Manual Guide i Lathe Training Workbook For Lathe Turning & Milling A-816A Hardinge Inc., 2008 Part No. A A-0009500-0816 Litho in USA June 2008
2
Section Pages Section One: Basic Machine Operations Sequence Of Operation 7-9 Enter Main Workshift Values 10 Enter Sub-Spindle Workshift Values 11 Enter Geometry Offset Values 12 Enter Safe Index Values 13 Accessing The Macro Variable Values 14 Inserting Manual Guide I (MGI) Tool Data 15-16 Part Number 123 17 Create A New Part Program 18 Create A New Part Blank 19-20 Set Tool Stations 21-22 Selecting A Spindle 23 FIXFRM (Fix Forms) Operation Start up Commands 24-25 Turning Cycle G1120 26-29 Defining A Part Profile For Turning 30-38 To End An OD Turning Cycle 39 Hole Machining With Spindle Rotating G1100 Center Drill Cycle 40-42 Hole Machining With Spindle Rotating G1101 Drill Cycle 43-45 Tapping With Spindle Turning G1102 Tapping Cycle 46-48 Turning Cycle (Finish) G1126 Finish Turning Cycle 49-51 Threading G1462 Threading Cycle 52-56 Grooving G1130 Grooving Cycle 57-62 Part Simulation 63-65 NC Conversion 66-67 3
Section Pages Section Two: Basic Main Spindle Machining For C Axis Cycles Inserting MGI Tool Data 76 Part Number 234 77 Center Drill Cycle G1110 and G1572 Cycles 78-87 Face Drill Cycle G1111 and G1572 Cycles 88-93 Face Tapping Mill Cycle G1112 and G1572 Cycles 94-99 OD Center Drill Cycle G1110 and GG1672 Cycles 100-105 OD Drill Cycle G1111 and G1672 Cycles 106-111 OD Tapping Cycle G1112 and G1672 Cycles 112-120 NC Conversion 120-125 Section Three: Basic Main Spindle Milling Operation For C Axis Inserting MGI Tool Data 127 Part Number 345 128 Face Mill A 1.000 Inch Pocket G1040 and G1521 Cycles 129-142 Part Number 345 143 Mill A Cylindrical Pocket on OD G1040 Cycle 144-157 To Simulate Part Number 345 158-160 NC Conversion Part Number 345 160-164 Section Four: Fix Forms Creation And Use Fix Forms (FIXFRM) 166 To Enter A FIXFRM Into Memory 167 To Edit a FIXFRM 168 To Delete A FIXFRM 168 Hardinge Entered Fix Forms Lathe 169-171 Mill 171 Section Five: Sub Spindle Transfer And Operation (Option) Sub Spindle Workshift Values 173 Setting The E Axis Workshift Value 174-175 Cut Off And Transfer To Sub Spindle 176-177 4
Section Pages Section Six: Machining On the Sub Spindle Sub Spindle Operation 179-181 Part Number 2333 182 Rough And Finish Turn On Sub Spindle G1120 And G1126 Cycles 183-189 A (C) Axis Machining Face Mill 190 Part Number 155 Cycle 1040 And 1521 191-196 Section Seven: Y Axis Machining Cycles (Option) Y Axis Option 198-199 Part Number 26 200 Y Axis Pocket Mill G1040 And G1320 201-208 NC Program Conversion 209 Section Eight: Quest Gang Tool Lathe Quadrants, Tool Layout, Part Number 500 211 Collet Dwell 212 Cut Depth Direction 213 Describing Part On Front of Spindle 213-216 Describing Part On Back of Spindle 216-223 Part Simulation 222 Part Programs 223-224 Section Nine: Hardinge Created Cycles G555; Cutoff Cycle For Main Spindle 226 G556: Tool Change Cycle 226 G557: Pull Stock Cycle 227 G558: Feedstock Cycle (Simple Bar Feed Systems) 227 G559: Y Axis Groove Cycle (Optional) 227-228 Section Ten: Addendum Part Number 2000 Casting Cycle G1120 230-235 Cycle Time Calculator 236 Intersecting Arc s 237-247 To Graph A Standard NC Program 248 5
Read prior to using Manual Guide i Introduction Manual Guide i was developed by GE Fanuc. It allows for interactive shop floor programming. The shop floor programmer can program different Turning & Milling Cycle with ease and still have the flexibility to interact with the part program. Hardinge has taken Manual Guide i another step by entering Customized Cycles and Customized Fix Form Sub Routines. This allows even the novice programmer the ability to quickly input data and achieve good programming results. For the experienced programmer, they may choose to use Manual Guide i or intermix the many different cycles with their M and G Coded program. When Using Manual Guide i there, are different ways to describe the different cycles and part contours. There are many graphic screens, that Manual Guide i displays. Each screen shows a different simulation for required input values. This LATHE TRAINING WORKBOOK FOR TURNING AND MILLING is setup to familiarize the shop floor programmer on the How To when using Manual Guide i. The Shop Floor Programmer should start at the beginning of the manual and work their way towards the back. Each section contains less information than the previous one. It is not a full comprehensive manual. If more information is needed please review the GE Fanuc manuals. At different intervals updates to the Mauual Guide I software will be made or needed information will need to be discussed. This will take place in the Addendum of this manual. Remember With this system you have the ability to out put both the MGI or the M and G Coded Conversion Program. When you have problems it is the very easy to e-mail these to Hardinge Inc. for help. Or you can call 1-800-843-8801. Good Luck and Enjoy your New System 6
SECTION ONE Basic Main Spindle Operation For The Following: Rough and Finish Turning Cycle Center Drill Cycle Peck Drilling Cycle Tapping Cycle Threading Cycle Grooving Cycle Section 1 is designed to show the operator the basic function of Manual Guide I. This Section should be reviewed prior to going to Section 2, 3, or 4. 7
SEQUENCE OF OPERATION 1. Mount Spindle Tooling Establish Workshift Values Main Spindle and Sub-Spindle (as required) Manually Load Macro Variable #500 (Main Spindle Workshift) Manually Load Macro Variable #501 (Sub-Spindle Workshift as required) 2. Mount Turret Tooling Establish X and Z geometry Values 3. Set X and Z Safe Index Values Manually Load Macro Variable #502 Main Spindle Safe Index Position Manually Load Macro Variable #503 Main Spindle Z Safe Index Position Manually Load Macro Variable #504 Sub-Spindle Safe Index Position ( as required) 4. Establish MGI Tool Data Manually Load ALL Tool Data Values On Tool Page 5. Create New Program (MGI Edit Mode) Input New Program Number (4 Numbers Max.) 6. Select Start and Create Blank Dimensions Input Part Diameter, and Facing Stock Input Facing Stock Sub-Spindle (as required) 7. Select Cycle And Auxiliary Select Tool Change Set Tool and Offset Number Set Safe Index Values and Workshift Macro Variables 8
8. Select Start THEN Select Spindle Input (1) Main or (2) Sub-Spindle (if optional sub-spindle is available) 9. Select FIXFRM (Fix Form) Insert Desired Fix Form (Select Correct Fix Form) Alter Inputted Values as Required 10. Select Type of Cycle (Turn or Mill) Select Cycle Insert ALL Required Values 11. Repeat / Create ALL required Cycles 12. Part Simulation Simulate ALL Operations 13. NC Convert Convert To an NC Program As Required. 9
ENTER MAIN SPINDLE WORKSHIFT VALUES Notes: Prior to determining the MAIN SPINDLE Z Axis WORKSHIFT Value, the workpiece-facing amount should be faced off to reveal the qualified surface. The MAIN SPINDLE Z Axis WORKSHIFT Value tells the lathe the work piece length measured from the Main Spindle Face to the Finish Part Face After the Z Axis WORKSHIFT Value for the MAIN SPINDLE is determined, it MUST be placed in Macro Variable Number #500 as a NEGATIVE NUMBER. The X Axis WORKSHIFT Value is always (0) Zero. 1. Enter: Z Axis MAIN Spindle Workshift Value into Macro Number #500 10
ENTER SUB-SPINDLE WORKSHIFT VALUES Notes: Prior to determining the SUB-SPINDLE Z Axis WORKSHIFT Value, the workpiece-facing amount should be faced off to reveal the qualified surface. The SUB-SPINDLE Z Axis WORKSHIFT Value tells the lathe the work piece length measured from the Main Spindle Face to the Finish Part Face After the Z Axis WORKSHIFT Value for the SUB-SPINDLE is determined, it MUST be placed in Macro Variable Number #501 as a NEGATIVE NUMBER. The X Axis WORKSHIFT Value is always (0) Zero. 1. Enter: Z Axis Sub-Spindle Workshift Value into Macro Number #501 11
ENTER GEOMETRY OFFSET VALUES Notes: Prior to creating a program with MANUAL GUIDE I, Tool Dimensions, Tool Radius Values, and Quadrants MUST be entered for all tools. 12
ENTER SAFE INDEX VALUES NOTE: Hardinge recommend and teaches the use of placing the turret at a Safe Index Position prior to Indexing the Turret. The Tool Change G Coded Macro (G556) is called by the operator and inserted into the Manual Guide I (MGI) program. This G coded Macro reads the values placed into Macro Numbers #502, #503, and #504. #502 = Main Spindle X Safe Index Position #503 = Main Spindle Z Safe Index Position #504 = Sub-Spindle Z Safe Index Position 13
ACCESSING THE MACRO VARIABLE FILES The Macro Variables are used to store data that is called upon within a part program. They are commonly used to store axis position values for such things as Workshift and Safe Index Values. The 500 series of locations (#500 to #532) are permanent until changed and cannot be cleared with E-Stop, Reset, or Power Down of the control. To Access File Locations: 1. OFFSET/SETTING Function Key FAR RIGHT Soft Key MACRO Soft Key Key In: Desired Location NO. SEARCH To Input Values 1. Turn: PROGRAM PROTECT Key to OFF Key In: Desired VALUES INPUT Key Repeat: Till ALL VALUES are Entered 14
INSERTING MANUAL GUIDE I (MGI) TOOL DATA Once all the tool geometry s are entered, it is necessary to access the MGI, Tool Data File and enter the different Tool Geometry s for each tool. 1. Turn: MODE SELECT Switch to EDIT GRAPH key CURSOR RIGHT Soft key till T-OFS Soft Key is displayed T-OFS Soft Key CHCURS (Change Cursor) Soft key till TAB is displayed at top of T-OFS screen 2. CURSOR RIGHT Key to TOOL DATA Once the Tool Data Screen is displayed, fourteen (14) different Tools can be described. If the desired tool is not displayed, PRESS CURSOR RIGHT Soft key for more selections. The following tools can be selected: a. General: Used for turning cycles b. Threading: Used for ID, OD, and Tapered Threads c. Grooving: Used for ID, OD, and Face Grooving d. Button: Used where a Button Nose tool is required e. Straight: Used for OD profiling where a negative rake is required. f. Drill Tool: Used for Drilling g. Chamfering: Used for chamfering the side of a mill cut h. Flat End Mill: Milling on the ID or OD of the part. i. Ball End Mill: Milling on the ID or OD of a part j. Tap: Tapping ID holes k. Reamer: Used for reaming holes Not on Centerline l. Boring Tool: Live Tool Straight Boring m. Versatile: (VRSTIL) Grooving tool used for turning n: Face Mill: Used for Face Milling (Mill) 3. Select: Desired Tool (a through m) INPUT Key CURSOR RIGHT to SET 4. Select: Desired TOOL NUMBER INPUT Key Cursor RIGHT to NEXT Field Key In: Desired Values INPUT Key Repeat: Till ALL FIELDS are entered 5. Repeat: For Each Tool SCREENS CONTINUE ON NEXT PAGE 15
6. CLOSE Soft Key when finished TAB 16
PART NUMBER 123 PART NUMBER 123.1875 R.0625 R 1.0 16 #3 Center Drill.25 Drill ¼ x 20 Tap 2.500 1.975 1.000 1.375.125 x 45.250 Wide x.125 Deep Groove.9375 1.000 1.750 2.000 6.000 17
CREATE A NEW PART PROGRAM 1. Turn: Program Protect Key to OFF Turn: Mode Select switch to EDIT 2. GRAPH Soft Key Cursor Right till NEWPRG (New Program) Soft Key is displayed NEWPRG Soft Key Key In: PROGRAM NAME (4 digits max.) 3. CREATE Soft Key New Program Soft Key New Program Name New Program Screen 18
