DIGI9 Lathe Controller

Transcription

1 DIGI9 Lathe Controller Contents Introduction Quick start guide G codes Other Codes Setting up for machining Program development Glossary Dot points Support for other controllers Important notes ED1005 9:13:23 pm 26/06/2014 V11 Page 1

2 Introduction The Digi9 controller is a fully functional closed loop digital controller utilising an industrial 32 bit embedded controller. The controller allows the operator to run G code programs and fully automate the machining process. It also allows manual operation of the machine. The controller s firmware contains powerful canned cycles that minimise code size and program development time. G Code programs can be developed with the accompanying software D9MAC, utilising code wizards, DXF file input from your favourite cad package allowing point and click code generation or imported G code from third party G code generators. Programs can be simulated in a no frills graphic display. This allows convenient program verification before actually machining anything. Tool graphics can also be adjusted. Programs are downloaded to the machine via the USB port. Other features Manual pulse generators (MPG) allow the machine to be operated manually. A display which shows the axis positions in cycle mode or manual operations either for simple jobbing work or for machine set-ups. Feedrate override via the LH MPG Spindle speed override via the RH MPG ED1005 9:13:23 pm 26/06/2014 V11 Page 2

3 Quick Start Guide The Quick Start Guide will have the machine operating with a valid program within minutes. This section demonstrates the first concept to finished product procedures, which are typical using this system. These instructions will produce a program with some default movements. When run, the program will start the spindle and move its axis albeit away safely from the chuck. When using the software you must click in the simulation window to activate the Simulation, Downloads and Other files menus. There is on YouTube a video which shows the following steps, it can be found at To Generate the code. For safety, remove all tooling and billets from the machine Connect the USB download cable to the PC and turn on the machine. 1) Launch the D9mac utility. 2) Select the Code Wizard menu item. 3) Select Initialise. The dialog will then change to Tool Setup page. Pick a right hand tool and select it as tool 1 and click OK to accept all other default tick boxes. At this point code will have been generated and will appear in the editor window to the left. The code wizard is designed as a top down sequence. This sequence loosely represents the procedural order you are likely to want when producing a program when using the code wizard. In fact, clicking on all of the features here (with appropriate tool changes) will produce a valid program that will produce a part based on the stock size. ED1005 9:13:23 pm 26/06/2014 V11 Page 3

4 Quick Start Guide 4) Select the Code Wizard menu item again. 5) Select Stock Removal. A dialog will appear giving Stock Removal options. Tick the following boxes. External, Generate a default framework and finally Add toolpath graphic syntax. Click on OK. More code will appear in the Editor Window to the left and the toolpath graphic will appear in the Simulation Window 4) Select the Code Wizard menu item again. Select Terminate. This will generate code to send the machine home, stop the spindle and end the program. The code will appear in the Editor Window. Your screen should look like this ED1005 9:13:23 pm 26/06/2014 V11 Page 4

5 Quick Start Guide Note the code generator will generate code at the current caret (See Glossary) position. The caret will always be at the end of the last generated code in readiness for any more additions. Do not move the caret unless you actually want to insert generated code somewhere else in the program. This is perfectly acceptable once you are familiar with the editor but for now the Quick Start Guide does not require this. You now (should) have a valid program. As long as the tool path syntax was included, you should also see a graphic appear over the stock indicating the final shape after machining. You can use the mouse wheel and slide bars to zoom in and out and scroll bars to pan around the view. Select the Simulate menu item. The program will simulate the program you have just produced. It will show how the stock removal canned cycle works. You can stop simulation via the esc key or the RH mouse button. Click on Download and select the Download and Run drop down item. The code will download to the machine after which it will home its axes, prompt for a tool change (if tool changing is manual) and run the program in the same way as the simulation did. Unless your machine is very small, the default G50 figures placed in the code should ensure that the program is executed well away from the chuck. To machine a part the G50 figures will need to be correctly set and changed in the program code. ED1005 9:13:23 pm 26/06/2014 V11 Page 5

