Advertisement
Quick Links
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.
Lathe Programming Guide
Advertisement
Related Manuals for Hurco TM6
Summary of Contents for Hurco TM6
- Page 1 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...
- Page 2 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...
- Page 3 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.
- Page 4 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...
- Page 5 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.
- Page 6 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.
- Page 7 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)
- Page 8 G71 U.1 R.1 G71 P3 Q4 U.005 W.002 F.005 S1000 N3 G1 Z.05 X.95 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)
- Page 9 The code above should display an image similar to this in the graphics screen.
- Page 10 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.
- Page 11 There are 3 cycles for threading in Mode B. Long Hand G33 X___ Z___ P___(Start angle) F___ Multiple Threading Cycle G76 PXXXXXX Q___ R___ G76 X(U)___ Z(W)___ R___ Q___ F___ Threading Cycle (box cycle) G78 X___ Z___ R____(taper) F____ For this example G76 will be used G76 P XX XX XX Q___ R___ The first two XX - number of finish passes 01-99 The second two XX –...
- Page 12 G76 P010060 Q.01 R.002 G76 X.875 Z-.25 R0 P.125 Q.015 F.076 X2.25 Z.25 (RETURN TO SAFE POSITION) M5 (STOP SPINDLE) At this point the part should resemble this in the graphics. Now that the threading has finished the machine is ready to call up another tool.
- Page 13 The next step is going to be drilling. The drill must be positioned T0303 G92 S1000 G97 M3 S700 G0 G95 Z.25 There are several drilling cycles G81 X___ Z___ F___ S___ (standard drill cycle) G82 X___ Z___ P___ F___ S___ (dwell drill cycle) G83 X___ Z___ P___ Q___ F___ S___ (peck drill cycle) G83.1 X___ Z___ P___ Q___ F___ S___ (chip breaker) X - X position...
- Page 14 There is also Rigid tapping available. This is not in the sample code, however here is the information for the canned cycle. Here is an example line of code for rigid tapping G84 X0. Z-.5 P1. Q.25 F.07692 S250 Q is Peck depth. The next process is boring.
- Page 15 M5 (STOP SPINDLE) Once those operations are completed the tool should be sent home for a tool change. G28 U0. W0. (SENDS TURRET HOME) Now the grooving tool should be called up in the program, and we can position to a safe position T0505 G92 S1000 G97 M3 S500...
- Page 16 There is no canned cycle for grooving; everything must be programmed point to point. X1.1 Z-.3 G1 X.865 F.005 G0 X1.1 Z-.25 G1 X1. F.002 Z-.275 G3 X.95 Z-.3 R.025 G1 X.865 G0 X1.1 Z-.35 G1 X1. F.002 Z-.325 G2 X.95 Z-.3 R.025 G1 X.865 G0 X2.25 M5 (STOP SPINDLE)
- Page 17 Cutoff Omit the 4 lines below (green) for two axis example; these 4 lines are only for reference for live tool examples. T0505 G92 S1000 G97 M3 S500 Z-1.75 X2.1 G1 X1.85 F.003 G0 X2.1 Z-1.65 G1 X2. Z-1.7 X1.9 Z-1.75 X-.04 X2.25 M5 (STOP SPINDLE)
- Page 18 Two axis sample program O1234(TWO AXIS SAMPLE) G20 G40 G80 G90 G28 U0. W0. (SENDS TURRET HOME) T0101 (CALL TOOL ONE OFFSET ONE) G92 S1000 (MAX RPM 1000RPM) G97 M3 S500 (TURN THE SPINDLE ON AT 500 RPM) G0 G95 Z.25 X2.25 G96 G1X2.1 F.004 G72 U.1 R.1 (U IS DEPTH OF CUT R IS RETRACT DISTANCE)
- Page 19 X2.25 G76 P010060 Q.01 R.002 G76 X.875 Z-.25 R0 P.125 Q.015 F.076 X2.25 Z.25 (RETURN TO SAFE POSITION) G28 U0. W0. (SENDS TURRET HOME) M5 (STOP SPINDLE) T0303 G92 S1000 G97 M3 S700 G0 G95 Z.25 G83 X0. Z-1.5 P1. Q.1 F.005 S700 G80 (CANCELS CANNED CYCLE) G28 U0.
- Page 20 Z-.25 G1 X1. F.002 Z-.275 G3 X.95 Z-.3 R.025 G1 X.865 G0 X1.1 Z-.35 G1 X1. F.002 Z-.325 G2 X.95 Z-.3 R.025 G1 X.865 G0 X2.25 Z-1.75 X2.1 G1 X1.85 F.003 G0 X2.1 Z-1.65 G1 X2. Z-1.7 X1.9 Z-1.75 X-.04 G0X2.25 M5 (STOP SPINDLE) G28 U0.