CREATE A NEW PART BLANK A New Part Program Number MUST be displayed on the screen prior to creating a Part Blank. The Lathe should be in EDIT Mode, Protect Key to OFF, and the GRAPHIC PAGE displayed on the screen. 1. Cursor Right till START Key is displayed START Soft Key Cursor Right to BLANK Cursor Down to Desired Blank One of the following blanks may be selected: a. Rectangular Blank Figure b. Cylinder Blank Figure c. Hollow Blank Cylinder Figure d. Free Contour Cylinder Blank Figure e. Prism Blank Figure F. Hollow Prism Blank 2. SELECT Soft Key Key In: VALUES INPUT Soft Key Repeat: Till ALL Values are entered 3. INSERT Soft Key when finished SCREENS CONTINUE ON NEXT PAGE 19
Part Blank Selection Part Blank Screen Diameter D = 2.5 Length L = 6.0 Work Origin K =.03 (Facing Stock) Work Origin Z (SPN 2) W =.03 (Facing Stock) 20
SET TOOL STATIONS Caution: When Lathe has the Sub Spindle Option, the Spindle Selection MUST be made prior to the start of each operation. The next step will input the following: 1.) Safe Index Positions, 2.) Tool Call Command, 3.) Geometry Call Command, 4.) Workshift. Ensure that the Cursor is in the RIGHT location. 1. Lathe CYCLE Soft Key Cursor Right to AUXILIARY Cursor Down to TOOL CHANGE SELECT Soft Key CYCLE Soft Key 2. Key In: TOOL NUMBER INPUT Key Key In: TOOL OFFSET Number INPUT Key 21
SET TOOL STATIONS (CONTINUED) After the Offset Number is entered the screen will change. The next screen will display the X Safe Index Position for the lathe. There will be TWO (2), Z Safe Index positions. If the optional Sub-Spindle is available the second value will display a different value. If the sub-spindle is not available enter the same Z Safe Index position as the Main Spindle. The Values displayed above come from Macro Numbers 500, 501, 502, 503, and 504. 3. Cursor Down Key to WORK OFFSET MACRO # A = Enter: Either 500 for tools working on the MAIN or 501 for tools working on the SUB-SPINDLE INSERT Soft Key when completed 22
SELECTING A SPINDLE The spindle Selection is used to tell the lathe which spindle you are working on. You will need to enter the Number ONE (1) or the Number TWO (2) for the Sub-Spindle. If you have only the main spindle you will still need to enter ONE (1). 1. Cursor Right till START Soft Key is displayed START Soft Key Cursor Right to SEL SPIND (select spindle) SELECT Soft Key When your lathe is equipped with a Sup-Spindle and you are using the Sub Spindle you will need to select Spindle 2 before the TOOL CHANGE is selected 2. Enter: Either ONE (1) Main Spindle or TWO (2) Sub-Spindle INSERT Soft Key 23
FIXFRM (FIX FORMS) Operation Start-Up Commands As a convenience Hardinge has entered into the control different FIXFRM (FIX FORMS) Cycles for Turning and Milling. In the Turning Cycle they are used to Start and End all Operations, Setting/Movement Commands, and Transfer Commands. On the Milling Cycle Side they are used to Start and End all Milling Operations for Facing and OD work, and to End all Milling Operations. The FIXFRN s can be altered, deleted, or new ones can be created. A maximum of Five FIXFRM s can be created per Tab. Once the desired FIXFRM is selected and inserted into the program, the operator will be prompted to update required information. This information may be Spindle Direction and CSS. This information to be altered is labeled with a RED QUESTION MARK. The FIXFRM s will vary, depending upon lathe. Information to be Altered 24
FIXFRM (FIX FORMS) Operation Start-Up Commands 1. CURSOR RIGHT till Desired FIXFRM Cycle is displayed FIXFRM Soft Key Select: Desired FIXFRM INSERT Soft Key 2. Edit/Alter: ALL Required Information 3. Place: Cursor on the LAST EOB to continue programming 25
TURNING CYCLE CYCLE G1120 Prior to entering a Cycle into a Part Program refer to the Sequence Of Operations. If starting a New Program PLEASE complete steps 1 to 9. If the program has been started please refer to step 7 to 9. 1. CYCLE Soft Key (Turning Cycles) CURSOR RIGHT Key to TURNING Tab CURSOR DOWN to TURNING OUTER ROUGH SELECT Soft Key Turning Cycle Soft Key Once the SELECT Soft Key is pressed the following screen will appear. 26
TURNING CYCLE CYCLE G1120 On this screen the following values will need to be entered: a. P = Z CUT DIRECTION b. Q = DEPTH OF CUT PER SIDE c. H = RATE OF CUT DEPTH % d. C = X AXIS FINISHING AMOUNT / DIAMETER VALUE e. D = Z AXIS FINISHING AMOUNT f. F = CUT DIRECTION FEEDRATE g. E = INFEED FEEDRATE h. V = PULLOUT FEEDRATE 1. Key In / Select: Desired Value for Each Entry INPUT Key Repeat: Till ALL Values are entered NOTE: Once all entries are entered the screen will change 27
TURNING CYCLE CYCLE G1120 On the screen the following values will need to be entered. a. K = FIRST PASS DEPTH OVERRIDE b. W = CUT RISE AMOUNT c. U = ESCAPE AMOUNT (PULLOFF AMOUNT) d. L = X AXIS CLEARANCE e. M = Z AXIS CLEARANCE f. Z = APPROACH MOTION 2. Key In / Select: Desired Value for Each Entry INPUT Key Repeat: Till ALL Values are entered NOTE: Once all entries are entered the screen will change 28
TURNING CYCLE CYCLE G1120 NOTE: When NO Facing Stock is Available 1. UNAVIL Soft Key INSERT Soft Key When Facing Stock is Available 1. AVAIL Soft Key Key In: END FACE REMOVAL Amount INSERT Soft Key Use for this exercise Rough Turning Cycle inserted into program 29
DEFINING A PART PROFILE FOR TURNING PART This section will define the part figure in the X and Z Plane. Once the Rough Turning Cycle is defined the screen will change to allow you to enter the part dimensions. G1450, DX and Z Plane Part Contour Start Position Enter: Enter: DX START POINT (0) Zero Input Key Z START POINT (0) Zero INPUT Key OK Soft Key Screen Will Change at this time G1451, X, Z Plane Part Contour Select: Select: Desired Element (Line, CW Arc,, CCW Arc, Insert Radius, Insert Chamfer Element LINE then UP Soft Key Screen will change at this time G1451, X, Z Plane Part Contour Input: X Print Values (1.0 ) INPUT Soft Key OK Soft Key Screen will change at this time 30
Select: Next Element CC (Chamfer G1454) was selected G1454 Chamfering, X, Z Plane Input: Print Values C (.125 ) INPUT Key OK Soft Key Screen will change at this time. The Chamfer will appear after the next element is selected and entered. Select: Select: Next ELEMENT (Line) Left Soft Key G1451, X, Z Plane Input: Print Values Z( 1.0 ) INPUT Key OK Soft Key Screen will change at this time. Chamfer will now be displayed 31
Select: Select: Desired Soft Key (Element LINE) G1451 UP Soft Key G1451 X, Z Plane Part Contour ST.PT + I Soft Key (Start Point + Incremental Value of move) Input: Print Value (.375 ) INPUT Key OK Soft Key Screen will change at this time. Select: Desired Element Directional Soft Key (G1455 CR Corner Radius Was Selected) G1455 Corner Rounding X, Z Plane Input: Print Value (.0625 ) INPUT Soft Key Press OK Soft Key Screen will change at this time. Radius will appear after the next element is selected. Select: Select: Desired Direction Element Soft Key (Line G1451 X,Z Plane Was selected) Left Soft Key 32
G1451 X, Z Plane Input: Print Values (Z-1.75 ) INPUT Key OK Soft Key Screen will change at this time. Part radius will now be displayed. G1451 X,Z Plane Screen will change at this time Select: Select: Next Element (LINE) Soft Key UP Soft Key G1451 X, Z Plane Input: Print Values (X1.600 ) INPUT Key OK Soft Key Screen will change at this time 33
Select: Next Element (CCW ARC G1453) Soft Key Input: Input: X Print Value (X1.975 ) INPUT Key Z Print Value (Z-1.9375 ) INPUT Key RADIUS Print Value (R.1875) INPUT Key OK Soft Key Screen Will Change at this time Select: Next Element (LINE) G1451) Soft Key Select: LEFT Soft Key 34
Key In: Z Print Value (Z-2.0 ) INPUT Key OK Soft Key The screen will change at this time. Select : Next Element (LINE) Soft Key UP Soft Key Key In: X Print Value (X2.500 ) INPUT Key OK Soft Key The screen will change at this time. 35
Select : Next Element (LINE) Soft Key The screen will change at this time. RIGHT Soft Key Key In: Z0 INPUT Key Select: CURSOR Key to Display ATTRIBUTE BLANK Soft Key OK Soft Key The screen will change at this time. When BLANK is selected you are telling the control where the stock is to be removed. All the prior dimensions describe the part only. 36
Select : Next Element (LINE) Soft Key The screen will change at this time. DOWN Soft Key Key In: X0 INPUT Key Select: CURSOR DOWN Key to Display ATTRIBUTE BLANK Soft Key OK Soft Key The screen will change at this time. When BLANK is selected you are telling the control where the stock is to be removed. All the prior dimensions describe the part only. 37
PART BLANK IS COMPLETELY CLOSED IN Select: CREATE Soft Key Screen will change at this time CURSOR DOWN and Select CREATE AS SUB-PROGRAM Key In: PROGRAM NAME (6001) INPUT Key Key In: FIGURE NAME (TEST) INPUT Key OK Soft Key NOTE: The Part Profile is now entered into the Main Program as a Sub-Program. This Sub-program can be used to define the Finish Part Profile. M CODE Soft Key 38
TO END AN OD TURNING CYCLE CURSOR DOWN to M01 INST +; Soft Key (Insert + EOB) Rough turning operation is now completed. 39
HOLE MACHINING WITH SPINDLE ROTATING NOTE: This section will only show you how to enter the cycle into the program. Prior to entering these cycles the Tool Selections, Spindle Selections, and the FIXFRM (Fix Form) must be entered into the part program. Once the FIXFRM is selected it must be updated. G1100 CENTER DRILL CYCLE 1. CYCLE Soft Key (Turning Cycles) Move: CURSOR to HOLE MACH CURSOR DOWN to CENTER DRILL SELECT Soft Key Insert: CLEARANCE AMOUNT C (.3) INPUT Key Insert: FEEDRATE F (.007) INPUT Key Insert: DWELL TIME P (As Required) INPUT Key APPROACH MOTION Soft Key Z = Z -> X MOV INPUT Key Screen will change at this time. 40
Insert: BASE POSITION B = 0 (This is the Part Face Zero (0) Position INPUT Key Insert: CUT DEPTH L (Minus Value (-.25) INPUT Key NOTE: When doing any type of Hole Machining the Tool Geometry Offset File must have the Tool Radius Value entered into the file. Once the information is entered the INSERT Soft Key need to be pressed to insert it into the part program. INSERT Soft Key Screen will change at this time 41
NOTE: Once the information is inserted into the part program, it MUST BE ENDED with the M01 and EOB command 42
HOLE MACHINING WITH SPINDLE TURNING NOTE: This section will only show you how to enter the cycle into the program. Prior to entering these cycles the Tool Selections, Spindle Selections, and the FIXFRM (Fix Form) must be entered into the part program. Once the FIXFRM is selected it must be updated. G1101 DRILL CYCLE 1. CYCLE Soft Key (Turning Cycles) Move: CURSOR to HOLE MACH CURSOR DOWN to DRILL SELECT Soft Key When the PECKING CUT DEPTH Q is left blank the Drill will drill the full depth without pecking. Insert: PECKING CUT DEPTH Q (.3) INPUT Key SETTING Soft Key (allows the Control will to Calculate the drill point length on the DETAIL page. Insert: CLEARANCE Amount C (.3) INPUT Key Insert: FEEDRATE F (.007) INPUT Key Insert: DWELL TIME P (As required) INPUT Key APPROACH MOTION Soft Key Z = Z -> X MOV INPUT Key Screen will change at this time. 43
Key In: BASE POSITION B = 0 (This is the Part Face Zero (0) Position INPUT Key Insert: CUT DEPTH L (Minus Value (-3.0 ) INPUT Key Screen will change at this time The DETAIL Screen allows the operator to adjust feedrates on the initial infeed and ending depth of the drill operation. These are OPTIONAL. CURSOR DOWN to TOOL DIAMETER Key In: DRILL DIAMETER U (.25) INPUT Key Key In: NOSE ANGLE V (118.) CAL Soft Key ONCE the information is entered the INSERT Soft Key need to be pressed to insert it into the part program INSERT Soft Key Screen will change at this time 44
NOTE: Once the information is inserted into the part program, it MUST BE ENDED with the M01 and EOB command 45