6 G codes The Digi9 controller is designed to execute valid G code*. Many of the G codes are firmly established in industry and all work the same way on different controllers. Such primitive codes would be G0 G1 G2 G3 G91 G92 M2 S M3 M4 M5 to name a few. Many commercial controllers have additional features that produce a particular series of movements in what is called a canned cycle. A canned cycle is also a G code and can make many movements but only require only a few (or even just 1) lines of code. Stock removal, threading or peck drilling are just a few examples of canned cycles. These canned cycles could (in some instances) be emulated with a multitude of primitive G0 and G1 commands but the program would be long and hard to maintain. The point here is that the syntax for canned cycles generally tend to be different between manufacturers but the established primitive G codes* work the same way. Since the established codes generally work the same way on all machines, third party software companies produce code wizards, which produce complex programs utilising only the established primitive codes. It is not unusual to see large programs automatically generated from a solid model CAD/CAM program. Since the process is automatic there is nothing wrong with it other than the generated code generally tends to be large. In fact the D9Mac application has the ability to explode its canned cycles into primitive codes in much the same way. Applied Numeric Control s Digi9 controller and PC software (D9MAC) come somewhere in between hand coding line by line and a fully featured code generator, by providing a means by which either the features of its code wizard are utilised or G codes from another source can also used. If you know G code dive right in and write your own. If you generate it externally it can be imported into the editor simulated and downloaded. *By G codes we also mean other misc codes such as M codes ED1005 9:13:23 pm 26/06/2014 V11 Page 6

7 G00 programmed rapid movement Example G00 X0.0 Z0.0 G codes Optional syntax if only one axis needs to move G00 X10.0 G00 Z23.0 A rapid movement moves the machines axis at a rapid feed rate. This movement is designed to get the tool to the required position as soon as possible. Note All X axis movements represent the diameter of the tool position and as such moves only half the distance of the value in the command G01 programmed movement at feed rate defined by F command Example G01 X0.0 Z0.0 Optional syntax if only one axis needs to move G01 X10.0 G01 Z23.0 If a G01 command has been previously issued, a G01 modal state is current and then allows the following syntax. This makes coding quicker. Eg G01 X0.0 Z0.0 this will enter the modal state for programmed movements X42.3 allowing this style of input Z 34.3 X 12.5 Z34.2 Any command other than these or a G01 will cancel the modal state and an error will be posted when run or simulated as per the following example. Eg G00 X0 Z0 modal state cancelled X42.3 this will cause an error message to be posted when simulated or run ED1005 9:13:23 pm 26/06/2014 V11 Page 7

8 G02 and G03 These commands are arc movements. G codes Example of a clockwise circular movement G02 X20.0 Z-10.0 I0.0 K-10.0 Example of a counter clockwise circular movement G03 X20.0 Z-10.0 I0.0 K-10.0 These commands will move in a circular arc from the current position to the position defined by the X and Z values. The arcs origin is the relative positions defined by the addition of the I and K values to the X and Z current positions respectively. An error will be posted if the final point defined by the X and Z values of this command do not lie on the arc. The movement is at the current feed rate. Please refer to drawing below G90 Absolute and G91 relative mode These commands change the way the positions of the subsequent G01 and G00 s are applied to the movement. If G90 is current, the movements are absolute. A movement G01 X1.0 for example will move the X axis to a diameter of 1.0. If G91 is current, relative movements are applied. A movement G01 X1.0 for example will move the X axis 1.0mm in the positive diameter direction by 1.0mm. When a program starts, its default setting is G90 (absolute) even if it is not entered in the program. ED1005 9:13:23 pm 26/06/2014 V11 Page 8

9 G codes G90 Absolute and G91 relative mode continued. Example - these 2 code snippets do the same thing. G90 G00 X20 Z0 G01 X0 G01 X20 G01 Z-10 G01 Z0 G00 X20 Z0 G91 G01 X-20 G01 X20 G01 Z-10 G01 Z10 This feature is useful for making a series of movements without having to calculate their absolute positions. You may want to make some small movements in and around a feature within your job just to clean it out. Say a boring bar was at the end of a bored hole and the diameter at this point needs to be made larger to account for the tool nose radius. Code as follows (Last movement of 20mm diameter bore 30 deep using a boring bar G01 X20 Z-30 (then to clean up using relative movements G91 G01 X0.3 G01 Z0.3 G01 X-0.3 G90 (don t forget to go back to absolute G91 is also a versatile setting when designing custom written canned cycles in function calls. See explanations of G57 function calls and function calls within the sample programs section. ED1005 9:13:23 pm 26/06/2014 V11 Page 9

10 G codes G50 Machine reference settings and offset adjustment. Example T1 G50 X100.0 Z100.0 The Code generator will optionally generate a table of these settings when program initialisation is executed. These settings represent the distance each axis must move for a given tool, to reach the reference point of the job. Please refer to the glossary for an explanation of the reference and how to set them in setting up for a program. If this table of codes are not present in the program the controller will remember the settings from the last program that was run that did contain them. If your tooling system is consistent in position every time a new tool is installed and you are disciplined in tool management, the G50 settings could be set once and forgotten. This would apply to automatic tool changers or quick change manual tooling systems. Smaller machine tools with manual square tool posts generally require this setting be changed every time a new tool is installed due to the inconsistency of the position of the installation. The D9MAC software only generates default values of offsets. These values (if used) will need to be changed to the correct values before running the program. Please refer to Fig 2 for a diagram of offsets. ED1005 9:13:23 pm 26/06/2014 V11 Page 10

