Download
Share
Print this page
Anilam 5000M Training Manual
  1. Manuals
  2. Brands
  3. Anilam Manuals
  4. Control Panel
  5. 5000M
  6. Training manual

Anilam 5000M Training Manual

Cnc control
Hide thumbs Also See for 5000M:

Advertisement

Quick Links

Download this manual See also: Installation Manual
5000M
CNC Control
TRAINING GUIDE

Advertisement

loading
Need help?

Need help?

Do you have a question about the 5000M and is the answer not in the manual?

Questions and answers

Related Manuals for Anilam 5000M

Summary of Contents for Anilam 5000M

  • Page 1 5000M CNC Control TRAINING GUIDE...
  • Page 2 Navigation Instructions Bookmarks Follow the bookmarks at the left side of the page to navigate to desired topic. Click plus and minus symbols to expand and compress menu display.
  • Page 3 6000M CNC CONTROL TRAINING GUIDE...
  • Page 4 Turning the Control ON After the control has been turned ON press F10 to continue. 1. Control Software This allows you enter CNC software 2. Setup Utility Machine configuration 3. Motion Setup/Testing Used to setup drive Then press ENTER to select CNC mode.
  • Page 5 First CNC Screen Control Manual Screen SECTION #1 SECTION #2 SECTION #3...
  • Page 6 Section #1 Mode of operation Machine position status Program name Machine status Messages display in this area Command line for MANUAL(MDI) instructions Error and warnings Section #2 Position relative to machine HOME Target or position to reach Distance to go to reach target Position relative to part ZERO...
  • Page 7 Section #3 Active tool # Number of loops Tool diameter Tool length offset Dwell in seconds Spindle speed Feedrate Active fixture offset Percentage of feed and RPM’s Active G codes Active M functions Parts counter and timer Override of feed and rapid...
  • Page 8 Softkey in Manual Mode Access tool Delete from Access help Edit program Single Step page command line menu in memory Mode Automatic Insert in Manual Mode Access list of Activate Mode command line programs handwheel Note:When handwheel is active colors will be reversed in box as shown below.
  • Page 9 Alfa - Numeric key board Note :- Most used key are yellow . Most key also double functions , the shift key is use to use secondary functions. < > ‘ ‘ Clear key & “ mm/in Dwell Plane Feed Tool Mcode Rapid...
  • Page 10 Manual panel There are two type of Manual panels. 1.As shown below. 2.The other without Handwheel on left side Manual spindle keys Manual handwheel Spindle override Feedrate override Servo reset FEED SERVO SPDL SPDL SPDL RESET RAPID % FEED % SPDL OVRD AXIS Hold Axis feed type...
  • Page 11 MOVING WITH JOG MOVEMENTS 1) Turn the jog mode selector switch on the MANUAL PANEL to 100, 10, 1, FEED or RAPID 2) Select the axis to move with the AXIS SELECTOR switch at the MANUAL PANEL 3) Press the or the key to move in the desired direction.
  • Page 12 MOST COMMON G-CODE COMMANDS TO REMEMBER: G00: Rapid move. G01: Feed move. G02: Arc clockwise G03: Arc counter clockwise G17: XY plane G18: XZ plane G19: Yz plane G40: Cutter comp off G41: Cutter comp left G42: Cutter comp right G53 Ox: Fixture offsets ( absolute shift from Machine Home).
  • Page 13 ADDRESS LETTERS USED IN PROGRAMMING Used for angles around X axis. Used for angles around Y axis. Used for angles around Z axis. Designates tool diameter in a program. Feedrate. Circle center X axis. Circle center Y axis. Circle center Z axis. Dessignates tool length in a program.
  • Page 14 RETREIVING PROGRAMS FROM DISK Transferring a program from a disk into the control Programs can be restored into the control if they have been previously saved on a disk. Insert the disk into the floppy disk drive (A:) on the machine. Program From the MANUAL mode press then press SHIFT...
  • Page 15 Keys to use when using Computer key board FUNCTION CNC KEYBOARD COMPUTER KEYBOARD X Axis Command X Key Y Axis Command Y Key Z Axis Command Z Key G Key Preparity G Code M Key Machine Function Code S Key Spindle Function Code ‘...
  • Page 16 6000M CNC CONTROL HELP MENU’S...
  • Page 17 The HELP MENU’S are access by pressing. HELP This can be done from either Manual or Edit. Manual mode soft keys Edit mode soft keys First Help screen Note: The center of the screen. There are two different displays, one has text about Help the other shows the program as it is being entered.