TAPPING WITH SPINDLE TURNING NOTE: This section will only show you how to enter the cycle into the program. Prior to entering these cycles the Tool Selections, Spindle Selections, and the FIXFRM (Fix Form) must be entered into the part program. Once the FIXFRM is selected it must be updated. G1102 TAPPING CYCLE 1. CYCLE Soft Key (Turning Cycles) Move: CURSOR to HOLE MACH CURSOR DOWN to TAPPING SELECT Soft Key 46
There are two (2) Types of Tapping Cycles, FLOAT using a Floating Tap Holder and RIGID using a Rigid Tap Holder. R = RIGID Soft Key Key In: THREAD LEAD (.0556) Note : If the thread lead is unknown, Key In Threads Per Inch Divided by One and Press the Input Key. Key In: Z Axis CLEARANCE C= (.3) INPUT Key Note : Keep Z Axis start point a MINIMUM of.3 in front of part face. Key In: Desired DWELL TIME P= (0) INPUT Key Select: Key In: Desired APPROACH MOTION Z = Z->X MOV Desired SPINDLE SPEED S = 800 INPUT Key Screen will change at this time. Key In: Key In: BASE POSITION B = 0 (This is the Part Face Zero (0) Position INPUT Key CUT DEPTH L (Minus Value (-.750 ) INPUT Key Screen will change at this time 47
NOTE: Once the information is inserted into the part program, it MUST BE ENDED with the M01 and EOB command 48
TURNING CYCLE (FINISH) CYCLE G1126 NOTE: This section will only show you how to enter the cycle into the program. Prior to entering these cycles the Tool Selections, Spindle Selections, and the FIXFRM (Fix Form) must be entered into the part program. Once the FIXFRM is selected it must be updated. G1126 TURNING CYCLE FINISH 1. CYCLE Soft Key (Turning Cycles) Move: CURSOR to TURNING TAB CURSOR DOWN to TURNING OUTER FINISH SELECT Soft Key Once the SELECT Soft Key is pressed the TURNING CYCLE Screen will appear. CURSOR RIGHT Soft Key to the TURNING TAB CURSOR DOWN Soft Key to TURNING (OUTER FINISH) SELECT Soft Key Once the SELECT Soft Key is pressed the CUT CONDITION Screen will appear. 49
Here we have to enter the different cut conditions for the OUTER FINISH Cycle Select: -Z (Minus) CUTTING DIRECTION P = -Z (Towards the Main Spindle) INPUT Key Key In: Desired Feedrate F = (.002) Key In: X-AXIS CLEARANCE AMOUNT L =.03 INPUT Key Key In: Z-AXIS CLEARANCE AMOUNT M =.1 INPUT Key Z->X MOV Soft Key INSERT Soft Key Once the SELECT Soft Key is pressed the INSERT TURNING Screen will appear. CANCEL Soft Key CURSOR RIGHT to SUB-PROGRAM Tab CURSOR DOWN Key to desired SUB-PROGRAM NUMBER ALL Sub-Program Numbers O6000 to O6999 that are entered into the control for the TURNING CYCLES will be displayed in a SUB-PROGRAM file. These files may be called out and used at any time in the program. If they are NOT NAMED FROM O6000 to O6999, they will not appear on the screen. Once the SELECT Soft Key is pressed the Screen will change. 50
NOTE: Once the information is inserted into the part program, it MUST BE ENDED with the M01 and EOB command 51
THREADING CYCLE CYCLE G1462 NOTE: This section will only show you how to enter the cycle into the program. Prior to entering these cycles the Tool Selections, Spindle Selections, and the FIXFRM (Fix Form) must be entered into the part program. Once the FIXFRM is selected it must be updated. G1462 THREADING CYCLE 1. CYCLE Soft Key (Turning Cycles) Move: CURSOR to THREADING TAB CURSOR DOWN to THREADING OUTER SELECT Soft Key The Included Tool Angle that is used in the Tool Data File determines at what angle the threading tool will infeed in at. If a 60 degree tool angle is used the infeed angle is 30 degrees. If it is desired to compound infeed in at 28 degrees, place 56 degrees into the Tool Data File. 52
There are six (6) different threading methods available. The CUT DEPTH is used to calculate the number of passes the control will need to take to produce the thread. The larger the value the fewer number of threading passes the lathe will take. The smaller the value the greater the number of passes the lathe will take. Once the value is entered the control calculates all passes by the following formula. 1 st Pass Depth Next Pass Depth SING. A BOTH.A STAG. A SING. D BOTH. D STAG. D Key In: Key In: (Single Amount) Compound Infeed using one side of cutter Volume Cut. (Both Angles) Plunge infeed. Volume Cut. (Staggered Angle) Compound Infeed using both sides of cutter. Volume Cut (Single Depth) Compound Infeed Using one side of cutter. Constant Depth (Both Depth) Plunge Infeed. Constant Depth (Staggered Depth) Compound Infeed using both sides of cutter. Constant Depth SING.A Soft Key - Z Cutting Direction Soft Key Desired FINISH Clean-Up Pass AMOUNT (.0004) INPUT Key Desired NUMBER OF FINISHING Passes (1) INPUT Key There are TWO DIFFERENT CUT METHODS AVAILABLE. They are NUMBER and CUT DEPTH. NUMBER is used to infeed at a constant amount. CUT DEPTH is used to calculate a volume cut depth. CUT DEPTH Soft Key Key In: Desired DEPTH OF CUT (.0102) INPUT Soft Key INSERT Soft Key Screen Will change at this time. Once the screen has changed the APPROACH MOTION will need to be selected. The SURFACE CLEARANCE is the desired X Clearance Amount. This amount should be at least 2 Thread Depths above the Part Radius. The ENTRANCE CLEARANCE needs to be the Greater Value of either 4 times the thread Lead or.250 in front of the Start of the Thread. The EXIT CLEARANCE allows the tool tip to continue in the Z Axis to clear an undercut (Groove) 53
Once the INSERT Soft Key is pressed the following screen will appear. There are FIVE (5) Types of threading figures. 1. ZX-THREAD (GENERAL) Used for any Type of thread other than a Unified, Metric, Or a Pipe Thread. 2. ZX-THREAD (METRIC) Used to cut METRIC Threads 3. ZX-THREAD (UNIFIED) Used to cut Unified Threads 4. ZX THREAD (TYPE T) Used to cut an OD Tapered Thread 5. ZX THREAD (TYPE F) Used to cut an ID Tapered Thread CURSOR DOWN to ZX THREAD (UNIFIED) SELECT Soft Key Screen will change at this time. 54
MALE SCREW Soft Key Key In: Thread Diameter (1.000 ) INPUT Key Key In: Key In: Key In: BASE POINT (Z) Z Start Point Zero (0) INPUT Key THREAD NUMBER (16) Threads Per Inch INPUT Key THREAD LENGTH POSITIVE VALUE (.875 ) INPUT Key The threading Depth can be calculated by the control, by pushing the CALC Soft Key. When pressed the thread depth is calculated by using Parameter Numbers 27152 and 27153. It uses the following formula for both ID and OD Threads: Depth =.6495 Lead Parameter Numbers 27152 and 27153 may be altered if desired. Tapered Threads uses Parameter Numbers 27154 and 27155. These may also be altered. When calculating the Tapered Thread depth the formula is as follows: Depth =.6403 Lead The THREAD NUM OF SCREW is used for Multiple start threads. CALC Soft Key Screen will change at this time. INSERT Soft Key 55
NOTE: Once the information is inserted into the part program, it MUST BE ENDED with the M01 and EOB command 56
GROOVING CYCLE CYCLE G1130 NOTE: This section will only show you how to enter the cycle into the program. Prior to entering these cycles the Tool Selections, Spindle Selections, and the FIXFRM (Fix Form) must be entered into the part program. Once the FIXFRM is selected it must be updated. G1130 GROOVING CYCLE 1. CYCLE Soft Key (Turning Cycles) OUTER ROUGH Move: CURSOR to T-GROOVING TAB CURSOR DOWN to TURN GROOVING OUTER ROUGH SELECT Soft Key There are Nine different grooving cycles. 1. TURN GROOVING (OUTER ROUGH) Used to rough out OD Grooves 2. TURN GROOVING (INNER ROUGH) Used To rough out ID Grooves 3. TURN GROOVING (FACE ROUGH) Used To rough out Face Grooves 4. TURN GROOVE (OUTER ROUGH AND FINISH) Used to rough and finish OD Grooves 5. TURN GROOVING (INNER ROUGH AND FINISH) Used to rough and finish ID Grooves 57
6. TURN GROOVING (FACE ROUGH AND FINISH) Used to rough and finish Face Grooves 7. TURN GROOVING (OUTER FINISH) Used to finish OD Grooves 8. TURN GROOVING (INNER FINISH) Used to finish ID Grooves 9. TURN GROOVING (FACE FINISH) Used to finish Face Grooves. Once the SELECT Soft Key is pressed the screen will change to the TURN GROOVE (OUTER GROOVE) Screen There are TWO (2) ROUGHING TYPES. 1. CENTER CUT Starts in the center of the groove, then moves towards the spindle, then towards the face of the part. 2. LAYER CUT Used to Peck out a groove. By selecting different Soft Key s the Z Start Position, Cut Direction, and Depth of Cut are entered CENTER Soft Key Once the CENTER Soft Key is pressed the screen will change. 58
PECKING NOTHING SCREEN Key In: SIDE FINISH AMOUNT C= 0 (Zero) Key In: BOTTOM FINISH AMOUNT D= 0 (Zero) Key In: FEEDRATE F= (.005) NOTHING Soft Key Once the Nothing Soft Key is pressed the screen will change. PECKING SCREEN If the PECKING Soft Key is Selected, the PECKING DEPTH, RATE OF CUT and RETURN AMOUNT must be inserted. Key In: Desired X Axis CLEARANCE L= (.2) INPUT Key Key In: Select: Bottom Groove Dwell Amount DWELL P = 0 (Zero) INPUT Key Desired APPROACH MOTION Z = (Z->X) Key In: Desired ESCAPE AMOUNT V= (.001) INPUT KEY The ESCAPE AMOUNT moves the tool away from the groove side on the tool retract INSERT Soft Key Once the INSERT Soft Key is pressed the screen will change 59
The type of GROOVE FIGURE must now be selected. There are Seven(7) types available. 1. ZX-GROOVE (OUTER NORMAL) Allows for programming a normal OD Groove 2. ZX-GROOVE (OUTER TRAPEZOILD) Allows for programming an OD Groove with Tapered Sides 3. ZX-GROOVE (INNER NORMAL) Allows for programming a normal ID Groove 4. ZX-GROOVE (INNER TRAPEZOILD) Allows for programming an ID Groove with Tapered Sides 5. ZX-GROOVE (FACE NORMAL) Allows for programming a normal FACE Groove 6. ZX-GROOVE (FACE TRAPEZOILD) Allows for programming a FACE Groove with Tapered Sides 7. ZX-TURNING GROOVE FIGURE Allows for turning with the grooving tool. Tool MUST be defined as VERSITAL CURSOR DOWN to ZX-GROOVE (OUTER NORMAL) SELECT Soft Key Once the SELECT Soft Key is pressed the screen will change. 60
Select: Desired BASE POINT SETTING U= The BASE POINT SETTING is determined by the Tool Touch Off Point. BASE POINT SETTING Z SID Key In: BASE POINT X= (1.000 ) INPUT Key Key In: BASE POINT Z= (-.9375 ) INPUT Key Key In: DEPTH L= (.125 ) Radial Value INPUT Key Key In: WIDTH D= (.250 ) INPUT Key Once the INPUT Key is pressed the screen will change. The CORNER INF Tab Page allows for the inputting of NO Chamfer of arc (NOTHING), a CHAMFER, or a ARC at each corner of a groove. Each corner is labeled A, E, I, and Q. Select: Desired CORNER TYPE 1 A = CHAMFR (CHAMFER) Key In: CORNER SIZE B= (.03 ) INPUT Key Select: Desired CORNER TYPE 2 E = NOTHING Soft Key INPUT Key Select: Desired CORNER TYPE 3 I = NOTHING Soft Key INPUT Key Select: Desired CORNER TYPE 4 Q = NOTHING Soft Key INPUT Key After INPUT Key is pressed screen will change. 61
The REPEAT tab allows for inserting more than one (1) groove into a program. These grooves will be identical. The Number of grooves desired, the Pitch (Distance between grooves), and the Pitch Width Direction must be defined. Key In: Desired GROOVE NUMBER M= (1) INPUT Key Press : INSERT Soft Key Once the INSERT Soft Key is pressed the screen will change. NOTE: Once the information is inserted into the part program, it MUST BE ENDED with the M01 and EOB command. NOTE: Once the M01 is inserted into the part program, End the Program with an M30 and the EOB Command. PART SIMULATION now needs to be performed. This allows for the correction of the part program prior to actually cutting the part 62
PART SIMULATION NOTE: This section will show you how to Simulate a part program that has been entered into the control through Manual Guide I. Prior to running the simulation, the part program and the Tool Data must be entered into the control. When Running the Simulation the Lathe Door MUST be closed. 1. Select: AUTO Mode SIMULAT (SIMULATE) Soft Key REWIND Soft Key START Soft Key PART SIMULATION ROUGH TURNING CYCLE CENTER DRILLING CYCLE 63
