Mm3216 milling tutorial

CNC Milling
MM3216 Computer Aided Machining

Prepared by Mok Chai Pui

School of Mechanical and
Aeronautical Engineering

Unit 1
Essentials of CNC Milling


Machine Information







MAZAKTROL MATRIX
NEXUS 410A-II Vertical
Machining Centre
X560 mm, Y410 mm, Z 510
mm
30 tools tool magazine
Maximum rotating speed is
12000 rpm


Machine Axes and Coordinates








3 mutually perpendicular
axes
Table movement by X and Y
axes.
Spindle movement on Z axis.

http://www.youtube.com/watch?v=AKwlzIJG5lo


Basics of Milling






Milling is performed with a rotating,
multi-edged cutting tool which
performs programmed feed
movements against a workpiece in
almost any direction.
Each of the cutting edges remove a
certain amount of metal, with a limited
in-cut engagement, making chip
formation and evacuation a secondary
concern.
Milling is applied to generate flat faces,
in most cases. However, with 5-axis
machines and form cutters, it can cut
in many shapes and forms.

What is a machine Coordinates System, MCS?




It refers to the physical
limits of the motion of the
machine in each of its
axes and the numerical
coordinate which is
assigned (by the machine
tool builder) to each of
these limits.
A reference point for the
workpiece coordinate
system to refer to.


What is a workpiece Coordinates System,
WCS?




Used to define the geometrical
shape and size of the workpiece
with all dimensions referring to
the zero point.
Defines the intersecting zero
point, X=0, Y=0 and Z=0


Workpiece Coordinates System (WCS)
Settings and Programming








6 workpiece coordinates
systems (G54 to G59)
Every workpiece need to
set its own WCS using the
work offsets.
The work offsets registers
the distance from the MCS
to WCS for each axis.
http://www.youtube.com/watch?v=EI2inCb0Wfs


Relationship of Workpiece Coordinate System
(WCS) to Machine Coordinate System (MCS)


In CNC machining, it is necessary to register the
position of the workpiece zero point (X,Y,Z) with
reference to the machine zero-point (X,Y,Z). This is to
enable the machine to locate the position of the
workpiece to the machining zone.


Tutorial
Standing in front of the machine, if you want to bring the
workpiece TOWARDS YOU, you have to move the table
in the
(a)
(c)

+X direction
+Y direction

(b)
(d)


-X direction
-Y direction

Tutorial
tool TO THE LEFT, you have to move the table in the
(a)
(c)

+X direction
+Y direction

(b)
(d)


-X direction
-Y direction

Tutorial
tool TOWARDS YOU, you have to move the table in the
(a)
(c)

+X direction
+Y direction

(b)
(d)


-X direction
-Y direction

Tutorial
workpiece TO THE RIGHT, you have to move the table in
the
(a)
(c)

+X direction
+Y direction

(b)
(d)


-X direction
-Y direction

Tutorial


Drilling of a hole involves only one axis, which is the
_______ axis.
Z



Profile milling involves two axes movement
simultaneously; the two axes are ____ and _____ axis.
X
Y


Tutorial


How does the machine locate the workpiece when
executing NC programs?



After established the relationship between the WCS
and MCS, the workpiece is located using any one of
the 6 coordinate systems, G54, G55 …… G59.


Tutorial
When executing a CNC program to cut a part on a 3-axis
CNC milling machine, we can observe that the
(a)
machine table moves according to the
programmed path.
(b) machine spindle moves according to the
programmed path.
(c) machine spindle and the machine table move
simultaneously according to the programmed path.
(d) machine spindle and the machine table move
sequentially according to the programmed path.


Unit 2
Face Milling & Profile Milling


Face Milling Process






Applied to generate flat
faces.
One or more of the following
cutting actions will be
involved:
 Radial
 Peripheral
 Axial
Face milling is on the
periphery with some extent
on the tool.

Speeds




Cutting Speed, m/min
 The surface speed at which the cutting edges pass the
workpiece surface. It depends on tool and work
material used. Parameters are available from
catalogues and handbooks.
Spindle Speed, rpm
 The number of revolutions at which the milling cutter
rotates on the spindle per minute.