  • Page 18 There are two different set of soft keys , as shown above. Arrow up and around to desired selection. Arrow down and around to desired selection. Not used. Text changes center of screen to diplay program. Text Selects required cycle.Enter will as do this. Select ReEdit ReEdits a cycle after it is already in a program.
  • Page 19 Section as shown below these are the major defaults. Hight lite the required in put and press either enter. Select Use up arrow key to move hight to next selection.
  • Page 20 Press the number 2 key or arrow up to number 2 . Select Press either enter Note:- the reverse color around Compensation. Press either Select enter 1. Puts a G40 into program comp off. 2. Enters G41 into program cutter comp left. 3.
  • Page 21 Rotation G68 Center of rotation X axis. Center of rotation Y axis. Start angle when using loop. Angle between loops or single shot. Subroutine #. Number of repeats. Note:The only entry that has to be program is C because it has 0 (Zero’s) next to it.
  • Page 22 Scaling G72 When using scaling if threre are any the axis must be scaled the same on both of these axis.If part is required to be half size .5 would be factor. G72 alone will turn off scaling.
  • Page 23 Lines Press # 3 either Select enter. Screen will now appear as below. Inputs will change according to which plane is active. 2. X axis input only. 3. Y axis input only. 4. X and Y axis. 5. Angle and X axis. 6.
  • Page 24 Arc’s Press # 4 either Select enter. Screen will now appear as below. Tool must be at start point before inputting arc’s Centers of arcs X=I , Y=J and Z=K Inputs will change according active plane. 2. Radius and End Point. 3.
  • Page 25 Corner Rounding And Chamfering Press # 5 either Select enter. Screen will now appear as below. 2. Radius One shot corner rounding.Inputs mid point X / Y,radius and end point X/Y. 3.Chamfer One shot chamfer. Inputs mid point X/Y, chamfer and end point X/Y.
  • Page 26 Multiple line, arc and chamfer moves. Press # 6 either Select enter. Screen will now appear as below. Tool must be positioned at start point. Inputs will change according to active plane. 2. Definition Inputs first angle, second angle and end point. 3.Radius Inputs first angle, radius, second angle and end point.
  • Page 27 Pockets Press # 7 either Select enter. Screen will now appear as below. Cutter comp is built into all pocket except Mold Rotation. X and Y centers are Optional but if not entered will assume it is positioned at center of pocket.
  • Page 28 Frame pocket G75 Only the input with in Zeros have to be entered the rest are optional. It will assume being at the center of pocket if no dimension are entered. X Center Center of pocket X axis.If not entered will assume tool is at center of pocket.Optional Y Center Center of pocket Y axis.If not entered will assume tool is at center of pocket.Optional Length of island (X).
  • Page 29 Circular pocket G77 X Center Center X axis. Optional Y Center Center Y axis. Optional Z Start Hgt. Start height .1 above surface to be cut into. Z Depth (abs) Absolute Z depth. Diameter Diameter of pocket, comp built in. Stepover Move over per pass.
  • Page 30 Area Clearance G169. Input Sub # Subroutine number. X position tool will Z down into part Y position tool will Z down into part Z Start Hgt. Start height .1 above top of pocket Z Depth (abs) Total depth of pocket absolute Cut Angle Used if starting in middle of radius X Start...
  • Page 31 Elbow Milling G49 Start Radius Radius at start of Elbow End Radius Radius at end of Elbow Included Angle Included angle Num of Cycles Sub. Profile forward direction X Center Sub. Profile Reverse direction Y Center Axis rotation is around X,Y or Z Direction CCW+ Center line X or Y if not Zero End Angle...
  • Page 32 High lite plunge pockets press Plunge Circular Pocket G177 X Center Center X axis Optional Y Center Center Y axis. Same as above. Optional Z Start Hgt. Start height .1 above surface to be cut. Z Depth (abs) Absolute Z depth. Diameter Diameter of pocket, comp built in.
  • Page 33 Pockets with Islands (G162) Format: G162 An Bn Cn Dn En This cycle allows islands in irregular pockets. The main pocket must the lowest subroutine number. Normally, this would be one (1). Pockets with Islands can be programmed using: • DXF (see “Section 17, Using DXF for Pockets with Islands (G162)”) •...