DRILLING CYCLE TAPPING CYCLE FINISH TURN CYCLE 64
THREADING CYCLE GROOVING CYCLE COMPLETED PART SIMULATION When SIMULATION is complete GRPOFF (Graphic Off) 65
NC CONVERSION NOTE: This section will show you how to convert a created part program that has been created through MANUAL GUIDE I to an NC Program. Prior to running the NC CONVERT, the part program and the Tool Data must be entered into the control. When Running the NC CONVERSION the Lathe Door MUST be closed. GRPOFF Soft Key (Graphic Mode OFF) FAR RIGHT Soft Key GPROFF Soft Key Far Right Soft Key NC CNV (NC Convert) 66
Key In: Desired PROGRAM NUMBER (124) CREATE Soft Key START Soft Key Once the START Soft Key is pressed the MGI Program will be converted into an NC Part Program. Start Soft Key 67
% O0123 G1900D2.5L6.K0.03W0.03 G556T1.W1.X19.V8.E-8.A500. G1998S1. G0G99M64 G28E#5045 G97M14(3,4,13,14)S500P1 G50S2800 G96S650 G1120P1.Q0.1H100.C0.01D0.01F0.01E0.005V0.005K100.W1.U0.05L0.03M0.1Z10.N1. M98P6001(TEST) M01 G556T2.W2.X19.V8.E-8.A500. G1998S1. G0G99M64 G28E#5045 G97M13(3,4,13,14)S2500P1 G1100C0.3F0.007Z10.B0.L-0.2Y1. M01 G556T3.W3.X19.V8.E-8.A500. G1998S1. G0G99M64 G28E#5045 G97M13(3,4,13,14)S2500P1 G1101Q0.3H2.C0.3F0.007Z10.B0.L-3.Y1.U0.25V118.K0.0751 M01 G556T4.W4.X19.V8.E-8.A500. G1998S1. G0G99M64 G28E#5045 G97M13(3,4,13,14)S800P1 G1102D0.0625C0.3Z10.R2.S800.B0.L-0.5Y1. M01 G556T5.W5.X19.V8.E-8.A500. G1998S1. G0G99M64 G28E#5045 G97M14(3,4,13,14)S500P1 G50S3500 G96S800 G1126P1.F0.005L0.03M0.1Z10. M98P6001(TEST) M01 68
G556T6.W6.X19.V8.E-8.A500. G1998S1. G0G99M64 G28E#5045 G97M13(3,4,13,14)S1200P1 G1140W1.B1.C0.0004K1.S1.P5.Z10.D0.2L0.3M0. G1462W1.D1.Z0.L20.M-0.875H0.0325 M01 M30 % % O6001(TEST SUB-PROGRAM) G1450H0.V0.A0. G1451H0.V0.375K3.D0.5L0.M0.T1. G1454H-0.125V0.5C0.125T1. G1451H-1.V0.5K5.C-1.L0.M0.T1. G1451H-1.V0.625K3.D0.6875L0.M0.T1. G1455H-1.0625V0.6875R0.0625I-1.0625J0.625K3.T1. G1451H-1.75V0.6875K5.C-1.75L0.M0.T1. G1451H-1.75V0.8K3.D0.8L0.M0.T1. G1453H-1.9375V0.9875R0.1875I-1.9375J0.8C-1.9375D0.9875E0.1875L0.M0.T1. G1451H-2.V0.9875K5.C-2.L0.M0.T1. G1451H-2.V1.25K3.D1.25L0.M0.T1. G1451H0.V1.25K1.C0.L0.M0.T2. G1451H0.V0.K7.D0.L0.M0.T2. G1456 M99 % 69
70 % O0124(NC CONVERTED PROGRAM) G1900D2.5L6.K0.03W0.03 G556T1.W1.X19.V8.E-8.A500. G1998S1. G0G99M64 G28E#5045 G97M14(3,4,13,14)S500P1 G50S2800 G96S650 (NC PROGRAM CONVERSION-START) G40 G18 G0Z0.115 X2.33 G1Z-1.975F0.01 X2.43Z-1.925 G0Z0.115 X2.13 G1Z-1.975 X2.23Z-1.925 G0Z0.115 X1.93 G1Z-1.8036 G3X2.025Z-1.9375I-0.165K-0.1339F0.005 G1Z-1.975F0.01 X2.125Z-1.925 G0Z0.115 X1.73 G1Z-1.7352 X1.83Z-1.6852 G0Z0.115 X1.53 G1Z-1.725 X1.6F0.005 X1.7Z-1.675F0.01 G0Z0.115 X1.33 G1Z-0.9847 G3X1.425Z-1.0625I-0.04K-0.0778F0.005 G1Z-1.725F0.01 X1.525Z-1.675 G0Z0.115 X1.13 G1Z-0.975 X1.25F0.005 X1.35Z-0.925F0.01 G0Z0.115 X0.93 G1Z-0.0546 X1.05Z-0.1146F0.005 Z-0.975F0.01 X1.15Z-0.925
G0Z0.115 X0.73 G1Z0.0454 X0.83Z0.0954 G0Z0.115 X0.7157 G1X0.6791Z0.0708F0.005 X0.7791Z0.1208F0.01 G0X2.59 X12. Z6.05 G18 F0. (NC PROGRAM CONVERSION-END) M01 G556T2.W2.X19.V8.E-8.A500. G1998S1. G0G99M64 G28E#5045 G97M13(3,4,13,14)S2500P1 (NC PROGRAM CONVERSION-START) G40 G0Z0.3 X0. G83Z-0.2R0.P0F0.007 G80 G0X12. Z3.5 G18 F0. (NC PROGRAM CONVERSION-END) M01 G556T3.W3.X19.V8.E-8.A500. G1998S1. G0G99M64 G28E#5045 G97M13(3,4,13,14)S2500P1 (NC PROGRAM CONVERSION-START) G40 G0Z0.3 X0. G83Z-3.0751R0.Q3000P0F0.007 G80 G0X12. Z2. G18 F0. (NC PROGRAM CONVERSION-END) M01 71
G556T4.W4.X19.V8.E-8.A500. G1998S1. G0G99M64 G28E#5045 G97M13(3,4,13,14)S800P1 (NC PROGRAM CONVERSION-START) G40 G0Z0.3 X0. M29S800 G84Z-0.5R0.P0F0.0625 G80 G0X12. Z3. G18 F0. (NC PROGRAM CONVERSION-END) M01 G556T5.W5.X19.V8.E-8.A500. G1998S1. G0G99M64 G28E#5045 G97M14(3,4,13,14)S500P1 G50S3500 G96S800 (NC PROGRAM CONVERSION-START) G40 G18 G0Z0.1 X0.55 G1X1.Z-0.125F0.005 Z-1. X1.25 G3X1.375Z-1.0625I0.K-0.0625 G1Z-1.75 X1.6 G3X1.975Z-1.9375I0.K-0.1875 G1Z-2. X2.56 G0X12. Z6.05 G18 F0. (NC PROGRAM CONVERSION-END) M01 72
73 G556T6.W6.X19.V8.E-8.A500. G1998S1. G0G99M64 G28E#5045 G97M13(3,4,13,14)S1200P1 (NC PROGRAM CONVERSION-START) G40 G18 G0Z0.3232 X1.4 Z0.3173 G92X0.9796Z-0.875R0.Q0F0.0625 G0X1.4Z0.3149 G92X0.9712Z-0.875R0.Q0F0.0625 G0X1.4Z0.313 G92X0.9647Z-0.875R0.Q0F0.0625 G0X1.4Z0.3114 G92X0.9592Z-0.875R0.Q0F0.0625 G0X1.4Z0.31 G92X0.9544Z-0.875R0.Q0F0.0625 G0X1.4Z0.3088 G92X0.95Z-0.875R0.Q0F0.0625 G0X1.4Z0.3076 G92X0.946Z-0.875R0.Q0F0.0625 G0X1.4Z0.3066 G92X0.9423Z-0.875R0.Q0F0.0625 G0X1.4Z0.3055 G92X0.9388Z-0.875R0.Q0F0.0625 G0X1.4Z0.3046 G92X0.9355Z-0.875R0.Q0F0.0625 G0X1.4Z0.3037 G92X0.9323Z-0.875R0.Q0F0.0625 G0X1.4Z0.3028 G92X0.9293Z-0.875R0.Q0F0.0625 G0X1.4Z0.302 G92X0.9264Z-0.875R0.Q0F0.0625 G0X1.4Z0.3012 G92X0.9237Z-0.875R0.Q0F0.0625 G0X1.4Z0.3004 G92X0.921Z-0.875R0.Q0F0.0625 G0X1.4Z0.3 G92X0.9196Z-0.875R0.Q0F0.0625 G0X1.4Z0.3 G92X0.9188Z-0.875R0.Q0F0.0625 G0X1.4Z0.3232 X12. Z6.05 G18 F0. (NC PROGRAM CONVERSION-END) M01
G556T7.W7.X19.V8.E-8.A500. G1998S1. G0G99M64 G28E#5045 G97M1(3,4,13,14)S500P1 G50S2500 G96S550 (NC PROGRAM CONVERSION-START) G40 G18 G0Z-0.87 X1.41 G1X0.76F0.005 G4P0 G0X1.41Z-0.87 Z-0.9325 G1X0.76F0.005 G4P0 G0X1.41Z-0.9325 Z-0.7715 G1X1.0161F0.005 X0.9441Z-0.8075 X0.76 G4P0 G0X1.41Z-0.8075 Z-0.673 G1X1.213F0.005 X1.0161Z-0.7715 G4P0 G0X1.41Z-0.7715 Z-0.5746 G1X1.213Z-0.673F0.005 G4P0 G0X1.41Z-0.673 X12. Z12. G18 F0. (NC PROGRAM CONVERSION-END) M01 M30 % 74
SECTION TWO Basic Main Spindle Operation For The Following C-Axis Cycles Center Drill OD and Face Cycles Peck Drilling OD and Face Cycles Tapping OD and Face Cycles Section 1 should be reviewed prior to using this section for a more in depth steps on MGi 75
INSERTING MANUAL GUIDE I (MGI) TOOL DATA All Workshift Values, Geometry Values, Safe Index Positions MUST be set at this time. It is now necessary to access the MGI, Tool Data Files and enter the required Tool Data. 1. Turn: Mode Select Switch to EDIT Graph Soft Key CURSOR RIGHT till T-OFS Soft Key is displayed CHCURS (Change Cursor) Soft Key till TAB is displayed Once the Tool Data Screen is displayed, the following tools need to be selected and all data entered. a. Center Drill Face Used for all types of Center Drilling on the Part Face Drill Tool Face: Used for all types of Drilling on the Part Face Tap Tool Face: Used for all types of Tapping on the Part Face b. Center Drill OD: Used for all types of Center Drilling on the Part OD Drilling OD: Used for all types of Drilling on the Part OD Tapping OD: Used for all types of Tapping on the Part OD Center Drill Face Drill Face Tap Face Center Drill Cross Working Drill Cross Working Tap Cross Working 76
PART NUMBER 234 3 Holes 120 Apart Center Drill #4 Drill #7 (.201) Tap ¼ - 20 1 Hole - On a 1.5000 BC Center Drill #4 (.3 Deep) Drill #7 (.201) (1.000 Deep) Tap ¼ - 20 (.5 Deep) C0 1.000 45 3 Holes 120 Apart 3.000 3.000 77
Section 1 should be reviewed prior to using the following instructions. Select: Key In: NEW PROGRAM Soft Key PROGRAM NAME INSERT Key Select: BLANK TYPE 78
Key In: Key In: Key In: BLANK DIAMETER INPUT Key BLANK LENGTH INPUT Key FACING STOCK (As Required) INPUT Key INSERT Soft Key to Insert into Part Program Select: CYCLE Soft Key Select: AUXILIARY Soft Key SELECT Soft Key 79
Key In: Key In: TOOL NUMBER INPUT Key OFFSET NUMBER INPUT Key The TOOL and the OFFSET NUMBER DO NOT need to be the same. Be sure to load the Correct Geometry Values in the correct file. Insure: SAFE INDEX and WORKSHIFT Values are Correct INSERT Soft Key Select: START Soft Key 80
CURSOR RIGHT to SEL. SPIND. SELECT Soft Key Enter: SPINDLE NUMBER (1 = Main Spindle) (2 = Sub-Spindle) INSERT Soft Key to insert into Part Program NOTE: At this time make sure the MILL CYCLE Soft Key is displayed FIXFRM Soft Key MILL CYCLE Soft Key 81
CURSOR RIGHT to AUX (Auxiliary) INSERT Soft Key Alter: ALL REQUIRED VALUES Place: CURSOR on ; (EOB) MILL CYCLE Soft Key MILL CYCLE Soft Key 82
CENTER DRILL CYCLE G1110 AND G1572 Ensure: CURSOR is on CENTER DRILLING SELECT Soft Key Reference Point Mode is used to tell the control the position to start the tool on the OD. INIT 1 : INIT 2 : REF. Key In: R Position. Allows the tool to Start and End Above the CLEARANCE (C) amount Entered. Tool Rapids to J + C. Value then Rapids to C Value. When all holes are completed the tool then Rapids to J + C Value. R Position. The Tool Rapids to J Value in front of part face. Then rapids to J - C. Value. Once hole is produced, tool then rapids back out to the J Start Point. Process is repeated till all holes are drilled. Tool Rapids to Tool Clearance Value (C). Once hole is produced, tool then rapids back out to the C Start Point. Process is repeated till all holes are drilled. REF. Soft Key DESIRED VALUES Press INPUT Key after each Value is entered. Press; INSERT Soft Key 83
G1110 CENTER DRILLING Cycle is now entered into the part Program and the MILLING SCREEN will appear. CURSOR DOWN Key to C AXIS HOLE ON FACE (ARC POINTS) SELECT Soft Key Key In: Key In: Key In: BASE POSITION B = 0 (Zero) (Face of Part) X POSITION of Holes (Radial Value) START ANGLE of hole INPUT Key 84
When producing only one hole the PITCH ANGLE needs to be left blank. Press CANCEL Key then the INPUT Key. Key In: Key In: PITCH ANGLE INPUT Key NUMBER OF HOLES INPUT Key +FACE Soft Key + FACE = Front / Main Spindle If lathe is equipped with the optional Sub-Spindle you will need to tell the lathe which spindle you are working on. C = Main Spindle, A = Sub-Spindle. INSERT Key 85
CENTER DRILL Cycle is now entered into the Part Program. Move: FIXFRM Soft Key CURSOR to the END TAB INSERT Soft Key Move: CURSOR to MAIN LIVE OFF INSERT Soft Key Ending format for Live Tooling is now entered into program M CODE Soft Key 86
CURSOR DOWN to M01 : OPTIONAL STOP INS+ Soft Key Center drilling operation is now complete 87
FACE DRILL MILL CYCLE This Section will only show you how to enter the cycle into the part program. Prior to entering these cycles, the Tool Selections, Spindle Selections, and the FIXFRM (Fix Form) must be entered into the part program. Once the FIXFRM is selected it must be updated. Ensure that you select the Mill Cycle FIXFRM. Select: MILL CYCLE Soft Key MILL CYCLE Soft Key CURSOR DOWN to DRILLING SELECT Soft Key 88
Key In: Key In: Key In: BASE POSITION Value INPUT Key X Axis POS (RAD.) Value INPUT Key START ANGLE INPUT Key 89
The G1111 Cycle (Drilling Tool Turning/Milling) Parameters are now entered into the part program. CYCLE Soft Key (Mill Cycle) CURSOR DOWN to C AXIS HOLE ON FACE (ARC POINTS) SELECT Soft Key Key In: Key In: Key In: BASE POSITION Value INPUT Key X Axis POS (RAD.) Value INPUT Key START ANGLE INPUT Key 90
Key In: Key In: Desired PITCH ANGLE INPUT key NUMBER OF HOLE INPUT Key Z = + FACE Soft Key ROTATION ANGLE NAME Soft Key INSERT Soft Key 91
CYCLE G1572 (FACE HOLES ON CIRCLE CX PLANE MILL/TURN) is now entered. FIXFRM Soft Key CURSOR RIGHT Soft Key to END INSERT Soft Key M CODE Soft Key 92
CURSOR DOWN Soft Key to M01 INSERT + ; Soft Key Drilling operation is now complete 93
FACE TAPPING MILL CYCLE This Section will only show you how to enter the cycle into the part program. Prior to entering these cycles, the Tool Selections, Spindle Selections, and the FIXFRM (Fix Form) must be entered into the part program. Once the FIXFRM is selected it must be updated. Ensure that you select the Mill Cycle FIXFRM. Select: MILL CYCLE Soft Key MILL CYCLE Soft Key Select: Select: HOLE MACH. Soft Key TAPPING Soft Key 94