πDN
Vc =
1000

Tutorial

39.27 m/min

509 rpm


Feed






Feed/tooth, mm/tooth
 It depends on the recommended maximum chip
thickness value that the tool removes for a specific
work material.
Number of teeth
 Available number of teeth on a milling cutter, it
depends on the diameter of the cutter. It is used to
calculate table feed.
Feed/minute, mm/min
 Also known as table feed,
 Feed/min=feed/tooth x no. of teeth x rpm

Tutorial


A 45 mm diameter end mill with 4 flutes is used in a
face milling operation. If the recommended spindle
speed is 2450 rpm and the feed rate is 0.05 mm/tooth.
What is the feed rate in mm/min?
Feed (mm/min)=rpm *feed/tooth * no. of teeth
Feed = 2450 * 0.05 * 4
Feed = 490 mm/min



A 16 mm wide slot is milled using an end mill of the
same diameter. The length of the slot is 86.5 mm. If
the feed rate is 200 mm/min, what is the required
machining time to finish the slot?
Time required to cut = 86.5*60/200 = 25.95 seconds.

What are some of the considerations when
performing face milling operation?












Include a small radial corner when changing
direction.
Keep the tool in full contact with the workpiece while
cutting.
As the tool enters and exits cutting edges, it may
break the inserts.
Avoid milling over holes.
Machine holes after the facing operation.
Reduce the recommended feed rate by 50% when
cutting workpieces with holes.
Avoid dwell and chatter.

Contour Milling (Profile Milling)




Cutting along the contour of a workpiece which may
consists of lines and arcs.
Depth of cut remains constant in 2D contours.


What is approach and retract?










Approach and retract profile parameters are also called
engage and disengage or lead-in and lead-out.
The value selected is crucial and usually set tangential to
the first point of cut and last point of cut.
The approach parameter is used to specify the line length
and arc radius for the tool to enter the machining
boundary.
The retract parameter is used to specify the line length and
arc radius for the tool to leave the machining boundary.
It is important to plan how the cutter will make initial
contact with the workpiece.


How many types of approach and retract?


There are three common ways for
the cutter to enter and leave the
workpiece:
 without approach or retract.
 with approach and retract using
arcs modes.
 with approach and retract using
arcs and lengths modes.


What could be the problem when there is no
retract and approach?






The cutter will start plunging directly at the start
point of the contour cut.
End Mill will break if there is no cutting edge at the
centre.
Cutter mark will be left on contour as there is a
momentarily stop at the start/end point of the
contour. The tool has to stop the movement in the
axial direction before picking up the feed rate of
the contour cut.


Circular Approach & Retract









Normally starts and ends at the midpoint of an entity if it is a closed
contour
Circular arc is usually of 90o movement
Depends on the radius of
approach/retract, the tool will plunge
outside the job
There is a smooth transition when
approach and exit from the contour. A
good surface finish could be attained.
Distinct positions for approach and
retract

Approach and Retract with Circular arc and
straight line moves




Similar benefits as in the circular approach and
retract method
Start and Exit can be at the same position. A predrilled hole could be made to facilitate the cutter
plunging if necessary.


(Straight Line) Approach and Retract for open
profile



Tool starts and exits away from the contour
Straight line tangential to the entry/exit geometry.
This avoids cutter mark on the workpiece


What is Cutter Compensation?










Cutter compensation is also called tool position or
offset.
Important when performing contour milling or profile
milling.
The cutter centre is offset to the specified side of the
programmed path with a value that is entered into the
control.
With this, the programmer is able to program the
profile of the workpiece without considering the
diameter of the tool used.
Different diameters of tools can be used for the
machining operation without affecting the program.

Example of cutter compensation








To produce a part 80mm
square.
Using tool of 25 mm dia.
Toolpath running along an
80 mm square.

http://www.youtube.com/watch?v=EVlm8aOtk6I


Example of cutter compensation








The actual tool will never be exactly 25mm dia. The
part will therefore end up with different dimensions.
The programmer does not know what exactly is the
tool size
The tool size is dynamically changing due to cutter
wear.
Nominal size 25mm tool may not be available at the
shop floor. It may have been signed out by other
users


Cutter compensation G41


Tool left, (G41): the
cutting edge of the tool
to the left side of the
workpiece contour.


Cutter compensation G42




Tool right (G42): the cutting
edge of the tool to the right
side of the workpiece
contour.
Tool on, (G40): the cutter
centre moves on the
workpiece contour. This will
result in undersize
workpiece produced.
Application example
include: slot cutting,
engraving.




Compensated tool path








Cutter dia 25mm, offset value is
12.5mm
Reference to the workpiece zero
point, w/p corner is 27.5 mm away.
With no offset, the cutter will move
to X-27.5, the size of the workpiece
will be reduced.
With offset, the cutter will move to
X-40 to produce correct size of the
workpiece.