- Page 21 STOP! If the machine to be programmed is one of the following machines all the post information needed is above. TM10 TM12 TM18 TM18L TMX8 TMX10 This includes any machine above with the letter “i” afterwards...
- Page 22 III. Live Tool Examples Tools 6. Live Drill .201 7. End mill .25 8. End mill .25 When dealing with Live Tool machines there must be an understanding of these simple codes and how to utilize them. First off there are two machine modes, milling and turning. M130 –...
- Page 23 G101 AXIS MAP DIAGRAM Notice that the axes are the same layout as turning with the addition of the Y axis. This map will always use the milling mode (M131) Again there is no C axis in this map! The intended purpose of this map is to handle all polar interpolation internally from X and Y positions.
- Page 24 G102 AXIS MAP DIAGRAM This map will swap the X and Z axis. Notice the Y axis is wrapped around the diameter of the bar to be programmed, and that Z0 is on the diameter of the bar. This map will need to be used in conjunction with an additional code to establish a working diameter.
- Page 25 G109 AXIS MAP DIAGRAM This axis map uses standard axes for a lathe and is suitable for all turning operations. The typical mode for this map is the Turning Mode (M130) This map also can be used in conjunction with the Milling Mode (M131) for drilling holes with X, Z, and C positions.
- Page 26 Utilizing the G109 map properly for drilling First call the proper tool and change modes. T0606 G109 (TURNING MAP) M131 (MILLING MODE) G7 (RADIUS PROGRAMMING) G97 M33 S1500 (TURN SPINDLE ON AT FIXED RPM) Now that the proper tool has been called up in the proper mode an approach can be designated.
- Page 27 After the holes are drilled the turret should be positioned to index the turret G28 U0. W0. (SENDS TURRET HOME) It is important to place a G7 at the beginning of any live tool operation to program in radius mode, if this isn’t done all x number will need to be doubled.
- Page 28 The next tool will be loaded and used to mill in the G101 map. The G109 mode will be used to execute an approach. Programming in the way allows the C axis to be positioned without forcing the tool to travel through the center of the part.
- Page 29 M130 M35 (STOP LIVE TOOL) At this point your part should resemble the picture above. Now the turret should be indexed so that the radial tool can cut on the surface of the bar. G28 U0. W0. (SENDS TURRET HOME) The next and final step for programming a live tool lathe will be to program machining on the diameter of the part.
- Page 30 T0808 G102 G25 Q2. M131 G97 M33 S1500 G0 X-1.25 Z.25 The diameter established is a 2 inch diameter; this is established with the G25 Q2. line. If we multiply the diameter by 3.1415 we get 6.2831. That means 0.000 will be at 0 degrees, and 6.2831 will be 360 degrees.
- Page 31 M130 G8 (DIAMETER PROGRAMMING) M35 (STOP LIVE TOOL) At this point the part should look like this After every live tool operation, before a tool change the map and mode will need to be switch back to Turning G109 M130...
- Page 32 O1234(SAFE STARTUP LINE EXAMPLE) G20 G40 G80 G90 G28 U0. W0. (SENDS TURRET HOME) T0101 (CALL TOOL ONE OFFSET ONE) G92 S1000 (MAX RPM 1000RPM) G97 M3 S500 (TURN THE SPINDLE ON AT 500 RPM) G0 G95 Z.25 X2.25 G96 G1X2.1 F.004 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.
- Page 33 X2.25 G76 P010060 Q.01 R.002 G76 X.875 Z-.25 R0 P.125 Q.015 F.076 X2.25 Z.25 (RETURN TO SAFE POSITION) G28 U0. W0. M5 (STOP SPINDLE) T0303 G92 S1000 G97 M3 S700 G0 G95 Z.25 G83 X0. Z-1.5 P1. Q.1 F.005 S700 G80 (CANCELS CANNED CYCLE) G28 U0.
- Page 34 Z-.25 G1 X1. F.002 Z-.275 G3 X.95 Z-.3 R.025 G1 X.865 G0 X1.1 Z-.35 G1 X1. F.002 Z-.325 G2 X.95 Z-.3 R.025 G1 X.865 G0 X2.25 M5 (STOP SPINDLE) G28 U0. W0. T0606 G109 (TURNING MAP) M131 (MILLING MODE) G7 (RADIUS PROGRAMMING) G97 M33 S1500 (TURN SPINDLE ON AT FIXED RPM) G0 Z.25 C0.
- Page 35 G101 X-.5 Y1.25 Z-1.625 G1 G42 Y.95 F10. G40 Y1.25 G0 Z.25 G109 X2.5 C180. G101 X.5 Y-1.25 Z-1.625 G1 G42 Y-.95 F10. X-.5 G40 Y-1.25 G0 Z.25 G109 M130 M35 (STOP LIVE TOOL) G28 U0. W0. T0808 G102 G25 Q2. M131 G97 M33 S1500 G0 X-1.25...