Select: TAP TYPE RIGID Tapping does not require a floating tap holder. FLOAT Tapping requires a floating tap holder RIGID Key In: THREAD LEAD (1/Threads Per Inch) INPUT Soft Key REF. Soft Key Key In: Key In: Key In: CUT DEPTH INPUT Soft Key CLEARANCE INPUT Soft Key APPROACH MOTION Z X MOV SPINDLE SPEED INSERT Soft Key 95
Tapping cycle has been entered and screen will now change. Move: CURSOR to C AXIS HOLE ON FACE (ARC POINTS) SELECT Soft Key Key In: Key In: Key In: BASE POSITION INPUT Key X AXIS POS. (RADIUS VALUE) INPUT Key START ANGLE INPUT Key 96
The PITCH ANGLE is used when there is multiple holes on an ARC CIRCLE. INPUT Key or CURSOR DOWN Key when doing one hole. Key In: NUMBER OF HOLES INPUT Key The + FACE is used when working on the MAIN SPINDLE INPUT Key The ROTATION AXIS NAME for the MAIN SPINDLE is C. INSERT Soft Key 97
Tapping Cycle is now entered into the part program. FIXFRM Soft Key Move: CURSOR to END Tab INSERT Soft Key M CODE Soft Key 98
CURSOR to M01 : OPTIONAL STOP INS+; Soft Key INSERT Soft Key Tapping cycle is now complete and entered into the part program. 99
OD CENTER DRILLING MILL CYCLE This Section will only show you how to enter the cycle into the part program. Prior to entering these cycles, the Tool Selections, Spindle Selections, and the FIXFRM (Fix Form) must be entered into the part program. Once the FIXFRM is selected it must be updated. Ensure that you select the Mill Cycle FIXFRM. Select: MILL CYCLE Soft Key MILL CYCLE Soft Key Select: Select: HOLE MACH. Soft Key CENTER DRILLING Soft Key Screen will now change 100
Select: REF. Soft Key The REF. Soft Key selection forces the tool to start and end at the clearance point Key In: CUT DEPTH INPUT Soft Key Key In: Key In: CLEARANCE INPUT Soft Key FEEDRATE INPUT Soft Key APPROACH MOTION Z X MOV INSERT Soft Key 101
MILL CENTER DRILL Cycle has been entered and screen will now change. Move: CURSOR to C AXIS HOLE ON CYLINDER (ARC POINTS) SELECT Soft Key Key In: Key In: Key In: BASE POSITION (X RADIUS VALUE) INPUT Key Z AXIS POS. INPUT Key START ANGLE INPUT Key 102
The PITCH ANGLE is used when there is multiple holes on an ARC CIRCLE Key In: Key In: PITCH ANGLE INPUT Key NUMBER OF HOLES INPUT Key The ROTATION AXIS NAME for the MAIN SPINDLE is C. C Soft Key INSERT Soft Key CENTER DRILL Cycle is now entered into the part program. FIXFRM Soft Key 103
Move: Select: CURSOR to END Tab MAIN LIVE OFF INSERT Soft Key M CODE Soft Key CURSOR to M01 : OPTIONAL STOP INS+; Soft Key INSERT Soft Key 104
CENTER DRILLING cycle is now complete and entered into the part program. 105
OD DRILLING MILL CYCLE This Section will only show you how to enter the cycle into the part program. Prior to entering these cycles, the Tool Selections, Spindle Selections, and the FIXFRM (Fix Form) must be entered into the part program. Once the FIXFRM is selected it must be updated. Ensure that you select the Mill Cycle FIXFRM. Select: MILL CYCLE Soft Key MILL CYCLE Soft Key Select: Select: HOLE MACH. Soft Key DRILLING Soft Key Screen will now change 106
Key In: PECKING CUT DEPTH INPUT Soft Key SETTING Soft Key The Setting allows the control to calculate the amount of tool tip. Key In: REF. POS Soft Key CUT DEPTH INPUT Soft Key Key In: Key In: CLEARANCE INPUT Soft Key FEEDRATE INPUT Soft Key APPROACH MOTION Z X MOV INSERT Soft Key The screen will now change Key In: Key In: TOOL DIAMETER INPUT Soft Key NOSE ANGLE INPUT Soft Key CALC. Soft Key INSERT Soft Key 107
MILL DRILL Cycle has been entered and screen will now change. Move: CURSOR to C AXIS HOLE ON CYLINDER (ARC POINTS) SELECT Soft Key Key In: Key In: Key In: BASE POSITION (X RADIUS VALUE) INPUT Key Z AXIS POS. INPUT Key START ANGLE INPUT Key 108
The PITCH ANGLE is used when there is multiple holes on an ARC CIRCLE Key In: Key In: PITCH ANGLE INPUT Key NUMBER OF HOLES INPUT Key The ROTATION AXIS NAME for the MAIN SPINDLE is C. C Soft Key INSERT Soft Key CENTER DRILL CYCLE is now entered into the part program. 109
FIXFRM Soft Key Move: Select: CURSOR to END Tab MAIN LIVE OFF INSERT Soft Key Select: MAIN LIVE OFF INSERT Soft Key M CODE Soft Key 110
CURSOR to M01 : OPTIONAL STOP INS+; Soft Key INSERT Soft Key CENTER DRILLING cycle is now complete and entered into the part program. 111
OD TAPPING MILL CYCLE This Section will only show you how to enter the cycle into the part program. Prior to entering these cycles, the Tool Selections, Spindle Selections, and the FIXFRM (Fix Form) must be entered into the part program. Once the FIXFRM is selected it must be updated. Ensure that you select the Mill Tap Cycle FIXFRM. Note that CSS has been eliminated and the RPM has been changed. Select: MILL CYCLE Soft Key MILL CYCLE Soft Key Select: Select: HOLE MACH. TAPPING 112
Select: TAP TYPE (RIGID TAP) The RIGID Soft Key selection allows the Lathe to tap a hole with a Rigid Style Holder. The FLOAT Soft Key selection requires the use a holder that allows the tap to float. The Thread lead is calculated by the following formula: Lead = 1 / Threads Per Inch. The example we are using is for 20 threads per inch. This Lead is.05 inches per thread. If this value is unknown the operator may input 1 / 20, then press the INPUT Key to get this value. REF. POS. Soft Key Key In: Key In: CUT DEPTH INPUT Soft Key CLEARANCE Amount (Radial Value) INPUT Key 113
MILL TAP Cycle has been entered and the screen will now change. Select: C AXIS HOLE ON CYLINDER (ARC POINTS) SELECT Soft Key Key In: BASE POSITION (X RADIUS VALUE) INPUT Key 114
Key In: Z AXIS POS. INPUT Key Key In: START ANGLE INPUT Key The PITCH ANGLE is used with multiple holes. Key In: Key In: PITCH ANGLE INPUT Key NUMBER OF HOLES INPUT Key 115
The TAP MILL CYCLE is now entered into the part program. FIXFRM Soft Key Select: Select: END Tab MAIN LIVE OFF INSERT Soft Key M CODE Soft Key 116
Select: M30 : PROGRAM END INSERT + : Soft Key The Mill Tap Cycle is now completed and entered into the part program. TO SIMULATE PART PROGRAM Place: Machine in AUTO / MEMORY Mode SIMLAT (SIMULATE) Soft Key 117
REWIND Soft Key START Soft Key PART SIMULATION NC CONVERSION GRPOFF (GRAPH OFF) Soft Key FAR LEFT Soft Key 118
NC CNV (NC CONVERT) Soft Key Key In: DEST. PROGRAM NO. CREATE Soft Key START Soft Key 119
When NC CONVERSION is complete, RETURN Soft Key MANUAL GUIDE PROGRAM % O0234 G1900D3.L3.K0.W0. G556T7.W15.X19.V5.E-5.A500. G1998S1. G0G98M66 G28E#5044 M23 G97M52(51,52,53,54)S3000P3 C0 G1110I3.L-0.3C0.1F5.Z10. G1572B0.X0.75A315.M1.Z1.Y1. M55 M24 M01 G556T8.W16.X19.V7.E-5.A500. G1998S1. G0G98M66 G28E#5044 M23 G97M52(51,52,53,54)S2500P3 C0 G1111Q0.25H2.I3.L-1.C0.1F5.Z10.U0.201V118.K0.0604 G1572B0.X0.75A315.M1.Z1.Y1. M55 M24 M01 G556T9.W17.X19.V7.E-5.A500. G1998S1. G0G98M66 G28E#5044 M23 G97M51(51,52,53,54)S800P3 120
C0 G1112D0.05I3.L-0.5C0.3Z10.R2.S800. G1572B0.X0.75A315.M1.Z1.Y1. M55 M24 M01 G556T10.W18.X19.V7.E-5.A500. G1998S1. G0G98M66 G28E#5044 M23 G97M52(51,52,53,54)S3000P3 C0 G1110I3.L-0.3C0.1F5.Z10. G1672B1.5Z-1.A0.C120.M3.Y1. M55 M24 M01 G556T11.W19.X19.V7.E-5.A500. G1998S1. G0G98M66 G28E#5044 M23 G97M52(51,52,53,54)S2500P3 C0 G1111Q0.25H2.I3.L-1.C0.1F5.Z10.U0.201V118.K0.0604 G1672B1.5Z-1.A0.C120.M3.Y1. M55 M24 M01 G556T12.W20.X16.V6.E-5.A500. G1998S1. G0G98M66 G28E#5044 M23 G97M52(51,52,53,54)S900P3 C0 G1112D0.05I3.L-0.5C0.3Z10.R2.S900. G1672B1.5Z-1.A0.C120.M3.Y1. M55 M24 M30 % 121
MANUAL GUIDE I PROGRAM CONVERSION % O0235 G1900D3.L3.K0.W0. G556T7.W15.X19.V5.E-5.A500. G1998S1. G0G98M66 G28E#5044 M23 G97M52(51,52,53,54)S3000P3 C0 (NC PROGRAM CONVERSION-START) G40 M47 G0Z0.1 X1.5 C315. G83Z-0.3R0.P0F5.M46 M47 G80 G0Z0.1 C0. X14. Z0. G18 F0. (NC PROGRAM CONVERSION-END) M55 M24 M01 G556T8.W16.X19.V7.E-5.A500. G1998S1. G0G98M66 G28E#5044 M23 G97M52(51,52,53,54)S2500P3 C0 (NC PROGRAM CONVERSION-START) G40 M47 G0Z0.1 X1.5 C315. G83Z-1.0604R0.Q2500P0F5.M46 M47 G80 G0Z0.1 C0. 122
X14. Z2. G18 F0. (NC PROGRAM CONVERSION-END) M55 M24 M01 G556T9.W17.X19.V7.E-5.A500. G1998S1. G0G98M66 G28E#5044 M23 G97M51(51,52,53,54)S800P3 C0 (NC PROGRAM CONVERSION-START) G40 M47 G0Z0.3 X1.5 C315. M29S800 G84Z-0.5R0.P0F40.M46 M47 G80 G0Z0.3 C0. X14. Z2. G18 F0. (NC PROGRAM CONVERSION-END) M55 M24 M01 G556T10.W18.X19.V7.E-5.A500. G1998S1. G0G98M66 G28E#5044 M23 G97M52(51,52,53,54)S3000P3 C0 (NC PROGRAM CONVERSION-START) G40 M47 G0Z-1. X3.2 C0. G87X2.4R0.P0F5.M46 M47 123
Z-1.C120.M46 M47 Z-1.C240.M46 M47 G80 G0X3.2 C0. X14. Z2. G18 F0. (NC PROGRAM CONVERSION-END) M55 M24 M01 G556T11.W19.X19.V7.E-5.A500. G0G98M66 G28E#5044 M23 G97M52(51,52,53,54)S2500P3 C0 (NC PROGRAM CONVERSION-START) G40 M47 G0Z-1. X3.2 C0. G87X0.8792R0.Q2500P0F5.M46 M47 Z-1.C120.Q2500M46 M47 Z-1.C240.Q2500M46 M47 G80 G0X3.2 C0. X14. Z2. G18 F0. (NC PROGRAM CONVERSION-END) M55 M24 M01 G556T12.W20.X16.V6.E-5.A500. G1998S1. G0G98M66 G28E#5044 M23 G97M52(51,52,53,54)S900P3 124
C0 (NC PROGRAM CONVERSION-START) G40 M47 G0Z-1. X3.6 C0. M29S900 G88X2.R0.P0F45.M46 M47 Z-1.C120.M46 M47 Z-1.C240.M46 M47 G80 G0X3.6 C0. X11. Z6. G18 F0. (NC PROGRAM CONVERSION-END) M55 M24 M30 % 125
SECTION THREE Basic Main Spindle Operation For The Following C-Axis Cycles Polar Interpolation On Part Face Cylindrical Interpolation On Part OD Section 1 should be reviewed prior to using this section for a more in depth steps on MGi 126
INSERTING MANUAL GUIDE I (MGI) TOOL DATA All Workshift Values, Geometry Values, Safe Index Positions MUST be set at this time. It is now necessary to access the MGI, Tool Data Files and enter the required Tool Data. 1. Turn: Mode Select Switch to EDIT Graph Soft Key CURSOR RIGHT till T-OFS Soft Key is displayed CHCURS (Change Cursor) Soft Key till TAB is displayed Once the Tool Data Screen is displayed, the following tools need to be selected and all data entered. a. Cross Mill: Used for all types of Milling operations on OD of Part b. Face Mill: Used for all types of Milling operations on Part Face Tool Number 16 is for Cross Milling Tool Number 17 is for Face Milling This section will only show you how to enter the cycle into the program. Prior to entering the Mill Cycles, the Part Program Name, Tool Selection, Tool Offsets, Spindle Selection and FIXFRM must be entered into the part program. Once the FIXFRM is entered it must be updated. 127
PART NUMBER 345 C0.250 Deep 1.500 Radius.500 1.0 Square C90.500.4375 Radius Hole 1.000.375.250 128
TO MILL A 1.000 INCH SQUARE POCKET Mill Cycle on screen The following information must be entered: Program Name, Stock Size Defined, Tool Change Entered, Workshift Defied, and a Spindle Selected. FIXFRM entered and UPDATED MILL CYCLE Soft Key Move: CURSOR RIGHT to POCKETING Tab CURSOR to POCKETING (ROUGH) SELECT Soft Key Bottom Thickness (T) and the Side Thickness (S) describe the amount of stock to be removed from the pocket(s). When the values are omitted the control assumes the full amount of stock is to be removed. When there is a pre-machined pocket these values are described as linear values. 129
Key In: Cut Depth of Radius (L).05 Radius Value (Step Over Amount) INPUT Key Key In: Cut Depth of Axis (J).1 (Depth of Cut) INPUT Key Key In: SIDE FINISH AMOUNT (0) Amount of Stock to be left for a finish side cut INPUT Key Key In: BOTTOM FINISH AMOUNT (0) Amount of Stock to be left for a finish side cut INPUT Key Key In: FEEDRATE - SINGLE CUT (5.0 Inches Per Minute) INPUT Key Key In: FEEDRATE BOTH CUT (5.0 Inches Per Minute) INPUT Key 130
Key In: Feed Rate - AXIS (3.0 Inches Per Minute) INPUT Key Screen Will now change Next: Select either CUT UP or CUT DOWN Soft key NOTE: When doing a pocket the CUT UP command is for CONVENTIONAL MILLING, and the CUT DOWN is for CLIMB MILLING. CUT DOWN Soft Key Key In: CLEARANCE OF RADIUS (.05) INPUT Key 131