Explain what is stepover distance?








Each roughing method uses a stepover value. The
stepover specifies the amount the tool moves over for
each cut in the roughing toolpath.
You can enter a stepover value as either a percentage or a
distance.
When you set a stepover percentage, a good starting
point is 50% to 75% of the tool tip (or minor) diameter.
The stepover distance shows how large a step is being
taken.


Effect of stepover distance




A wide stepover distance, there will be lesser passes
and machining time will be shorter. To an extent, there
may be uncut material left behind.
A narrower stepover distance, there will be more
passes and machining time will be longer.


Tutorial


A student has to carry out a Face milling and Contour
Milling on a workpiece of size about 100 x 100mm.
T03 (Ø16 endmill) is to be used in contour milling. He
claims that he can achieve time saving by using the
same tool to do the face milling as there is no tool
change is required. Comment on the student’s claim.



With a 60mm Face Mill, 4 passes will be required to cover the
whole area with default setting on MasterCam.
With a 16mm Endmill, 10 passes will be required to cover the
whole area with default setting on MasterCam. This leads to a
much longer machining time for the facing operation.




Tutorial


The Aluminum part shown has to be machined from a
rectangular stock. Student ‘A’ suggests to mill the
steps prior to drilling. Student ‘B’ says that it is better
to drill all the holes first followed by milling of steps.
Evaluate the pros and cons of the two approaches.


Solution






Student ‘B’ – Drill all the holes prior to milling of steps
It could be a little easier for programming as drilling all start at
the same plane. There is no worry that the drill will hit the
shoulder on the stepped block. However, the drilling time will be
much longer as all 3 holes are equally deep. When the milling
cutter cuts over the holes, interrupted cuts occur. This leads to
chattering and shorten tool life.
Student ‘A’ – Mill steps prior to drilling
This is the preferred planning. It leads to shorter processing
time and better tool life in both drilling and milling operations.
The student has to make sure that there is sufficient retraction
distance to avoid the drill collision with the stepped block.


Tutorial


An experienced process engineer
said that it is no good to use
Ø16mm endmill to do the contour
cut on the following alumimum
part shown below. Explain what
could be his reasons. What is the
recommended tool diameter to be
used?


Solution




The smallest radius on the profile is R8. This means
that the Ø16 endmill will be in full contact with the
part when performing contour cut at that position. An
excessive contact area between the tool and the
workpiece leads to vibration and poor surface finish.
It will also be difficult to control the dimension.
It is recommended the cutter to be used has to be
slightly smaller than the radius that it is going to cut.
Possible suggestion could be Ø12.


Tutorial


Refer to the question above, an
endmill is registered on the
machine with Nominal Ø12 and
Actual Ø12mm. After the
finishing cut, a measurement of
90.05mm is noted across the
contour. The part is oversized.
What could be the main reason?
What has to be done to achieve
the desirable dimension 90mm?


2 main possible reasons:
1.

2.

Tool may be deflected in the cutting
process due to the cutting forces and
machine rigidity. As the tool bends away
from the work material, it cuts less and
ends up with oversized parts.
Tool may have worn off. It is smaller than
12mm.
 The difference 90 – 90.05 = -0.05mm
 The Tool Offset, Actual diameter
should be input as 12 – 0.05 = 11.95mm
 Carry out another cutting pass to
yield the desirable dimension.

Tutorial


When the cutter diameter increases, what will happen
to the table feed (mm per minute)?
a) The table feed increases if the cutting speed and feed
per rev remians unchanged.
b) The table feed decreases if the cutting speed and
feed per rev remians unchanged.
c) The table feed remains unchanged if the cutting
speed and feed per rev remains unchanged.
d) The table feed increases if the cutting speed and feed
per rev also increase.


Unit 3

Engraving and Pocketing Operations


What is engraving?




Metal engraving is the process of cutting a series of
lines and arcs into the surface of a metal object or
plate to form a design, image or words.
CNC machines are commonly used in this process as
the controller can follow the contour of the word or
the image closely.


Engraving tools






Engraving tools are usually small in
diameter and they are made from solid
carbide for maximum tool strength.
As the tip is relatively weak, the plunge
feed rate has to be lower than an
endmill.
Applications of engraving can be easily
found in plastic injection moulds,
jewellery, plagues, medals....