11 G76 Threading Example G76 X24.00 Z D0.02 P1.0 G codes The G76 commands the controller to start a series of synchronised movements from the current position to the final positions denoted by the X and Z values of this command. Each pass moves the X axis by the amount denoted by the D parameter until the final diameter is reached after which a final spring pass will execute. The Z axis feed rate Is calculated from the current spindle speed to result in the desired pitch denoted by the P parameter. Threading can be internal, external right or left handed depending on the relationship of the current position and finishing position parameters of this command. Example for internal threading. Move to a diameter which is less than the maximum diameter of the thread. G00 X20.0 Z3.0 (Thread to a larger diameter G76 X21.0 Z-10.0 D0.02 P1.0 Note. At the end of the canned cycle the tool returns to the position that it was at when the canned cycle started. The operator must ensure that additional clearance movements are added if necessary, at the end of this command to clear the billet when proceeding with further operations particularly if an internal thread was cut. Simulation checking always helps here. Also (and obviously) feed rate and spindle overrides do not operate during this cycle. ED1005 9:13:23 pm 26/06/2014 V11 Page 11

12 G83 Peck drilling Example G00 X0.0 Z1.00 G83 Z D1.00 F50.00 G codes The G83 commands the controller to peck drill to the depth denoted by the Z parameter. Each plunge depth into new material is the distance denoted by the D parameter. The feed rate is denoted by the F parameter. The tool will retract at the rapid feed rate to the starting Z position then return to the previous depth to commence a new cut thereby clearing swarf from the flutes of the drill. Please note that a previous movement to the starting position is required (particularly on the X axis to the centre of the billet). This command can also be used with other tooling. For example a boring bar as an alternative way to manage stringy swarf in internal boring. In such a case the x axis would not be 0.0 G96 Stock removal. Example shown here with code to produce a simple profile. G00 X25.00 Z3.00 G96 X0.00 Z D0.50 L6 G00 X0.00 Z3.00 G01 X0.00 Z0.00 G01 X12.00 Z-1.00 G01 X12.00 Z G01 X22.00 Z G01 X25.00 Z The G96 command starts a series of movements to remove the bulk of the material surrounding the desired profile. The command in this example will successively take cuts with the Z axis from the current position to the final position denoted by the X and Z parameters in this command. In each pass the X axis will advance by the amount denoted by the D parameter. Before moving the Z axis in each pass, the controller will look ahead in the code by the number of lines denoted by the L parameter. If the intended movement intersects any of the lines or arcs between points of the encompassed G code, the Z movements end position is changed to this intersection, thereby stock removing to the profile. A safe way to see stock removal and experiment with its parameters is to use the simulation. ED1005 9:13:23 pm 26/06/2014 V11 Page 12

13 G96 Stock removal continued G codes The operator must ensure that additional clearance movements may be necessary at the end of this command to clear the billet when proceeding with further operations particularly in internal stock removal. Simulation checking always helps here. (STOCK REMOVAL G00 X30.00 Z2.00 G96 X0.00 Z25.00 D1.60 L6 G00 X0.00 Z4.06! G01 X0.00 Z01.00~ G01 X14.40 Z-0.02~ G01 X14.40 Z-16.34~ G01 X26.40 Z-21.44~ G01 X30.00 Z-21.44~ (INTERNAL STOCK REMOVAL G00 X6.00 Z4.19 G96 X19.23 Z D0.60 L6 G00 X12.00 Z-21.44! G01 X12.00 Z-21.44~ G01 X14.40 Z-16.34~ G01 X14.40 Z-0.02~ G01 X26.40 Z1.00~ G01 X36.00 Z1.00~ (AWAY FROM CHUCK STOCK REMOVAL G00 X25.00 Z G96 X8.00 Z-6.00 D0.50 L6 G00 X8.00 Z-22.00! G01 X10.00 Z-20.00~ G01 X10.00 Z-10.00~ G01 X12.00 Z-8.00~ G01 X23.00 Z-8.00~ G01 X25.00 Z-6.00~ ED1005 9:13:23 pm 26/06/2014 V11 Page 13