Key In: CLEARANCE OF AXIS (.1) INPUT Key 2 AXES APPROACH MOTION Soft Key Key In: CUT ANGLE (0) INSERT Key The CUT ANGLE allows the Tool to cut into a pocket at an Angle. This allows to load on the end mill to be reduced. Screen will change at this time. 132
G112/G12.1 Polar Interpolation Main Spindle Polar coordinate interpolation (G112 / G12.1 ) is used to machine on the face of the workpiece. This program function allows simultaneous movement in the X and C axis. When using polar interpolation, view the workpiece from the tool point of view to plot the tool path. Establish a grid system as shown below. X zero and C zero is the spindle centerline. With Manual Programming both axes are programmed in inches, with X points and C points specified as radii. With Manual Guide I Programming both axis are programmed in Linear Distances measured from the X0 C0 Position. When programming with MGI all C Axis movements will be described using UP or Down and all X Axis movements will be described using Right or Left. X+ +C +X Turret C+ X0 C0 +C LEFT +X 1.0 Square UP X0, C0 X- DOWN RIGHT C- X- C- Machine Bed Programming G112 / G12.1 Activates Polar Interpolation Programming G113/G13.1 Cancels Polar Interpolation 133
We will produce the Square Pocket first using the XC FREE CONCAVE FIGURE, then the XC-CIRCULAR CONCAVE Pocket. This will be done with the same tool. CURSOR RIGHT to POCKET FIGURE CURSOR DOWN to XC-FREE CONCAVE FIGURE SELECT Soft Key INPUT Key to select (T=CONCAVE) Key In: X START POINT (0) INPUT Key Key In: ZC START POINT (0) INPUT Key Key In: BASE POSITION (0) INPUT Key Key In: HEIGHT/DEPTH (-.250) INPUT Key Screen will change at this time. +FACE Soft Key (For working the Main Spindle) Screen will change at this time. ROTARY AXIS NAME (C) Soft Key The C Soft Key tell the control that the ROTARY AXIS is the MAIN SPINDLE OK Soft Key Screen will change at this time. 134
LINE Soft Key UP Soft Key Key In: END POINT C (1.0) OK Soft Key LINE Soft Key LEFT Soft Key Key In: END POINT X (-1.0) OK Soft Key 135
DOWN Soft Key Key In: END POINT C (0) OK Soft Key 136
RIGHT Soft Key Key In: END POINT X (0) OK Soft Key CREATE Soft Key Screen will change at this time. NEXT FIGURE (NXFIG) Soft Key 137
CURSOR DOWN to CREATE AS SUB PROGRAM Key In: SUB PROGRAM NUMBER (350) INPUT Key Key In: FIGURE NAME (SQUARE) NXTFIG Soft Key (NEXT FIGURE) Screen will change at this time. Move: CURSOR XC-CIRCLE CONCAVE SELECT Soft Key CONCAVE Soft Key 138
C+ X0 C+ X+ C0 X+ Using the following grid system the circular pocket lies in the X, and the C grid area. The X, and C linear dimensions measured from X),C0 position. X- C- X- C- Key In: BASE POSITION Z (0) INPUT Key Key In: HEIGHT/DEPTH L (-.250) INPUT Key 139
Key In: X AXIS POSITION H (-.500) INPUT Key The X and C AXIS POSITION is a LINEAR DIMENSION measured from X0, C0. Key In: C AXIS POSITION V (.500) INPUT Key Key In: RADIUS (.4375) INPUT Key Screen will change at this time. 140
The FACE + Soft Key tells the control that we are working on the Main Spindle FACE+ Soft Key The C Soft Key tells the control that the ROTARY AXIS is the Main Spindle. INSERT Soft Key The SQUARE and the CIRCULAR Pockets are now entered into the program. FIXFRM Soft Key 141
CURSOR to END Tab CURSOR DOWN to MAIN LIVE OFF INSERT Soft Key CURSOR DOWN to M01 INS+ (INSERT + EOB) Soft Key Screen will change at this time. 142
PART NUMBER 345 C0.250 Deep x 2.3562 Long 1.500 Radius.500 1.0 Square.500.4375 Radius Hole 1.000.375.250 143
TO MILL A CYLINDERICAL POCKET.250 DEEP BY.500 WIDE AND 2.3562 LONG The following information must be entered: Program Name, Stock Size Defined, Tool Change Entered,, Workshift Defined, and a Spindle Selected. Enter: FIXFRM and UPDATE VALUES MILL CYCLE Soft Key Move: CURSOR to POCKETING Tab CURSOR to POCKETING (ROUGH) SELECT Soft Key BOTTOM THICKNESS (T) and the SIDE THICKNESS (S) describes the amount of stock to be remover from the sides of the pocket(s). When the values are omitted the control assumes the full amount of stock is to be removed. When there is a pre-machined pocket these values are described as linear values. 144
Key In: Cut Depth of Radius (L).05 Radius Value (Step Over Amount) INPUT Key Key In: CUT DEPTH OF AXIS (J).05 Depth Of Cut. INPUT Key Key In: SIDE FINISH AMOUNT (K) 0 Amount of stock to be left for a Finish Side Cut INPUT Key Key In: BOTTOM FINISH AMOUNT (H) 0 Amount of stock to be left for a Finish Bottom Cut INPUT Key Key In: FEEDRATE SINGLE CUT (5.0 Inches Per Minute) INPUT Key 145
Key In: FEEDRATE SINGLE CUT (5.0 Inches Per Minute) INPUT Key Key In: FEEDRATE BOTH CUT (5.0 Inches Per Minute) INPUT Key Key In: FEEDRATE AXIS (3.0 Inches Per Minute) INPUT Key Screen will now change. 146
UP CUT or DWNCUT Soft Key When cutting a pocket the UP CUT is for CONVENTIONAL MILLING and the DOWN CUT is for CLIMB MILLING. DWN CUT Soft Key Key In: CLEARANCE OF RADIUS (.05) INPUT Key Key In: CLEARANCE OF AXIS (.1) INPUT Key 2 AXES Approach Motion Soft Key 147
Key In: CUT ANGLE (0) INSERT Key The CUT ANGLE allows the Tool to cut into a Pocket at an Angle. This allows the load on the End Mill to be reduced. Screen will change at this time. We will produce a Rectangular Pocket using the ZC PLANE FREE CONCAVE FIGURE FOR CYLINDERICAL CURSOR to POCKET FIG (Pocket Figure) CURSOR to the ZC PLANE FREE CONCAVE FIGURE FOR CYLINDERICAL SELECT Soft Key Screen will change at this time. 148
CYLINDERICAL INTERPOLATION MAIN SPINDLE GRID SYSTEM Cylindrical Interpolation is used to machine on the side of the workpiece. With this program function simultaneous movement in Z and C axes is allowed. When using Cylindrical Interpolation, it is possible to plot tool paths by laying the Part circumference (C Axis) flat. Next, establish a grid system with the vertical axis being Z (Part Face Z0 is at the top) and the Horizontal Axis being C (C0 to C360 Degrees). Cylindrical Interpolation is programmed in Degree s Z0 C Axis LEFT UP Z0 C0 C0 Z Axis DOWN RIGHT Z+ C- C+ Z- The following formulas are used for Cylindrical Interpolation: 1. Determine the Circumference of the part: CIRCUMFERENCE = PART DIAMETER x 3.14159265 2. C Axis must be programmed in Degrees. Inch Dimensions must be converted to Degree s. DEGREE = INCH x 360 CIRCUMFERENCE 149
CYLINDRICAL INTERPOLATION MODE 1. The following G codes may be used while G7.1 is active: G1, G2, G3, G40, G41, G42, G65, and G98. 2. G00 positioning is not allowed while G7.1 is active. 3. When using G2 or G3, the arc radius must be specified with an R word. 4. M23 must be commanded before the C axis may be positioned. 5. The spindle should be oriented to C0 before commanding Cylindrical Interpolation. 6. When machining in the Z axis only, do not program the G7.1 command. 7. Cylindrical Interpolation is activated on the Main Spindle by commanding the G7.1 And the C Word. The C Word specifies the part radius. 8. When programming Cylindrical Interpolation the Unit for C Axis is Degrees NOT Inches. 9. When using Cylindrical Interpolation the Z tool Geometry Offset is the center of the tool, and Quadrant 9 is required. 10. Specify feedrate in Inches Per Minute (IPM) mode G98. Determine the Circumference of the part: CIRCUMFERENCE = PART DIAMETER x 3.14159265 3.0 X 3.14159265 = 9.4248 CIRCUMFERENCE = C Axis must be programmed in Degrees. Inch Dimensions must be converted to Degree s. DEGREE = INCH x 360 CIRCUMFERENCE = 2.3562 x 360 = 848.232 = 90 Degrees 9.4248 9.4248-90 Left Down.250 Deep X 2.3562 Long Slot C0 Up Right 150
CONCAV Soft Key Key In : START POINT Z (-.375) INPUT Key Key In : START POINT C (0) INPUT Key Key In : BASE POSITION (1.500 ) INPUT Key OK Soft Key The BASE POSITION is the Radius of the PART 151
Key In : HEIGHT/DEPTH (-.250) INPUT Key Screen will change at this time. Select:: ROTATION AXIS NAME C Soft Key OK Soft Key Machines with the optional Sub Spindle will be required to select the desired Rotational Axes. C = Main Spindle, and A = Sub Spindle. Screen will change at this time. LINE Soft Key UP Soft Key 152
Key In: END POINT C (-90.) INPUT Soft Key OK Soft Key All minus input values causes the spindle to turn in the forward direction (M03). When inputting a positive value the spindle will turn in the reverse direction (M04). The Minus 90 Degrees was calculated from the following formula: Degree = Inch x 360 Circumference LINE Soft Key LEFT Soft Key Key In: END POINT Z (-1.000 ) INPUT Key OK Soft Key 153
Select: LINE Soft Key DOWN Soft Key Key In: END POINT C (0) INPUT Key OK Soft Key Select: LINE Soft Key 154
RIGHT Soft Key Key In: END POINT Z (-.375) Press INPUT Key OK Soft Key Pocket is complete and will be saved in a Sub Program. CREATE Soft Key Move: CURSOR to CREATE AS SUB PROGRAM Key In: SUB PROGRAM NUMBER (354) INPUT Key Key In: FIGURE NAME (CYLINDERICAL POCKET) OK Soft Key 155
Screen will change at this time. Program will appear on the screen. FIXFRM Soft Key Move: Select: CURSOR to END TAB MAIN LIVE OFF INSERT Soft Key Screen will change at this time. Program will appear on the screen. M CODE Soft Key 156
Move: CURSOR to M30 : PROGRAM END / REWIND INS +; Soft Key Screen will change at this time. Program will appear on the screen in its completed form. 157
To Simulate Program Place: Lathe in AUTO Mode SIMLAT (SIMULATE) Soft Key Screen Will now change. FAR RIGHT Soft Key ROTATE Soft Key Screen Will now change. ISO YZ Soft Key The part may be rotated in different directions by pressing the FAR LEFT Soft Key. 158
OK Soft Key FAR LEFT Soft Key REWIND Soft Key START Soft Key OK Soft Key 159
Simulation is now complete. NC CONVERSION FAR LEFT Soft Key GRPOFF GRPOFF (GRAPH OFF) Soft Key FAR LEFT Soft Key NC CNV Soft Key Key In: DEST. PPROGRAM NO. SELECT Soft Key 160
START Soft Key START Soft Key Manual Guide I program has now been converted to an NC format. MANUAL GUIDE PROGRAM % G556T7.W16.X19.5V5.E-5.A500. O0345 Pg. #1 G1998S1. Pg. #2 G1900D3.L3.K0. G0G98M66 G556T8.W17.X19.5V5.E-5.A500. G28E#5045 G1998S1. M23 G0G98M66 G97M52(51,52,53,54)S1500P3 G28E#5045 C0 M23 G1040L0.05J0.05K0.H0.F5.V5.E3.W2.B0.05C0.1Z2.A0. G97M52(51,52,53,54)S1500P3 M98P354(CYLINDERICAL POCKET) C0 M55 G1040L0.05J0.1K0.H0.F5.V5.E5.W2.B0.05C0.1Z2.A0. M24 M98P350(SQUARE) M30 G1521T3.B0.L-0.25H-0.5V-0.5R0.4375Z1.Y1. % M55 M24 M01 161
% O0350(SQUARE) G1990(GROUP START) G1500T3.H0.V0.B0.L-0.25Y1.Z1.A0. G1501H0.V1.K3.D1.L0.M0.T1. G1501H-1.V1.K5.C-1.L0.M0.T1. G1501H-1.V0.K7.D0.L0.M0.T1. G1501H0.V0.K1.C0.L0.M0.T1. G1506 G1991(GROUP END) M99 % Pg. #3 % Pg. #4 O0354(CYLINDERICAL POCKET) G1990(GROUP START) G1600T3.H-0.375V0.I-0.375J0.B1.5L-0.25Y1.A0. G1601H-0.375V-2.356195K7.D-90.L0.M0.T1. G1601H-1.V-2.356195K5.C-1.L0.M0.T1. G1601H-1.V0.K3.D0.L0.M0.T1. G1601H-0.375V0.K1.C-0.375L0.M0.T1. G1606 G1991(GROUP END) M99 % MANUAL GUIDE I NC CONVERSION PROGRAM % O0543 G1900D3.L3.K0. G556T8.W17.X19.5V5.E-5.A500. G1998S1. G0G98M66 G28E#5045 G10L50 N5461R4 G11 G97M52(51,52,53,54)S1500P3 C0 (NC PROGRAM CONVERSION-START) G40 G12.1 G1X-0.95C0.475F78.7 Z0.1 Z-0.1F5. C0.525 X-1.05 C0.475 X-0.95 X-0.9C0.45 C0.55 X-1.1 C0.45 X-0.9 X-0.8C0.4 C0.6 X-1.2 C0.4 X-0.8 X-0.7C0.35 C0.65 X-1.3 C0.35 X-0.7 Pg. #1 X-0.7C0.35 C0.65 X-1.3 C0.35 X-0.7 X-0.6C0.3 C0.7 X-1.4 C0.3 X-0.6 X-0.5C0.25 C0.75 X-1.5 C0.25 X-0.5 X-0.5707C0.2854 Z0.1F78.7 X-0.95C0.475 Z-0.1 Z-0.25F5. C0.525 X-1.05 C0.475 X-0.95 X-0.9C0.45 C0.55 X-1.1 C0.45 X-0.9 X-0.8C0.4 C0.6 X-1.2 C0.4 X-0.8 X-0.7C0.35 C0.65 X-1.3 Pg. #2 162