What is a pocketing process?




Pocketing process is to
remove a volume of
material in a cavity.
It may involve the drilling
first and then opening up
through long-edge milling.


What tools can be used for pocketing?




Slot drill - made from HSS or
solid carbide. The longer
cutting edge extends right to
the centre which allows
centre cutting or plunge
milling.
Inserted Carbide Endmill –
both inserts are of the same
size. There is no cutting
action at the centre. It does
not support plunge milling


What are the 3 basic methods in machining a
cavity? Discuss the factors governing your
choice.
a.

a.

a.

Pre-drill a starting hole
 Applicable in most cases, disadvantage is that
additional processes are required prior to cavity
milling.
2 axis ramping
 Applicable in machining cavities which are rectangular
in nature.
Helical ramping
 Applicable in machining cavities which are circular in
nature.

Methods 1: pre-drill a starting hole










A starting hole is drilled prior to
milling.
The endmill is always fed into the
cavity at the starting hole position.
The tool does not require centre
cutting capability.
The endmill machines the cavity from
the start hole spiralling from inside
out.
Applicable in most cases.
Disadvantage is that additional
processes are required prior to cavity
milling.

Method 2: 2 axis ramping






By linear ramping with X
and Z axis, an insert
endmill is able to feed into
the cavity at a small angle,
typically 3 to 5o.
After reaching the cut
depth, it will cut in the XY
plane. Upon completion, it
will ramp to the 2nd cut
depth.
Applicable in machining
cavities which are
rectangular in nature.

Method 3: Helical ramping










The tool is fed in a helical path in
the axial direction of the spindle.
It is very useful if the cavity is
too small for 2 axis ramping.
Typical application is to machine
holes with large diameters.
It is recommended that the
diameter of the hole is about
twice the diameter of the cutter.
Applicable in machining cavities
which are circular in nature.

Name some strategies for removing material in
a cavity.


Depends on the shape of cavity, different roughing
patterns can be applied to clear stock material in a
cavity.


What is an island in a pocket? What is a gouge?






Islands are areas inside the pocket
boundary that are not intended to be
cut during pocketing.
In machining a pocket with islands,
the size of the tool may not machine
the space between two islands or
between an island and the pocket
wall. This is known as a gouge.
A gouge happens when the gap
between the islands is smaller than
the cutter diameter.

Tutorial


An island is a part of the material remaining
____________ after the machining operation.

uncut


A gouge happens when the cutter is ________ than
the gap between the island and the wall of the
contour.

bigger


What are the differences among Slot Drill, End Mill and
Inserted Endmill? State the respective applications.














Slot Drills are usually of 2 cutting flutes. They are rather short in
length and rigid to cut in the axial direction. They are good to
start machining slots or cavities without pre-drilled holes.
End Mills are usually having 4 or 6 cutting flutes, depending on
the tool diameter. They are relatively longer in length.
Some of them could perform cutting in the axial direction. One of
the cutting edges is longer than others so as to cut material up
to the centre of the tool.
Some of the End Mills have a cavity at the centre of the tool
which does not allow axial feeding.
Inserted Endmills have usually 2 to 4 Indexable Carbide inserts
mounted onto the Endmill.
The number of cutting edges depends on the tool diameter. The
Inserted endmill usually does not support axial cutting. Ramping
at an angle of 5 degree is normally used in machining cavities.
Inserted Endmill usually start from Ø10 onwards.

Question 10
After milling a cavity, you noticed that there is a slight
error in the width of the cavity. Which of the following is
a possible solution?
 changing the tool offset register
 G41 should be changed to G42
 G42 should be changed to G41
 can use only G40


Unit 4
Drilling


What are the considerations when drilling?








HSS twist drills can be TiN coated or uncoated. Common
size ranges from 0.2 to 20mm.
Important to maintain the temperature on the tool tip.
When the drill is cutting deep into the work material,
coolant may not be able to reach the cutting zone. Thus
the temperature arises which causes the drill to lose its
cutting edge. Rubbing will start rather than cutting which
leads to subsequent drill breakage.
Swarf removal is also becoming more difficult when a deep
hole is drilled.
To overcome the problem, Chip breaking or Peck drilling
technique could be employed.

Spot drilling (G81)








90o NC Centre drill is used for
spot drilling.
It is much shorter than twist
drills, thus provides the
rigidity to achieve the
positional accuracy of holes.
The tip angle could also serves
as chamfer on drilled holes.
What should be the depth of
spot drilling if a chamfer of
1mm is required on a Ø8 hole?
What is the size of NC centre
drill used?