14 G96 Stock Removal continued G codes Stock removal only works when the cutting travels from smaller to larger diameters. The final cut will however follow the profile and you must be take care not to cause any damage if using this canned cycle. It is up to you to ensure the depth of the final cut is acceptable. Using Stock Removal can be quite useful to machine the undercut for threads, particularly when smaller threads and softer materials mean that the loading for the final cut is acceptable. Hatched areas shown below indicate material that will be removed during the final cut of stock removal. ED1005 9:13:23 pm 26/06/2014 V11 Page 14

15 G59, G57 G58 program function calls G codes A function is a group of program lines. These lines can be any valid codes you would see in a normal program. In a function, the start of this group of code is marked by G57, and the end of the group is marked by G58. A function is called as many times as desired. Calling a function eliminates the need to write many repeated movements. It is a versatile feature allowing many creative techniques to be employed in programming style. Some examples- 1 Creating your own custom canned cycle. 2 Rapid program entry in production machining by negating the need for the machine to initialise itself at the start of the program. 3 Dividing a large program into functions allows a convenient form of a mid run start. This makes set ups easier, and in reworking, previously machined sections of code can be jumped over to save time. 4 A program may produce a similar parts with or without a particular feature. Using functions allows the operator to call the relevant function only for that version of the part, all in the same program. ED1005 9:13:23 pm 26/06/2014 V11 Page 15

16 G codes G59, G57 G58 program function calls continued. Example program that cuts a simple chamfer and a shoulder. G00 X25 Z0 Move to the start position where we want to do some work. G59 R1 C20 call the function R1 20 times (continue on with other commands (G57 marks the start of the function, the R1 is the routine number and identifies the (function. G57 R1 G91 G01X-0.5 G01 X5 Z-10 G01 Z-5 G01 X1 G00 Z15 G01 X-6 G90 G58 (The G58 marks the end of the function Functions are extremely versatile in larger programs and at this point we would recommend use of a programming style which makes the readability of the code easier. To do this you would consider your program to have a structure whereby the main body of your code be considered as the master of all of the operations. In this main body, there is a minimum of anything other than function calls. At the bottom of the main section come the functions. Liberal line spacing of the functions from each other and from the main section makes the program look more readable. In addition to this, the use of comments explaining what each function does also helps. ED1005 9:13:23 pm 26/06/2014 V11 Page 16

17 G Codes G59, G57 G58 program function calls continued. Example of a large program architecture. (Main program. Some codes possibly to move to an appropriate location G59 R1 C 1 A function call with a comment indicating what the function does. G59 R2 C2 Another function call with a comment indicating what the function does. Etc Etc Optional other coding Program termination Some clear lines G57 R1 Start Function 1 with an identifying comment Some lines of code G58 End of function Some clear lines G57 R2 Start Function 2 with an identifying comment Some lines of code G58 End of function Etc Etc ED1005 9:13:23 pm 26/06/2014 V11 Page 17

18 G Codes G59, G57 G58 program function calls continued. As mentioned earlier, a whole section of code can be called or ignored by using a simple comment character (. For example our program calls R1 R2 and R3 to make a part. R2 is an optional feature. So the following calls make the product G57 R1 C1 G57 R2 C1 G57 R3 C1 then G57 R1 C1 (G57 R2 C1 G57 R3 C1 Produces the part but without the features of R2 Please refer to the samples section to see an example of function calls G52 Move to absolute machine location. Example. G52 X0.0 Z0.0 G01 and G00 s move the tool to a position relative to the origin of the billet by using the G50 setting. By comparison a G52 moves the tool to a position relative to the home position of the machine. No offset G50 s are involved For example G52 X-10 Z-10 will move the tool 10mm on each axis just to the left and in from the home position. You often see G52 X0.0 Z0.0 in the termination section of generated code which sends the axis to the home position. ED1005 9:13:23 pm 26/06/2014 V11 Page 18

19 G4 Timed Pause. Example G4 1.5 G codes This command will delay execution of the program for 1.5 seconds. This is useful when drilling or grooving to ensure the spindle has turned enough times at the end of the final depth of cut to ensure a clean finish. G94 G G94 sets the feed rate to units per minute G95 sets the feed rate to units per revolution of the spindle G72 Grooving. Example: G00 X25.00 Z-8.00 G72 X16.00 Z I2.50 K2.00 These commands instruct the controller to move the tool to a diameter of 25.0mm, Z-8.0mm and begin a grooving cycle. A groove will be produced via pecking movements of 2.5 mm deep, denoted by the I parameter. After each peck, the Z axis moves 2.0 mm, denoted by the K parameter and then proceeds with another peck. These sequences repeat until the tool is at the finishing position denoted by the X and Z parameters. The groove starts at Z-8.0 and finishes at Z The command makes no assumption about the tool width and as such the resulting groove will be 8.0mm plus the tool width of 2.0mm. See drawing below. If finning occurs between pecks, reduce K to less than the width of the grooving tool. ED1005 9:13:23 pm 26/06/2014 V11 Page 19