163 C0.35 X-0.7 X-0.6C0.3 C0.7 X-1.4 C0.3 X-0.6 X-0.5C0.25 C0.75 X-1.5 C0.25 X-0.5 X-0.5707C0.2854 Z0.1F78.7 G13.1 G0Z4. X12.8C0. G18 F0. (NC PROGRAM CONVERSION-END) (NC PROGRAM CONVERSION-START) G40 G12.1 G1X-0.975C-0.5F78.7 Z0.1 Z-0.1F5. G3X-1.025I-0.0125J0. X-0.975I0.0125J0. G1X-0.925 G3X-1.075I-0.0375J0. X-0.925I0.0375J0. G1X-0.825 G3X-1.175I-0.0875J0. X-0.825I0.0875J0. G1X-0.725 G3X-1.275I-0.1375J0. X-0.725I0.1375J0. G1X-0.625 G3X-1.375I-0.1875J0. X-0.625I0.1875J0. G1X-0.725 Z0.1F78.7 X-0.975 Z0. Z-0.2F5. G3X-1.025I-0.0125J0. X-0.975I0.0125J0. G1X-0.925 G3X-1.075I-0.0375J0. X-0.925I0.0375J0. G1X-0.825 G3X-1.175I-0.0875J0. X-0.825I0.0875J0. G1X-0.725 G3X-1.275I-0.1375J0. X-0.725I0.1375J0. G1X-0.625 G3X-1.375I-0.1875J0. X-0.625I0.1875J0. G1X-0.725 Z0.1F78.7 X-0.975 Z-0.1 Z-0.25F5. G3X-1.025I-0.0125J0. X-0.975I0.0125J0. G1X-0.925 G3X-1.075I-0.0375J0. X-0.925I0.0375J0. G1X-0.825 G3X-1.175I-0.0875J0. X-0.825I0.0875J0. G1X-0.725 G3X-1.275I-0.1375J0. X-0.725I0.1375J0. G1X-0.625 G3X-1.375I-0.1875J0. X-0.625I0.1875J0. G1X-0.725 Z0.1F78.7 G13.1 G0Z4. X12.8C0. G18 F0. (NC PROGRAM CONVERSION-END) M55 M24 M01 G556T7.W16.X19.5V5.E-5.A500. G1998S1. G0G98M66 G28E#5045 G10L50 N5461R4 G11 G97M52(51,52,53,54)S1500P3 C0 (NC PROGRAM CONVERSION-START) G40 G1G19W0H0 G7.1C1.5 G1C-11.459Z-0.675F78.7 X3.2 X2.9F3. C-78.541F5. Z-0.7 C-11.459 Z-0.675 Z-0.625C-9.549 C-80.451 Z-0.75 C-9.549 Z-0.625 Pg. #3 Pg. #4
164 Z-0.6604C-10.9 X3.2F78.7 Z-0.675C-11.459 X3.1 X2.8F3. C-78.541F5. Z-0.7 C-11.459 Z-0.675 Z-0.625C-9.549 C-80.451 Z-0.75 C-9.549 Z-0.625 Z-0.6604C-10.9 X3.2F78.7 Z-0.675C-11.459 X3. X2.7F3. C-78.541F5. Z-0.7 C-11.459 Z-0.675 Z-0.625C-9.549 C-80.451 Z-0.75 C-9.549 Z-0.625 Z-0.6604C-10.9 X3.2F78.7 Z-0.675C-11.459 X2.9 X2.6F3. C-78.541F5. Z-0.7 C-11.459 Z-0.675 Z-0.625C-9.549 C-80.451 Z-0.75 C-9.549 Z-0.625 Z-0.6604C-10.9 X3.2F78.7 Z-0.675C-11.459 X2.8 X2.5F3. C-78.541F5. Z-0.7 C-11.459 Z-0.675 Z-0.625C-9.549 C-80.451 Z-0.75 C-9.549 Z-0.625 Z-0.6604C-10.9 X3.2F78.7 G7.1C0 G0X15.5 C0.Z5. G18 F0. (NC PROGRAM CONVERSION-END) M55 M24 M30 % Pg. #5 Pg. #6
SECTION FOUR Fix Forms Creation and Use Prior sections should be reviewed prior to using this section for a more in depth steps on MGi 165
FIXFRMS (Fix Forms) There are two Fix Forms selections on the Operators screen. One for Mill functions and one for Turning functions. The Fix Forms are loaded into the control prior to machine shipment. They provide the operator the ability to insert into the part program, small sub-programs functions. In each Fix Form there will be a total of five different Tabs. Under each of these Tabs there can be up to five different Fix Forms. The Fix Forms are to be insert into the part program where required. In the TURNING there are Spindle transfer, Spindle Transfer with Cutoff, Tail Stock Call Up, and Tool / Spindle Start Up to mention a few. The Mill Fix Forms include Main/Sub OD Live Spindle Start Up and End, Face Live Spindle Start Up and End. The number of FIX Forms will vary depending upon options. New Fix Forms may be added or the ones in the control may be altered. TURNING FIX FRM (FIX FORM) MILL FIX FRM (FIX FORM) TURN 1 MILL 1 MILL 2 166
The Number and Content of the FIXFRM s in your lathe may vary. This section may not contain all FIXFRM S in your lathe. In the TURNING FIXFRM area there are two TAB not used. These are the END TAB and the TURN 1 TAB. In the MILL FIXFRM area there also two TABS not used. They are MILL 1 and MILL 2 TABS. TO ENTER A FIXFRM (FIX FORM) INTO MEMORY 1. Select: EDIT Mode Turn: MEMORY PROTECT to OFF FAR RIGHT Soft Key till SETTING Soft Key appears on screen SETTING Soft Key 2. Move: CURSOR to desired FIX FORM setting (A or B) A: REGISTERED FIX FORM SENTENCE FOR MILLING B: REGISTERED FIX FORM SENTENCE FOR TURNING SELECT Soft Key CURSOR RIGHT or LEFT to desired TAB 3. NEW Soft Key Key In: Desired REGISTERED NAME (32 Alpha/Numerical Characters Max.) INPUT Key 4. Key In: DESIRED Code After each block of information is entered, end it with the EOB statement. DO NOT press INSERT UNTIL all of the FIX FORM is entered. EXAMPLE ONLY: G1G98G40;G97S1000M03;W-1.F50.;G4U2.;W1.;G4U2.; INSERT Soft Key (FIX FORM is now entered into memory) When Complete: 5. TO MENU CANCEL 167
TO EDIT A FIXFRM (FIX FORM) IN MEMORY 1. Select: EDIT Mode Turn: MEMORY PROTECT to OFF FAR RIGHT Soft Key till SETTING Soft Key appears on screen SETTING Soft Key 2. Move: CURSOR to desired FIX FORM setting A: REGISTARED FIX FORM SENTENCE FOR MILLING B: REGISTARED FIX FORM SENTENCE FOR TURNING SELECT Soft Key CURSOR RIGHT or LEFT to desired TAB Move: CURSOR to select FIX FRM to be ALTERED 3. ALTER Soft Key Key In: Desired FIX FORM change INSERT Soft Key When Complete: 4. TO MENU CANCEL TO DELETE A FIXFRM (FIX FIRM) IN MEMORY 1. Select: EDIT Mode Turn: MEMORY PROTECT to OFF FAR RIGHT Soft Key till SETTING Soft Key appears on screen SETTING Soft Key 2. Move: CURSOR to desired FIX FORM setting (A or B) A: REGISTARED FIX FORM SENTENCE FOR MILLING B: REGISTARED FIX FORM SENTENCE FOR TURNING SELECT Soft Key CURSOR RIGHT or LEFT to desired TAB Move: CURSOR to select FIX FRM to be DELETED 3. DELETE Soft Key YES Soft Key When Complete: 4. TO MENU CANCEL 168
LATHE FIX FORMS N84(CUTOFF AND TRANSFER); G10P0Z#500M64; Set Main Workshift Value, Encoder feedback from Main Spindle M?S500G97P1; Spindle Direction, Direct RPM, Starts Main Spindle G0T0X#502; Rapid Mode, Cancel Geometry Offsets, Move to X Safe Index Position Z#503; Rapid to Z Safe Index Position G28E#5045Y0M32; Rapid to E Axis Home Position, Rapid to Y 0 Position, Sync Spindles Speeds T?; Index Turret to Cutoff Station M56; Sub Spindle Collet OPEN G4U0.2;M7; Dwell, Phase Sync Spindle Positions G0Z-?; Rapid to Z Cutoff Position E0.1; Rapid E Axis to.1 in Front of Main Spindle Part Face G1G98E-?F100.0; Linear Move, IPM, E Axis Over Part By Gripping Amount M77; Spindle Drive to LOW Torque G4U0.4; Dwell M57; Sub Spindle Collet Closed G4U0.4; Dwell M76; Sub Spindle Drive OFF M78; Sub Spindle Drive Normal Torque X?; Feed To Clearance Point Above Part OD G50S?; Set RPM Limit G96S?; Set CSS G53E#5025; E Axis Verification Position Check G1G99X-0.01F?; Linear Move, IPR, X Cutoff Position, FEED RATE G4U.1; Dwell G28E#5045; Rapid E Axis to Home G97S500; Cancel CSS G0T0X#502; Rapid Mode, Cancel Geometry Offsets, Move to X Safe Index Position Z#503M35; Rapid Main Turret to Safe Position, STOP Sub Spindle Rotation M1; 169
N84(TRANSFER MAIN TO SUB); G10P0Z#500M64; Set Main Workshift Value, Encoder feedback from Main Spindle G97S500M?P1; Spindle Direction, Direct RPM, Starts Main Spindle G0T0X#502; Rapid Mode, Cancel Geometry Offsets, Move to X Safe Index Position Z#503; Rapid to Z Safe Index Position G28E#5045Y0M32; Rapid to E Axis Home Position, Rapid to Y 0 Position, Sync Spindles Speeds M56; Sub Spindle Collet OPEN G0E.2; Rapid E Axis.200 Infront of Z0 Part Position Face G1G98E-?F100.; Linear Move, IPM, E Axis Over Part By Gripping Amount M77; Spindle Drive to LOW Torque G4U.2; Dwell M57; Sub Spindle Collet Closed G4U.2; Dwell M76; Sub Spindle Drive OFF M21; Main Collet OPEN G4U.5; Dwell M78; Sub Spindle Drive Normal Torque G53E#5025; E Axis Verification Position Check G28E#5045; Rapid E Axis to Home M1; Optional Stop (SUB SPINDLE HOME); G28E#5045; (MAIN TURNING); G0G99M64; G28E#5045; G97M?(3,4,13,14)S500P1; G50S?; G96S?; (SUB TURNING); G0G99M65; G28E#5045; G97M?(33,34)S500P2; G50S?; G96S?; M?(COOLANT); (SET TAILSTOCK POSITION); G65P9130A?D?M?C?; (TAILSTOCK FORWARD); M84; 170
(TAILSTOCK HOME); M85; MAIN OD LIVE; G0G98M66; G28E#5045; M23; G97M?(51,52,53,54)S?P3; C0; MILL FIX FORMS (MAIN FACE LIVE); G0G98M66; G28E#5045; M23; G97M?(51,52,53,54)S?P3; C0; (SUB OD LIVE); G0G98M66; G28E#5045; M223; G97M5?(51,52,53,54)S?P3; A0; (SUB FACE LIVE); G0G98M66; G28E#5045; M223; G97M?(51,52,53,54)S?P3; A0; (MAIN LIVE OFF); M55; M24; (SUB LIVE OFF); M55; M224; (MAIN OD LIVE Y/B AXIS); G0G98M66; G28E#5045; M71; G97M5?S?(51,51,53,54); B?(POSITION)M?(COOLANT); (SUB OD LIVE Y/B AXIS); G0G98M66; G28E#5045; M70; G97M5?S?(51,51,53,54); B?(POSITION)M?(COOLANT); 171
SECTION FIVE Sub Spindle Transfer and Operation Prior sections should be reviewed prior to using this section for a more in depth steps on MGi 172
SUB SPINDLE E AXIS (OPTION) The Sub Spindle Option allows for the workpiece to be machined on both ends. This reduces cycle time by eliminating the need for handling and for secondary operations. All functions allowed on the main spindle are allowed on the Sub Spindle. This includes Threading, Rigid Tapping, Live Tooling, and Y and C (A) Axes. SUB SPINDLE WORKSHIFT VALUE The Workshift Value tells the control the distance measured along the Z AXIS from the MAIN SPINDLE FACE to the Finished Sub Spindle Part Face. To determine the correct Sub Spindle Workshift value, refer to the Operator s Manual or Operator s Guide supplied with your lathe. The Sub Spindle Workshift Value is the Distance Measured from Main Spindle Face to Finish Face of Part in Sub Spindle Sub Spindle Z0 Once this value is determined, it MUST be placed in MACRO VARIABLE NUMBER 501. This value will then be loaded through the Manual Guide Program every time a tool change is done. After the Workshift value is entered in to the Workshift file the operator can then touch off all tooling to be used on the Sub Spindle. (Please refer to your OPERATOR S Guide or OPERATOR S MANUAL supplied with your lathe.) 173
SUB SPINDLE (OPTION) (SETTING E AXIS WORKSHIFT VALUE) When using the Sub Spindle Option, setting an E Axis Workshift value will make programming easier for part transfers from one spindle to the other. The programmer will program the Sub Spindle in reference to the Main Spindle Z Zero Position. Once this value is determined it will be stored in the E Axis Workshift File. The programmer then programs the Sub Spindle to a desired position off the Main Spindle Part Face. To Determine the E Axis Workshift Value: 1. Install: Spindle Tooling on Sub Spindle 2. Position: TURRET to a SAFE POSITION to allow MOVEMENT of the Sub Spindle 3. Ensure: There is a finished part in the MAIN SPINDLE at the Correct length E0 (ZERO) Position 4. Select: JOG JOG Sub Spindle (E AXIS) towards Part in Main Spindle 5. Select: HANDWHEEL HANDWHEEL Sub Spindle (E AXIS) till the Sub Spindle tooling is Flush with the Part in Main Spindle 174
6. OFFSET/SETTING Function Key FAR RIGHT Soft Key TWICE W.SHIFT Soft Key 7. Move: CURSOR to MEASUREMENT E Key In: ZERO (0) INPUT Key E0 (ZERO) WORKSHIFT VALUE 175
CUT OFF AND TRANSFER TO SUBSPINDLE This Section will only show you how to enter the CUT OFF AND TRANSFER cycle into the part program. Prior to entering this cycles, the Tool Selections, Spindle Selections, and the FIXFRM (Fix Form) must be entered into the part program. Once the FIXFRM is selected it must be updated. If no or the incorrect Tool Data is entered the simulation will not be correct. When using the Sub Spindle Option, setting an E Axis Workshift value MUST be done prior to running this FIX FORM. This value is to be stored in the E Axis Workshift File. The programmer then programs the Sub Spindle to a desired position off the Main Spindle Part Face. TURNING FIXFRM Soft Key Move: Move: CURSOR to TRANSFER Tab CURSOR to CUTOFF AND TRANSFER INSERT Soft Key 176
The CUT OFF AND TRANSFER FIXFRM is now inserted into the main program. The FIXFRM now has to be altered. See Example Below: Part Diameter 3.0 Length Of Part 1.5 Cutoff Blade Width.125 The following FIXFRM places the SUB Spindle in Phase SYNC N84(CUTOFF AND TRANSFER); G10P0Z#500M64; M?S500G97P1; M? = Spindle Direction M4 G0T0X#502; Z#503; G28E#5045Y0M32; T?; T? = Turret Station and Offset Number T1212 M56; G4U0.2;M7; G0Z-?; Z? = Z Cutoff Position Z-1.5 E0.1; G1G98E-?F100.0; E? = Sub Spindle Rapid over Part E-1. M77; G4U0.4; M57; G4U0.4; M76; M78; X?; X? = Start Point of Cut Off X3.2 G50S?; S? = Maximum RPM S2500 G96S?; G53E#5025; G1G99X-0.01F?; F? = Feedrate of Cut Off Tool F.002 G4U.1; G28E#5045; G97S500; G0T0X#502; Z#503M35; M1; 177