  • Page 34 Figure 5-13, Subroutines Pockets with Islands Example Workpiece Table 5-22, Pockets with Islands Subroutines Programming Example G00 G17 G70 G90 T1D.0205 L-1 M6 S1250M3 G53O01 G162 A2 B3 C4 D5 E6 G162 A7 B8 C9 D10 G162 A-11 B12 C-13 D-14 G169 W1 H0.1 Z-0.0050 C299.
  • Page 35 X1.2598 Y0.5 X1.2226 X1.2135 Y0.525 X1.1507 X1.1416 Y0.5 X1.1044 G00 Z0.1 X1.1634 Y0.56 Z0.1 G01 Z-0.005 G01 X1.1821 Y0.6112 X1.2007 Y0.56 X1.1634 G00 Z0.1 X1.4007 Y0.55 Z0.1 G01 Z-0.005 G01 X1.3612 G02 Y0.6 I-0.0312 J0.025 G01 X1.4007 G03 Y0.55 I-0.0707 J-0.025 G00 Z0.1 G0 X1.42Y.5 G1 X1.42Y.65...
  • Page 36 #2. Ellipse. Produces an ellipse, uses special cutter comp. #3. Spiral. Will cut a tapered thead. #5. Facing. Faces large surfaces. #7. Circular Profile Cut circle either inside or outside. #8. Rectangular Profile. Cut rectangle inside or outside.
  • Page 37 Ellipse G05 Note: All dimensions are INCREMENTAL. End Horizontal Distance from start to end X axis. End vertical. Distance from start to end Y axis. Center Horizontal Distance to center from start. Center Vertical Distance to center from start. Half lenght Half length of ellipse x axis Half width Half width of ellipse Y axis.
  • Page 38 Facing G170 Length Increamental length X axis. Width Increamental width Y axis. X Stepover Stepover X . Y Stepover Stepover Y. Feedrate Feedrate. Z Start hieght Start height .1 above surface. Finish depth. Z Depth Absolute X Start Start X axis. Y Start Start Y axis.
  • Page 39 Circular profile G171 Center X. X Center (optional). Center Y. Y Center (optional ). Start height. Start height above surface to be cut. Diameter. Diameter of pocket (actual). Z depth (absolute). Depth to be cut (absolute). 0 = inside, 1 = outside. 0 insde ,1 outside of circle.
  • Page 40 Thread Mill Cycle (G181) Format: G181 Xn Yn Zn Hn Pn Dn Cn Bn Rn Sn En Jn Kn Vn WARNING: The first move in this cycle is a rapid move to the center of the thread before moving the Z axis. Make sure the tool is properly located before calling up this cycle.
  • Page 41 Table 5-28 describes the Thread Mill Cycle entry fields. Table 5-28, G181 Address Words Address Word Description Absolute X coordinate of the center of the thread. If no coordinate is entered, the CNC puts the center of thread at the current tool position. (Optional) Absolute Y coordinate of the center of the thread.
  • Page 42 Table 5-28, G181 Address Words Address Word Description Feedrate for roughing. (If not set (blank), the cycle will use the current active feedrate) (Optional) Feedrate for the finish pass. (If not set (blank), the cycle will use the current active feedrate) (Optional) Angle on one side of the thread, (not the included angle).
  • Page 43 Sample Thread Milling Cycle Program G0 G90 G70 G17 T1 M6 S2000 M3 X0 Y0 G181 Z-1. H0.1 P.5 D1. C.0625 B8. R.1 S.002 E2 J20.0 K5.0 With a cutter diameter of 0.625, this program will cut a 1-8 inside thread at X0 Y0.
  • Page 44 Drilling Cycles G80 Series Note:That there is now a G80 in the first box on left. All G80 cycles must be turn OFF with a G80 as soon as drill operation is finished.
  • Page 45 Basic Drilling Cycles G81 Finish Depth. Finish depth of hole. Start height above surface to be drilled. Start Hgt. Feedrate. Feedrate for drilling. Return Hgt. Return height if higher than R plane. Counter Boring Cycles G82 Finish Depth. Finish depth of hole. Start Hgt.
  • Page 46 Tapping Cycles G84 Finish Depth. Finish depth of hole. Start Hgt. Start height above surface to be drilled. TPI/Lead. TPI if inch/Lead if MM. Spindle. Spindle sync. 0 = OFF, 1 = ON Return Hgt. Return height if higher than R plane. Dwell time Dwell at bottom if necessary.
  • Page 47 Chip Breaking Cycle G87 Finish Depth. Finish depth of hole. Start Hgt. Start height .1 above surface to be drilled. Feedrate. Feedrate for drilling. First Peck. Amount of first peck. Delta Peck. Amount to decrease peck each peck. Minimum Peck. Smallest peck amount.
  • Page 48 Bolt Hole Circle Drilling G79 Center. Center X axis. Center. Center Y axis. Index Angle. Angle to rotate 0 angle from 3 o’cclock. First Angle. Angle of first hole from 0. Last Angle. Angle of last hole, if full pattern not required. Number Holes.