Chip Break Drilling (G73)


Drilling starts at the top surface
until the peck depth is reached, the
drill will retracted for a short
distance (Retract amount). This
prevents formation of continuous
chip which is dangerous, difficult
to dispose and may obstruct
coolant reaching the drill tip.


Peck Drilling (G83)


Similar to Chip Break Drilling,
except that the drill is fully
retracted to the clearance height
which is above the work top
surface. It gives sufficient time
for the coolant to maintain the
drill tip temperature and the
swarf to be washed away from
the drill flutes.


Rigid Tapping (G84)






Small sizes of threaded
holes are done by machine
tapping.
The tap is fed into the work
with a feed rate (mm/rev)
which is equal to the pitch
of the thread.
Upon reaching the bottom,
the tap is reversed at the
same rate back to the start
point.

Reaming (G85)






Simple drilling will not be able to produce very
precise holes and surface finish.
In order to achieve holes of H7 dimensional
accuracy and surface finish better than Ra0.8,
reaming is to be done after drilling.
The reamer cuts with feed in and out of the hole
while drilling has rapid retract.


Reaming (G85)


To produce a hole of Ø8H7 (+0.015/+0) to a depth of
20mm, the typical steps could be:
 NC Spot drill to depth 4.5mm, this will leave 0.5mm
chamfer on the reamed hole
 Peck Drill to a depth of 25mm with a twist drill Ø7.8mm
 Ream to a depth of 21mm, (1mm is the chamfer on the
end of the reamer)


Tutorial


A 9 mm dia spot drill is used to drill a centre hole with
a depth of 3.5 mm, what is the dia of the hole when
the spot drill is finished?
 7 mm



What should be the depth of spot drilling if a chamfer
of 1.5 mm is required on a Ø8 mm hole?
 5.5 mm



Tapping an M8x1.5 threaded hole to a depth of 10 mm.
How long does it take? (Given the spindle is rotating
at 350rpm)
 Feed/min=1.5*350=525mm/min
 Time required =10/525*60=1.14seconds

Tutorial


Using a drill 10 mm in diameter to drill a through hole
in a block of metal 35mm thick, the depth of the hole
need to be programmed as _________ mm. (Given
that the included angle of the drill is 118 deg, and
answer in 2 decimal point.)



Depth=5/(tan59)=2.88
Allowance=0.5
Z=-38.38





Tutorial


You need to drill a 20 mm diameter hole in mild steel
with a high speed steel drill. You look in a cutting
conditions handbook and find the recommended
speed is 100 m/min. What speed in rpm should you
use?



N=(100*1000)/(3.1416*20)=1592rpm


Tutorial


A student working on FYP has to drill a series of Ø3
holes on an aluminium plate at a pitch of 20mm
accurately. He makes use of a CNC Milling machine to
carry out the task. However, he still could not achieve
the pitch distance consistently. Explain what could be
the problem and what will be your recommendation.



Possibly, the Ø3 mm twist drill wandered off from the
desirable position. To drill holes at specific positions,
he must do spot drilling first. The spots will lead the
3mm drill in the subsequent operation.

Tutorial







Identify the four different
types of holes in the
drawing.
Countersink hole
Counterbore hole
Threaded hole
Reamed hole


Drill depths
Drill Depths
1. Centre drill
1. Peck drill
2. Centre drill
2. Peck drill
2. Counterbore
3. Centre drill

1

2 3

3. Peck drill
3. Tapping
4. Centre drill
4. Peck drill
4. Reaming


4

Drill depths
Drill Depths
Centre drill -1

-4

Peck drill -1

-43

Centre drill -2

-4 or ?

Peck drill -2

-14

Counterbore -2

-2

Centre drill -3

-5

Peck drill -3

-18

Tapping -3

-15

Centre drill -4

-6

Peck drill -4

-45

Reaming -4

-21

1

2 3


4

Tutorial


Match the command on the left to the description on
the right.

G73

Rigid Tapping

G81

Peck Drilling

G83

Spot Drilling

G84

Reaming

G85

Chip Breaking


Mm3216 milling tutorial

Recommandé

Recommandé

Contenu connexe

Tendances

Tendances (20)

Similaire à Mm3216 milling tutorial

Similaire à Mm3216 milling tutorial (20)

Dernier

Dernier (20)

Mm3216 milling tutorial