Calculating
the correct cutting feeds and speeds
Why is this
important?
The manufacturers
of modern cutting go to a lot of trouble to make their cutting tools efficient
and reliable. The
following examples and explanations are just an overview to get you started,
we recommend you contact
your tooling supplier for detailed data and specification sheets on
your particular tool.
Overview..
The following support
sheet contains:
1.
Calculating correct spindle RPM.
2.
Calculating correct feed rate.
3. Understanding
the isle Easy move feed commands
4. Understanding
the Isycam feed entry field.
1. Calculating
the correct spindle RPM (Revolutions
per minute)
What exactly are we
doing here?
Whether we are using
a electric drill a hand router or in this case a CNC milling machine
it is important to
have the tool rotating at the correct speed to ensure correct tool ware,
accurate result, safety
and economy.
We will use a simple
formula to calculate correct RPM.
325V
= RPM
D
V = Surface speed
This is the value
that is specified by the tool manufacturer and is specified in m/min
(meters per minute).
This is the recommend amount of material that should pass by the
cutting edge per minute,
we basically use our formula to convert a linear specification to
a radial one.
D = Tool diameter
This is the tool diameter
value, this is usually stamped or marked on the tool.
RPM = Revolutions per
minute
Example:
In this example we
are using a 10.00 diameter HSS slot drill to machine aluminum, my
tooling salesman recommend
that I use cutting speed of 60m/min (60 metres a minute).
325V
D
325 x 60
= 1959 RPM
10
Set the spindle speed
to 1950 revolutions per minute.
2.
Calculating the cutting feed rate
(millimeters per minute)
What's feed rate?
Now that we have calculated
the correct spindle RPM it is also important to get the cutting
feed rates correct.
The cutting feed rate is the speed in which the table moves, we will use
a simple formula to
calculate this.
Feed rate formula.
RPM
x Number of teeth x chip per tooth = Feed rate in mm/min
RPM
We need to calculate
the spindle RPM first.
Number of teeth
We also need to know
how many teeth our cutter has.
Chip per tooth
This information is
also available from your tooling supplier, it specifies the maximum chip
load per tooth/flute.
Example:
Using a 3 fluted 6.00mm
diameter Unimill machining plastic with a recommended cutting
speed of 120m/min.
We will calculate
the correct cutting feed rate.
a. The formula requires
the RPM to be calculated so we will do that first.
325V
D
325 x 120
= 6500 RPM
6
b. Now we can calculate
the cutting feed rate.
RPM x Number of teeth
x chip per tooth = Feed rate in mm/min
6500 x 3 x .1 = 1950mm/min
The cutting feed rate
for the above example is:
1950 mm/min (millimeters
per minute)
1.950 m/min
(metres per minute)
32500 um/sec (Thousandths
of a mm per second)
3.
Understanding the isel Easymove feed commands.
How does the Isel
Easymove format specify feed rate.
There are two basic
commands:
FASTVEL
VEL
FASTVEL 50000
The FASTVEL
command is used to specify a positioning (non cutting) movement the 50000
specifies 50000 um/second
( Thousandths of a mm per second).
VEL 6660
The VEL
command is used to specify a cutting feed rate and the 6660
specifies
6660 um/second ( Thousandths
of a mm per second).
How do I convert um/sec
to mm/min?
Divide Vel by 1000
to get mm/sec then multiply by 60 to get mm/min.
(VEL / 1000) x 60
= mm/min
Example:
VEL6660
(6660 / 1000) x 60
= 399 mm/min
What if I want to calculate
what the feed rate is in um/min?
Divide the mm/min
value by 60 to get mm/sec then multiply by 1000 to get the um/sec value.
(mm_min / 60) x 1000
= um/min
Example:
300 mm/min
(300/60) x 1000 =
5000 um/sec (VEL5000)
Tip:
Why not use your
favorite spread sheet program to create a quick reference chart !
4.
Understanding the Isycam feed entry field.
If you are using Isycam
CAD/CAM software take note that when in the CAM module feed
rates are entered
in mm/min, the post processor will automatically convert the feed values
to um/sec.
Example:
A feed rate of 500 mm/min
is directly entered in the Velocity field.
Take note that the
500 mm/min feed rate programmed in Isycam has been converted to um/sec.
The result after post
processing (creating NC program)
00011
00012 FASTABS Z1000
00013 VEL 1667
;Feed rate is reduced to 20% when plunging
in Z.
00014 MOVEABS Z0
00015 MOVEABS Z-1000
00016 VEL 8333
;Feed is reset to 100% for X,Y feed movements.
00017 MOVEABS X50000
00018
|