  • Page 49 G-Code without Graphics Dwell In seconds with Tn Exact stop will stop exactly in positiion one shot. Stroke Limit set a box that tool cannot move outside or inside. Reference Point Return sends machine home in designated axis. Reference Point Return Fixture offset Absolute zero shift from Home.
  • Page 50 6000M CNC Control Program Management...
  • Page 51 INTRODUCTION The Program Directory provides access to all the program management and disk utilities. These functions include Creating, Selecting, Deleting, Undeleting and Copying programs. The Program Directory also provides access to the Floppy Drive utilities. Accessing PROGRAM DIRECTORY page. Program (1) From the MANUAL mode press: The Program files are listed in alphabetical order.
  • Page 52 Method No.2 Copying and using an existing program. If a similar program to that required already exists, it may be copied and given a new name. This allows similarly formatted programs to be used without having to re-type the information. (1) Using the keys High Light the existing program to be copied Utility...
  • Page 53 To UNDELETE / RESTORE a deleted program. Should a program become accidentally deleted the following method can be used to restore the program. NOTE: The restore capability of the system is determined by the space available on the drive. If the space on the drive where the program was stored has been reused restore will not be an available function.
  • Page 54 When in the PROGRAM directory the drive and directory are displayed in the lower left corner of the screen. The 5000M uses the A:/ drive for the Floppy Disk Drive. Programs may be copied to or copied from the Floppy Drive individually or in multiples.
  • Page 55 To COPY a program from the A: Drive (Floppy Disk) to the Program Directory C:\USER The 5000M uses the A:/ drive for the Floppy Disk Drive. Programs may be copied to or copied from the Floppy Drive individually or in multiples. To view or copy the programs on a Floppy Disk, the operator...
  • Page 56 To COPY program files to the A: (Floppy Disk) when using the CAM When using the CAM Editor to write programs the 5000M system will create additional program files, and ALL these files MUST BE COPIED to ensure correct operation of the program.
  • Page 57 To COPY all the program files to the A: (Floppy Disk) when using the CAM continued….. The 5000M uses the C:/USER drive in the Program Directory. Upon entering the Program Directory the programs displayed will all have an extension of .G To view all the program files described on the previous page the operator must first LOG to the the root of C:\USER directory (this is where all program files with any extension can be viewed).
  • Page 58 To COPY all the program files to the A: (Floppy Disk) when using the CAM continued….. An alternative method is also provided to obtain the screen showing all programs with all extensions Directory. Display This method is completed using the keys.
  • Page 59 To COPY all the program files to the A: (Floppy Disk) when using the CAM continued….. To COPY all the EXAMPLE program files shown below complete the following: (1)Use the keys to High light the first program to be copied (EXAMPLE.1) to the Floppy Drive (2) Using the key High light the remaining EXAMPLE program files Utility...
  • Page 60 6000M CNC CONTROL Simple Program...
  • Page 61 CREATING A PROGRAM PROGRAM From Manual page press The softkeys will changed as shown below. CREATE Press Type the program name (Maximum 8 letters/numbers). Press Enter put into program directory...
  • Page 62 High light will be on program just created. Press EDIT...
  • Page 63 This is how screen will appear when entering EDIT Program name Note: Insert is turn ON ,if not will not go past bottom of page. Note:Softkeys have change .
  • Page 64 X0 Y0 2.75 This part needs to have 4 hole drilled .25 dia and .5 deep...
  • Page 65 Press HELP High light will be on G0 press enter Move high light G17 , G70 and G90 press enter on each of these. Press M5 press Press it will go into program as shown below. Exit...
  • Page 66 Top line of program. Program has been edited Cursor position line and column Lines 2 and 3 are typed in manually. The * allows commence into program control will read ignore after it.
