05.

  • Periodically checked and corrected.

  • Control X offset of threading tool.

 

 

ISO metric thread Pitch cutting methods

0.5

0.75

1.0

1.25

1.5

1.75

2

2.5

3

3.5

4

4.5

5

5.5

6

In smaller pitch thread height is smaller (0.63 * Pitch). If we use flank entry, thread base get weaken and possibility of thread tear can happen.

 

Better chip flow and improved tool life

 

 

Better chip flow, improved tool life and reduced insert contact length.

Thread on the following materials:

Brittle

Tensile

Soft

  • Do not use idle passes in brittle material, since the material won’t deform while threading.

  • Since the brittle materials abrasive in nature, idle passes will reduce insert life.

  • Use average cutting speed (Vc)

  • Use only one idle pass, more idle passes may lead to work hardening, built-up edge and reduce insert life.

  • If you are using flank entry method and zig zag method, do not use finishing allowance. By using finishing allowance the final cut happened at centre of thread and both edges of inserts engage and results in chattering, reduced insert life, sharp edges and burr on thread.

  • Use average and above cutting speed (Vc)

  • Do not use idle pass, using idle passes may lead to work hardening, built-up edge and reduce insert life.

  • If you are using flank entry method and zig zag method, do not use finishing allowance. By using finishing allowance the final cut happened at centre of thread and both edges of inserts engage and results in chattering, reduced insert life, sharp edges and burr on thread.

  • Use maximum recommended cutting speed. (Vc)

Optimum threading cycle parameter for FANUC on the basis of Pitch:

Pitch

 

Program format for FANUC

0.5

Q1=30 Q2=100

G76 P010060 Q1 R0

G76 X Z P Q2 F

Q1= Minimum depth of cut

Q2= First depth of cut

Use Q1 and Q2 under 1:4 ration

 

Note:

  • Idle passes and Q values determine the insert life

  • Values given are subject to machine, work hold, tool used and material condition

0.75

Q1=40 Q2=110

1.0

Q1=50 Q2=120

1.25

Q1=60 Q2=140

1.5

Q1=70 Q2=180

1.75

Q1=70 Q2=200

2.0

Q1=70 Q2=220

2.5

Q1=80 Q2=250

3.0

Q1=90 Q2=300

3.5

Q1=100 Q2=350

4.0

Q1=100 Q2=375

4.5

Q1=110 Q2=400

5.0

Q1=110 Q2= 400

5.5

Q1=120 Q2=420

6.0

Q1=120 Q2=500

Add new comment

Filtered HTML

  • Web page addresses and e-mail addresses turn into links automatically.
  • Allowed HTML tags: <a> <em> <strong> <cite> <blockquote> <code> <ul> <ol> <li> <dl> <dt> <dd>
  • Lines and paragraphs break automatically.

Plain text

  • No HTML tags allowed.
  • Web page addresses and e-mail addresses turn into links automatically.
  • Lines and paragraphs break automatically.