- Page 36 M130 G8 (DIAMETER PROGRAMMING) M35 (STOP LIVE TOOL) G28 U0. W0. T0505 G92 S1000 G97 M3 S500 Z-1.75 X2.1 G1 X1.85 F.003 G0 X2.1 Z-1.65 G1 X2. Z-1.7 X1.9 Z-1.75 X-.04 X2.25 M5 (STOP SPINDLE) G28 U0. W0.
- Page 37 STOP! If the machine to be programmed is one of the following machines all the post information needed is above. Please refer to the 2 axis section for cutoff example. TMM8 TMM10 This includes any machine above with the letter “i”...
- Page 38 IV. Live tool Y axis No additional tools will need to be setup There are two additional axis map codes used for milling on the main spindle utilizing the Y axis. G103 - Milling on the face of the part with Y axis G104 - Milling on the diameter of the part with Y axis Everything is programmed very similar to the G101 map code.
- Page 39 Why use a Y axis? On the face of the part there isn’t any reason to use the Y axis in theory. The machine with a G101 map could very easily hit every angle, and cut every feature. However Angular accuracy is decreased as the machine gets further away from the center of rotation.
- Page 40 Milling with the Linear Y G103 Axis Map First step is to call the tool On all Y axis lathes the tool change block will be different from the two axis and live tool machine. Since we are adding another axis an offset for the axis must be able to be applied in case live tools are shifted, or gang tool holders are used.
- Page 41 Next we will return everything back to turning settings and call up the next tool. G109 M130 G28 U0. W0. From this point the final axis map code for the main spindle will be covered. G104 AXIS MAP DIAGRAM This axis map is defined similar to the G102 however the Y axis is not wrapped around the part, in this map it is linear up and down.
- Page 42 This map can use a G25 Q0. If programming around the center is desired, or programmed where Z0. is the diameter of the bar. To begin a tool must be called and positioned G103 (ALLOWS THE Y AXIS TO BE USED) T0606 (CALLS UP THE TOOL AND APPLIES OFFSET) Y0.
- Page 43 STOP! If the machine to be programmed is one of the following machines all the post information needed is above. Please refer to the 2 axis section for cutoff example. TMX8MY TMX10MY This includes any machine above with the letter “i”...
- Page 44 The following will apply to sub spindle machines. Part Transfer The first step is recognizing that the work will be transferred and positioned inside the machine so we will need to setup a new work offset. On the input screen press part setup.
- Page 45 At the point the screen will look similar to this. The G54 value will most likely not be 10 inches, this is only here as an example.
- Page 46 On this page there needs to be an offset with the sub spindle check box selected. This will allow the sub spindle to rotate instead of the mail spindle. From here an offset for the “W” axis can be set on the main spindle offset and sub spindle The offset should be set with the sub spindle on the face of the part.
- Page 47 On the last screen press additional offsets, this page with the “W” axis will become available. The check box for the “W” offset will need to be selected, and then the machine can jog to the front of the part and the position can be stored. The spindle can then be jogged to a safe position and an offset can be stored for the position of the “W”...
- Page 48 The part transfer should be programmed as follows G109 (TURNING MAP) M130 (TURNING MODE) G0 G54 (CALLS MAIN SPINDLE OFFSET) M203:0 (COMMANDS SPINDLE SYNC AT 0 DEGREES) G97 M3 S500 (TURNS THE MAIN SPINDLE ON AT A FIXED RPM) M241 (ALLOWS THE SUB SPINDLE TO OPEN WHILE ROTATING) M114 (SUB-SPINDLE OPEN)
- Page 49 The part cutoff with bar pull should be programmed as follows G103 (CALLS MAP WITH Y AXIS AVAILABLE) T0505 (CALLS TOOL AND APPLIES OFFSETS) (SHIFTS THE TOOL TO Y 0.) G109 (TURNING MAP) G92 S1000 (SETS MAX RPM AT 1000RPM) G97 M3 S500 (TURNS THE SPINDLE ON AT 500RPM) (CALLS MAIN SPINDLE OFFSET)
- Page 50 The main spindle graphics do not show the part being pulled. A Hurco MYS machine (equipped with a sub spindle) can turn between spindles. The example above should be used up until the move to position the part for the cutoff, at that point you could insert turning, milling, drilling, or any operation desired instead of cutting the part off.
- Page 51 The final examples will show how to program on the sub spindle. Tools 9. Sub Spindle Turning Tool Turning on the sub spindle is identical to the main with one difference, all moves will be positive instead of negative. G103 T0909 G109 G92 S1500...
Need help?
Do you have a question about the TM6 and is the answer not in the manual?
Questions and answers