  • Page 67 Press press #9 for DRILL press HELP Screen will appear as shown below. Press #2 for basic drilling, press enter.
  • Page 68 Enter values Finish Depth -.5 press down arrow, enter Start Hgt .1 down arrow and Feedrate 12 Press exits help menu and enters line into program. Exit The next enter hole positions. Type G0 X.75 Y.5 X2.75 Y1.5 X.75 Type G80 Cancel drill, this must always in program after last hole.
  • Page 69 Type in last three lines. Press press Exit Draw Soft key will change as shown below. Fit to screen Edit program Zoom window Exit draw mode Half current size Double current size Run program Scale drawing Pans part around screen Erase screen View XY plane Displays text ----------------...
  • Page 70 Press cursor will be on FIT press enter DISPLAY This will fits drawing to screen. Red lines are RAPID moves , blue circle are the holes and purple circle is the tool. Press this brings control back to program page Exit Press to select program ,check that high light is...
  • Page 71 SETTING PART ZERO. If using an edge finder , touch edge of part using jog keys. Go to tool page press press Tool OFFSETS Cursor to required OFFSET using arrow up and down keys. Move X axis until part is located with edge finder. Press this will enter value into table.
  • Page 72 SETTING TOOL LENGTH OFFSETS Put tool in spindle , bring tool tool down to top of part. Tool Press high light correct tool number in tool page press CalibZ If there are more move Z axis up change to next tool and calibrate it as before,tool #0 must always be active when setting offsets.
  • Page 73 6000M CNC CONTROL GENERATING PROGRAMS USING CAM...
  • Page 74 STEP BY STEP CREATION OF A PROGRAM USING THE SHAPE EDITOR The following presentation shows a step by step procedure of how to create a part program using the Anilam 5000 Control. This procedure details the use of the interactive CAM that creates the part profile through simple entry of geometrical elements (points, lines and circles) without having to calculate intersections, tangency points etc.
  • Page 75 - High light the name the needs the program for, press - The machine program can be coompletely produced in CAM. Line tool Arc tool Geometry tool Corner radius Corner chamfer Chaining tool When Shape is press, soft keys will change as shown below. F4- Back Moves curser backwards on a shape.
  • Page 76 Pressing S-Edit the following pop-up menu will appear Create Create a start point for a shape. Copy Copy a shape to another location. Move Move a shape to anew location. Delete Delete a shape. Rev Arc Reverses direction of an arc in a shape. Project Replaces a radius and joins lines.
  • Page 77 Display Pressing the following pop-up menu will appear Fit to screen. Zoom in on windowed area. Redraw screen Half size of screen. Double size of screen. Scale screen. Pan move part around on screen. Erase screen. Misc Pressing the following pop-up menu will appear List shapes by number.
  • Page 78 Setup Pressing the following pop-up menu will appear Parameters for CAM. Turn shapes ON/OFF. Turn geometry ON /OFF. Turn tool paths ON/OFF. Parameters for post. When high light is on setting press the pop-up menu will appear. Type of dimensioning ABS/INC. Units INCH/MM.
  • Page 79 The part below needs to be pocketed. 6.25” 2” rad X0 Y0 4”rad 3.75” 1.8”rad...
  • Page 80 When CAM is accessed The high light will be on the top left icon, for the following exercise the third icon down is the one required. Press down arrow key twice icon on right will become point definitions. Enter a point using X & Y coordinates. Increamentally move from an existing point.
  • Page 81 Press icon on right will change to line definitions. A line along X axis. Aline along Y axis. Aline between two points A line through a point at an angle. A line parallel to an existing line. A line tangent to a circle through apoint. Press to get to circle icons.
  • Page 82 High light third Icon down on left. Press right and then up. Circle icon high lighted Geometery icon turn blue. 6.25” 2” r X0Y0 4”r 3.75 1.8r Press R value =4 Press It will now ask for center definition and point definition will appear in right column of icons.