SECTION SIX MACHINING ON THE SUB SPINDLE Prior sections should be reviewed prior to using this section for a more in depth steps on MGi 178
Once the part is transferred to the Sub Spindle the Workshift value MUST be established and entered into Macro Variable #501. This value will then be loaded through the Manual Guide I Program every time a tool change is done. After the Workshift value is entered in to the Workshift file the operator can then touch off all tooling to be used on the Sub Spindle. (Please refer to your OPERATOR S Guide or OPERATOR S MANUAL supplied with your lathe.) 500 = Main Spindle Workshift 501 = Sub Spindle Workshift 502 = X Safe Index Position 503 = Z Safe Index Position Main Spindle 504 = Z Safe Index Position Sub Spindle Displays tool facing towards the Sub Spindle The TOOL DATA Page needs to show the correct Set Number. SET NUMBER 5 tell the control that the Turning Tool is working towards the Sub Spindle. Remember to also place the correct QUADRANT in the TOOL GEOMETRY OFFSET FILE. 179
On the Part Blank Page the WORK ORIGIN Z(SPN 2) W= would have a value to show facing stock. When setting the tool change make sure that there are values for SAFE INDEX SUB (Z) E=. Change WORK OFFSET MACRO # (Number) A= 501 As the drawing shows 501 is the Sub Spindle. 180
When selecting a spindle set the SPINDLE NUMBER S=2. This tells the control you are working on the Sub Spindle When selecting the FIXFRM to be inserted into the program for turning, select the TURNING Tab then CURSOR DOWN to TURN SUB. Once the FIXFRM is inserted UPDATE required data. On line 7 the M33 causes the Sub Spindle to run in the FORWARD Direction. M34 causes the spindle to run in the REVERSE Direction. The P2 on this line tells the Control the Sub Spindle is to be turned ON. On Line 10 there is an M8 command. This turns the COOLANT ON. There is NO command to turn the Sub Spindle and Coolant ON at the same time. 181
PART O2333 (SUB SPINDLE ROUGH AND FINISH TURN).500 Rad. 1.000 3.000.500 1.000 182
When inputting Parameter Values in the ROUGH TURN OUTER. The CUTTING DIRECTION (P) will be set to +Z Once the cycle is inserted into the part program, it will be necessary to create the part figure. The Z Axis clearance values for the part on the Sub Spindle will always be NEGATIVE VALUES. When machining the Part on the Sub Spindle the Z AXIS cutting moves will be Positive. Remember, this is the opposite of machining a part on the Main Spindle. 183
Remember ALL Z Axis moves beyond the Z (Zero) position are positive values. Drawing Direction is moving towards the Right (Sub Spindle Face) 184
When closing the part contour the Z movement will be to the LEFT. Select BLANK to let the control know where the stock is to removed. Once the drawing has been completed and the Part Figure Closed, it is ready to be inserted into the Part Program Select: Select: Key In:: CREATE Soft Key CREATE AS A SUB PROGRAM Desired Program Name OK Soft Key to enter Sub Program into Main Program 185
Once the Sub Program is entered into the Main Program, end it with an M01 Command The Process will need to be repeated for each operation. REMEMBER, When inputting the TOOL CHANGE CYCLE you must input 501 for the Sub Spindle When working on the Sub Spindle, select the correct S Word (S2) Once the information is entered, the TURNING OUTER FINISH Cycle was selected. Note the CUTTING DIRECTION. It is going in the + Z direction. Input all required data then press the INSERT Soft Key 186
Once the Cycle is inserted into the Part Program, you may either Key In the Code M98P31 or move the cursor up to it in the Part Program and do a COPY and PASTE to insert it into the Part Program All operations done on the Sub Spindle, are done in the same way as the main spindle. The main thing to remember is that you must assign the operation to Spindle 2 (G1998 S2) and assign the proper Machining Direction. Remember all moves to the right of the FINISH PART FACE ON THE SUB SPINDLE ARE POSITIVE VALUES. All CLEARANCE MOVES AWAY FRON THE SUB SPINDLE ARE NEGATIVE VALUES. 187
% O0233(MGI PROGRAM) G1900D3.L3.K0.01W0.01 G556T1.W1.X19.V5.E-5.A501. G1998S2. G0G99M65 G97M34(33,34)S500P2 G50S3500 G96S650 M8(COOLANT) G1120P2.Q0.1H100.C0.01D0.01F0.005E0.003V0.005W1.U0.05L0.1M0.1Z10.N2.I0.01K100. M98P31(SUB PART) M1 G556T1.W1.X19.V6.E-5.A501. G1998S2. G0G99M65 G97M34(33,34)S500P2 G50S3500 G96S750 M8(COOLANT) G1126P2.F0.003L0.M0.1Z10. M98P31 M01 M30 O0031(TEST 2) G1450H0.V0.A0. G1451H0.V0.5K3.D0.5L0.M0.T1. G1451H0.5V0.5K1.C1.L0.M0.T1. G1455H1.V1.R0.5I0.5J1.K3.T1. G1451H1.V1.5K3.D1.5L0.M0.T1. G1451H0.V1.5K5.C0.L0.M0.T2. G1451H0.V0.K7.D0.L0.M0.T2. G1456 M99 % 188
% O2333(PART O233 NC CONVERSION) G1Z0.8406 G1900D3.L3.K0.01W0.01 X1.5Z0.7906 G556T1.W1.X19.V5.E-5.A501. G0Z-0.1624 G1998S2. X1.2 G0G99M65 G1Z0.7417 G97M34(33,34)S500P2 X1.3Z0.6917 G50S3500 G0Z-0.1624 G96S650 X1.02 M8(COOLANT) G1Z0.4688 (NC PROGRAM CONVERSION-START) G3X1.2Z0.7417I0.4588K0. G40 G1X1.3Z0.6917 G18 G0X3.2 G0Z-0.0724 X11.633 X3.2 Z-6.8997 G1X-0.0624F0.005 G18 X0.0376Z-0.1224 F0. G0Z-0.1724 (NC PROGRAM CONVERSION-END) X3. M1 Z-0.1624 G556T1.W1.X19.V6.E-5.A501. X2.8 G1998S2. G1Z0.9276 G0G99M65 X2.9Z0.8776 G97M34(33,34)S500P2 G0Z-0.1624 G50S3500 X2.6 G96S750 G1Z0.9276 M8(COOLANT) X2.7Z0.8776 (NC PROGRAM CONVERSION-START) G0Z-0.1624 G40 X2.4 G18 G1Z0.9276 G0Z-0.1624 X2.5Z0.8776 X1. G0Z-0.1624 G1Z0.4688F0.003 X2.2 G3X1.9376Z0.9376I0.4688K0. G1Z0.9276 G1X3. X2.3Z0.8776 G0X11.633 G0Z-0.1624 Z-6.8997 X2. G18 G1Z0.9276 F0. X2.1Z0.8776 (NC PROGRAM CONVERSION-END) G0Z-0.1624 M01 X1.8 M30 G1Z0.9224 % G3X1.9376Z0.9276I0.0688K-0.4536 G1X2.0376Z0.8776 G0Z-0.1624 X1.6 G1Z0.8954 X1.7Z0.8454 G0Z-0.1624 X1.4 189
A (C) AXIS MACHINING ON THE SUB SPINDLE PART PROGRAM 155 (SUB SPINDLE A (C) AXIS FACE MILL) When doing Live Tooling Machining on the Sub Spindle the axis selection will not be C Axis like the Main Spindle. On the Sub Spindle it is called the A Axis When using the Sub Spindle Live Tooling Option, the tools (End Mills, Drills, Taps, Etc.) MUST be defined correctly and the Proper SET MUST BE SELECTED. For Milling on the Sub Spindle we are using SET POSITION Number 4 Remember the radius of the tool being used MUST be entered into the TOOL GEOMETRY OFFSET File and the QUADRANT Must be set to 0 (ZERO). Program Name and the Part Stock Dimensions are defined into the control. This is done with NEW PROGRAM function and the G1900 Block of information. After this is entered, the correct Spindle MUST be selected for the control. Remember, when using the Sub Spindle you must select SPINDLE 2. FIX FORM for SUB SPINDLE LIVE FACE Once SPINDLE 2 is inputted into the program, select the TOOL CHANGE CYCLE. Remember, to set the WORK OFFSET NUMBER to 501 Select the Mill Cycle FIXFRM then SUB FACE LIVE. UPDATE all required data. 190
PART NUMBER 155 2.000 Diameter 1.000.500 191
You will now need to select the MILL CYCLE Soft Key Mill Cycle Soft Key Since we are doing a Circular Pocket on the part face, select the POCKETING TAB, POCKETING ROUGH, then SELECT Soft Key. You will need to key in the required data on the CUT CONDITION TAB 192
Completely fill in the data on the DETAIL TAB When completed press the INSERT Soft Key and insert it into the part program. Once the POCKETING information is inserted in to the Part Program, the MILLING FIGURE Page will appear. Select the POCKET FIGURE, then move the cursor DOWN to #2 XC CIRCLE CONCAVE. 193
When the XC CIRCLE CONCAVE is selected the following screen will appear. You will need to input the required information. The BASE POSITION will be 0 (ZERO) Face of the Part. The DEPTH/HEIGHT will be -.500 inches. The FACE POSITION screen you will need to select the FACE Soft Key. On the ROTATIONAL AXIS Screen you must select the A Soft Key. This tell the control that the you are doing C Axis work on the Sub Spindle. NOTE: The Control cannot have two C Axes. The Main Spindle is called the C Axis and the Sub Spindle is called the A Axis. 194
After the Information is entered insert the cycle into the Part Program. To end the Program select the M+; Soft Key and insert the M30; into the Part Program % O0155(SUB SPINDLE FACE MILL) G1900D2.L2.3K0.05W0.05 N7(FACE MILL) G1998S2. G556T7.W7.X12.V7.E-7.A501. G0G98M66 G28E#5044 M223 G97M51(51,52,53,54)S3000P3 A0 G1040L0.2J0.1K0.H0.F7.V7.E5.W2.B0.001C0.1Z2.A0. G1521T3.B0.L-0.5H0.V0.R0.5Z2.Y2. M30 % 195
% O1555(SUB SPINDLE FACE MILL O155 NC CONVERSION PROGRAM) G1900D2.L2.3K0.05W0.05 N7(FACE MILL) G1X0.596 G1998S2. G2X-0.596I-0.298J0. G556T7.W7.X12.V7.E-7.A501. X0.596I0.298J0. G0G98M66 G1X0.594 G28E#5044 Z-0.1F78.7 M223 X0.196 G97M51(51,52,53,54)S3000P3 Z0.3 A0 Z0.5F5. (NC PROGRAM CONVERSION-START) G2X-0.196I-0.098J0.F7. G40 X0.196I0.098J0. G12.1 G1X0.596 G1X0.196A0.F78.7 G2X-0.596I-0.298J0. Z-0.1 X0.596I0.298J0. Z0.1F5. G1X0.594 G2X-0.196I-0.098J0.F7. Z-0.1F78.7 X0.196I0.098J0. G13.1 G1X0.596 G0Z-2.822 G2X-0.596I-0.298J0. X5.306A0. X0.596I0.298J0. G18 G1X0.594 F0. Z-0.1F78.7 (NC PROGRAM CONVERSION-END) X0.196 M30 Z0. % Z0.2F5. G2X-0.196I-0.098J0.F7. X0.196I0.098J0. G1X0.596 G2X-0.596I-0.298J0. X0.596I0.298J0. G1X0.594 Z-0.1F78.7 X0.196 Z0.1 Z0.3F5. G2X-0.196I-0.098J0.F7. X0.196I0.098J0. G1X0.596 G2X-0.596I-0.298J0. X0.596I0.298J0. G1X0.594 Z-0.1F78.7 X0.196 Z0.2 Z0.4F5. G2X-0.196I-0.098J0.F7. X0.196I0.098J0. 196
SECTION SEVEN Y AXIS MACHINING CYCLES (Optional) Review prior sections for more in depth steps on using MGi 197
Y AXIS OPTION The Y Axis option allows the Turret/Tooling to move perpendicular to the base of the lathe in the positive and negative directions. This feature is ideal for milling on the OD of the part and producing holes on the face of the part, off the spindle Centerline. The limitation of this feature is the maximum movement in the Y an X Axes. Y Axis Turret Movement +Y +X -X -Y Lathe Bed +Y +X Hole #2 Hole #3 Hole #1 -X -Y The above example, Hole Number 1, requires the tool to move below the X and Y Axis Centerline in the Minus direction. When using the X/Y machining function the turret Tooling moves not the spindle. This type of move will cause a X OVER TRAVEL Alarm. When producing Holes #2 and #3, both the X and Y Axis movements can be made. 198
When producing a pocket or an island on the face of a part with the Y and X Axis movement, the tool will start at Point 1 then move to Point 2 then to Point 3. When the control tries to move the tool to Point 4, it will have to move on the Negative Side of the Spindle Centerline in the X Axis direction. This will cause an alarm -X OVER TRAVEL. When using the X/Y machining function the turret Tooling moves not the spindle. The only way to machine this pocket/island is by using the POLAR (C AXIS) function. +Y +X 1 2 3 4 -X -Y 199
PART 26.500.750 1.000 200
When doing Y Axis machining, the correct TOOL SET Data MUST inputted into the control. Remember to input the RADIUS value of the End Mill into the GEOMETRY OFFSET RADIUS File. You will need to create the Part Program Number. Once that is entered into the control, insert the PART BLANK information and the TOOL CHANGE INFORMATION. Remember to input the correct WORKSHIFT NUMBER. Once the tooling information is inputted into the program, the insert the SPINDLE SELECTION. 201