Hurco TM6 Operating instructions

Lathe Programming Guide
I. Getting Started.
Steps to make sure your lathe is configured properly.
II. Two Axis Lathe Samples
Machines Covered
TM6, TM8, TM10, TM12, TM18
TMX8, TMX10
III. Live Tool Lathe Samples
Machines Covered
TMM8, TMM10
IV. Live Tool Y Axis Lathe Samples
Machines Covered
TMX8MY, TMX8MYS, TMX10MY, TMX10MYS
All live tool lathes that are an “i” series machine will use the same examples.
All examples are done programming in software version 09.02.68
Please read this document until a stop for your machine type is reached.
This document was designed to be used as a work book, do not jump ahead!
This document was developed by Hurco Applications in Indianapolis Indiana by Hurco USA.
THIS DOCUMENT IS STILL IN THE TESTING, THIS DOCUMENT MAY NOT BE EXACT OR COMPLETE AT THIS
TIME, PLEASE CALL HURCO APPLICATIONS FOR ADDITIONAL SUPPORT.

I. Getting Started
Make sure the software version on the machine is on this software or a
more current version than 09.02.68.
Check the first two digits to make sure it is larger than 09
Check the second set of digits to make sure it is larger than 02
Check the last set of digits to make sure it is larger than 68

The next step is to make sure the NC setting have been
properly set.
Press the AUX/Menu button on the control.
This button is located next to the Input button on the control. It will be one of the large
oval shaped buttons.
Press the utilities key on the touch screen.
Press the user preferences soft key
Press the NC Setting key
This control should display this screen.

Set all the settings as displayed above. The only setting
that may change is the ISNC G Code Mode. (see next page)
There are Two settings for G code interpertation.
The easiest way to think about these two modes is to imagine they are dialects, some of the
codes will mean different things, however all the functionallity exist in both modes, you may just need
to use a different code.
STOP!
Some codes are only available in certain modes. The mode of ISNC G-code will determine how
to program the machine.
Mode A is an older style of code and may not have all the functionality that Mode B will
contain. Mode A’s purpose is to add flexability. Mode A may allow programs from an older
control that is not a Hurco control to run on a hurco control will little to no modification.
Mode B is the Prefered way to program a Hurco Turning
Center!
ALL EXAMPLES WILL BE IN MODE B!

Most codes will retain the same functionallity.
These codes Containt the same functionality between modes, however may still require different
parameters.
G00, G01, G02, G03, G04, G06, G07, G08, G09, G10, G11, G17, G18, G19, G20, G21, G28, G40, G41, G42,
G53, G54-G59, G54.1, G61, G64, G65, G66, G67, G70, G71, G72, G73, G74, G75, G76, G80, G81, G82,
G83, G84, G85, G86, G87, G88, G89, G93, G96, G97.
This table will show the main differences
Mode A
Mode B
G50
Max RPM
G92
Max RPM
G98
Per Min Feed
G94
Per Min Feed
G99
Per Rev Feed
G95
Per Rev Feed
No Code
G98
Return to Initial Level
No Code
G99
Return to R point Level
G94
End Face Turning Cycle
G79
End Face Turning Cycle
G92
Thread Cutting Cycle
G78
Thread Cutting Cycle
No Code
X,Y,Z Coordinates Abs
G90
Absolute Programming
No Code
U,V,W Coordinates Inc
G91
Incremental
Programming
G90
Outer/Inner Cutting
Cycle
G77
Outer/Inner Cutting
Cycle
G32
Thread Cutting
G33
Thread Cutting
The table above can be used as a reference guide to change
codes to alter an existing program.

II. Two Axis Lathe Programming Guide
Tools
1. OD turning tool
2. OD threading tool
3. ½ inch drill
4. ID turning tool
5. 1/8 cutoff/grooving tool
To start a Lathe Program begin with a safe startup line.
%
O1234(SAFE STARTUP LINE EXAMPLE)
G20 G40 G80 G90
G28 U0. W0. (SENDS TURRET HOME)
From This point call up a tool and set the max rpm and turn on the spindle.
T0101 (CALL TOOL ONE OFFSET ONE)
G92 S1000 (MAX RPM 1000RPM)
G97 M3 S500 (TURN THE SPINDLE ON AT 500 RPM)
Now we are ready to call up a work offset and command motion
G54
G0 G95 Z.25
From this point on we are able to begin programming features
From this point on most likely the next operation would be facing the part. We will leave
stock to take off later with a finish cycle.
Note: you must leave stock with a roughing cycle.
Tip: the position right before a canned cycle should be a safe position or
rapid position.

X2.25
G96 G1X2.1 F.004 (CONSTANT SURFACE SPEED)
G72 U.1 R.1 (U is depth of cut R is retract distance)
G72 P1 Q2 U0.005 W0.005 F.002 S1000 T0101
N1 G1 X2.0 Z0.
X-.04
N2 Z.05
G0 X2.25 Z.25 (RETURN TO SAFE POSITION)
Since the face is now roughed we can come back in with a finish pass
G70 P1 Q2 F.002 S1000
X2.25 Z.25 (RETURN TO SAFE POSITION)
In this example the profile was used from the roughing cycle.
Next step is to cut a profile. The profile for this example will be a basic step cylinder.

G71 U.1 R.1
G71 P3 Q4 U.005 W.002 F.005 S1000
N3 G1 Z.05 X.95
Z0.
X1.Z-.025
Z-.5
X1.2
X1.25 Z-.55
Z-1.
G2 X1.75 Z-1.25 R.25
G1 X1.95
X2. Z-1.3
N4X2.05
X2.25 Z.25 (RETURN TO SAFE POSITION)
Now the profile is roughed finishing can be done with one line of code.
G70 P3 Q4 F.002 S1000
X2.25 Z.25 (RETURN TO SAFE POSITION)
M5 (STOP SPINDLE)

The code above should display an image similar to this in the graphics screen.

Note: G73 can also be used to rough a profile, or to do multiple finish passes to
step down a profile.
Tool change
Before the turret is indexed to the next tool it should be at the home position.
G28 U0. W0.
Now the turret can index and setup the speed for the next tool and move to position.
T0202
G92 S1000
G97 M3 S500
G54
G0 G95 Z.25
X2.25
From this point an OD thread will be cut.