  • Page 83 Press Fit and screen show the circle that was just entered. Display 6.25” 2” r X0Y0 4”r 3.75” 1.8”r Using same icon put in 2” radius ccircle. Press enter 2” for radius Press press to select point value X0 , value Y 4.25 (6.25-2) press Two circle will now show up on screen.
  • Page 84 The next element required is the 1.8 radius arc. In order to do this it is necessary put in some constrution geometry. First a line has to be draw at -3.75 in the Y axis. 6.25” 2” r X0Y0 4”r First high light geometry icon as shown below, 3.75”...
  • Page 85 The next geometry required are two points at the intersect of the 4” radius circle and the -3.75 line. To do this use icon circled below. These are the two points that needed to be found. They are the intersect of circle #1 and line #3. Press Enter number of first element 1 press second element 3.
  • Page 86 It is now posible to drive an arc between points #4 & #5. 6.25” 2” r X0Y0 4”r 3.75 1.8r Use the Icon that allows a circle between two elements. First question R value. Press Second question Press Third question Press...
  • Page 87 Point required for start It is necessary to figure the best place to start. On this part the top will allow us to completely clean this shape. 6.25” 2” r X0Y0 4”r 3.75 1.8r Use icon circled line tangent to a circle at an angle. First question Press Press...
  • Page 88 All the necessary geometry has been established, the next thing is to make a shape, to pocket and contour. Press S-Edit A start point needs to be established for are shape, high light will be on Create. Create will set where the shape is going to start. Press select point definition,Use the icon circled.
  • Page 89 Enter 8 when it says “From point” Press Press The white number one is the start point for shape #1. The icon circle is the construction icon, high light it press it will ask for an element tobe selected. Enter -2 press When selecting circles if cutting in clockwise the number is positive if counter clockwise the number is negative as shown above.
  • Page 90 The next selection is -1 and there are selection 1 and 2, inthis case 2 is required. Press 2 Notice that after 2 was selected element #2 when from green to white and element #1 became green. The next element is #6, this is positive because the direction is clockwise. Press 6 select #2 press -1...
  • Page 91 The geometry and shape are complete, the next is to produce a tool path to pocket and contour. Press Motion The first tool path is pocket using arrow keys high light pocket press. Press...
  • Page 92 There are two methods of entering tool diameters, direct just type in value and select it from toll table. Tool table A pop-up window will appear as above. To enter a value in any of these parameters first press enter value press When More is reached it will bring up anew pop-up window.
  • Page 93 Second page of parameters. Angle of cut can be left at default or an angle entered, on this part an angle of 200 deg’s will be entered. Entry and Exit Move these are the three options. Linear is straight line move on to start point, circular ram on move. Arc Length is the angle arc ramping on move.
  • Page 94 Coolant turn ON at start but not OFF at end as the same tool will be used for pocketing and contouring. The same applies with spindle. Press Press Cont Cont Press Calc On the right is how it will appear on screen. Red is geometry.
  • Page 95 The Contour now need to be done as the edges are still rough. Press press Motion It now needs to know which side to put tool comp. Stepover this is around contour only. Number of passes around contour. Do this for both Entry and exit moves.
  • Page 96 There is no need for a tool change because the same tool is being use for the contour as pocketing. Note: Coolant and spindle at start are entered as None and turned Off at end,as they are still on from pocketing. Pocket tool path #1 Profile tool path #2...
  • Page 97 Arrow down to post Setup If machine has a tool changer arrow down to Tool Change press enter arrow down to Tool Change Format if M06 is required it should read as follows T%02DM06. Block Number are set to start at 10 and increament by 10 this can be change dependinng on your preferance.
  • Page 98 High light EXAMPLE.G press Draw press fit will be high lighted press Display XY view Isometic view All that is left to do is set tool length offsets and fixture offsets, part is ready to run.

  • Page 99: Press

    If the G-Code Configuration is now correct it can be save for future use. Press Display until top left corner shows Utility ..\ high light EXAMPLE.CAM press high light will be on Copy press Arrow down to Other Type in C:\P5M\DEFAULTS.CAM...
  • Page 100 6000M CNC CONTROL DXF Converter...

  • Page 101: Press -1

    DXF file can be converted into 5000 machine programs using the Offline software. The DXF files are stored in the Program Page. When going to Program Page only .G and/or .M file will be displayed,press shift twice, this will Display display all files on Program page.
  • Page 102 File name Select: Used when selecting elements on drawing. Layers: Allows layer on drawing to be turned Off or On. View: XY,XZ,YZ or isometric. Display:Fit, window, redraw, half or double. Save: Saves program with .G once converted. Setup: Allows setup of inputs and outputs. Exit : Goes back to Program page...

  • Page 103: Press

    Zero on most drawings is usually not at a point that is covenient for programing, so there is a way it can be changed. In the case of current drawing, the center of the hole in center of part is the best point X0 Y0.
  • Page 104 Exit Press Press ALTkey and letter Fkey at the same time, this will mark the end of each element. DISPLAY Press high light Window press A box will appear on screen move around sceen using press Compress position box as shown below press...
  • Page 105 Press point mouse arrow to lower end of a line as shown Select and pess left mouse key. Line will turn green as above and put a number at low end of line, the position of the number is the start point. Now point to the line below it and press left mouse key, all off the line will be come green.
  • Page 106 Save Press Press Exit Press Press Y it will now return to Program page. High light .G or .M file press Edit...
  • Page 107 High light .M file press Edit in coversational will appear as below Start of program End of program Program has to be Edited , to put in tool changes or cutter comp and Z moves. High light .G file press Edit in G code format will appear as below Program has to be Edited , to put in tool changes or cutter comp and Z moves.
  • Page 108 This example will show multiple subroutines. Select and pick all holes that are the same size , in this Press case 8. When going to second set of holes press right key on mouse. The green circle is the last of previously selected holes. The yellow circle is the one selected with right mouse button and in the bottom left it is asking if this is a new shape, the answer is Y .It will put a number 2 next to this hole, meaning this is shape 2.
  • Page 109 The print below shows the four shapes of the different size holes. Press Save Press Exit...
  • Page 110 Below is the output from the DXF converter. Some editing is required to put in drilling cycles. Subroutine calls Subroutine for positions of the eight holes numbered in black. Subroutine for positions of the two holes numbered in green. Subroutine for positions of the two holes numbered in blue.
  • Page 111 The program below is Edited with the drill cycles in the program.
  • Page 112 In this example of a full drawing and how to turn off unnecessary information ,such as dimensions etc.
  • Page 113 Layers Press High light Toggle Layers press Put high light on layers not required and press to turn OFF. In the drawing shown the only layer required to be left on is #11...
  • Page 114 Only the part profiles and holes are left. The circled area is blown up below. It show an error in the drawing , where two lines are not connected. It will stop, select next element and the following message will appear. Press Y to continue.