20 ( Comment delimiter.. Other codes If you look at a long G code program it would be daunting to see exactly what is going on. A comment allows the programmer to write within the code, comments identify individual sections of the code. A comment can be added to G code with the addition of the left hand parenthesis i.e. ( before any text. Example (DIAMETER TO BEARING FIT The text can be anything at all, but the parenthesis must be the first character on the line. Another less known use for a comment is to prevent the controller from executing code. Eg (G83 X0 Z-10 D0.5 will prevent the controller from executing the drilling cycle. This is a time saving procedure when re running a program over a pre machined part M00 program pause. Example snippet will move the axis away, stop the spindle halt the machine and wait for a keyboard input before continuing. G52 X0.0 Z0.0 M5 (Clear swarf M00 M3 (more code M2 Program end An M2 indicates to the controller the program has ended. This code does not necessarily have to be at the end of a program. It could be inserted in code well before the end while checking and debugging a new program. ED1005 9:13:23 pm 26/06/2014 V11 Page 20

21 Other Codes S800 Set spindle speed to 800 RPM This command does not start the spindle M3 Start spindle forward rotation at the current spindle speed. A speed setting must have been previously set M4 Start spindle reverse rotation at the current spindle speed. A speed setting must have been previously set M5 Stop the spindle Alternative syntax which sets the speed and starts the spindle in one line S500 M M8 Turn on coolant if fitted. M9 Turn off coolant T1 M6 Tool change. The M6 command changes the tool in an automatic tool changer to the tool number defined by the T parameter. In manual tool changers, the program halts and prompts for the user to insert the tool. ED1005 9:13:23 pm 26/06/2014 V11 Page 21

22 Controller Setting up for machining and the manual/offsets page. In order to run a program the machine has to be set up. Setting up requires that all of the intended tools are ready either in the automatic tool changer or on hand ready to be fitted into the quick change tool post when prompted. It also requires that the intended billet be fitted in the chuck and the distance from the home position to the reference of the billet for each tool be known. This requires the operator understands the importance of the reference, how his program works and most importantly whether a new program is compatible with a particular set-up. It may sound complicated but in reality it is just common sense. Please refer to the section and drawings outlining reference points on page 11. These settings can be derived and in some cases depending on your programming style, need only be entered into the controller once. The Digi9 controller provides 2 methods for setting offsets and your preference is the deciding factor here. Method 1 via the Tool offsets table These distances, once established, are entered into the G50 values in the tool offset table generated by the code generator. Method 2 via touching the stock with the tool. If this method is used, the optional tool offsets table must be omitted from the program. Remember the controller retains these setting in memory and the memory is updated any time a G50 setting present in a program. The software will prompt any G50 settings in the code giving the option to overwrite or not overwrite. ED1005 9:13:23 pm 26/06/2014 V11 Page 22

23 Controller Setting up for machining and the manual/offsets page continued The manual/offsets pages provide all of the facilities for setting up the tooling. Pressing the Manual page button on the controller enters the manual page. In the manual page, the spindle can be started and stopped, The spindle speed can be entered, the axes can be homed or moved via the 2 Manual pulse generators and the operator can see the actual position of both axes via the display. While in the manual page, successive pressing of the Manual Page button will toggle the page from a manual page to an offsets page and back again. The difference between these pages is subtle. The manual page is designed to allow the operator to operate the machine as a manual machine via the MPG s. The ZERO X and ZERO Z button will zero the positional displays of the axis allowing the operator to utilise the digital readout in manual operations. The offsets page is also designed to allow the operator to operate the machine as a manual machine via the MPG s. The ZERO X and ZERO Z buttons however is different and will initiate a conversation to set the offsets. To set offsets the first thing the operator should do is ensure he is in the offsets page and home the machine by pressing the HOME button on the controller keypad. This will send the axis home and zero out the position indicators on the display. After homing the axis can be moved via the manual pulse generators. Note that before the machine is homed, the positional displays are terminated with a?. This means that the values are questionable and should not be used. The? disappears after the machine has been homed. ED1005 9:13:23 pm 26/06/2014 V11 Page 23

24 Controller Setting up for machining and the manual/offsets page continued. At this point we need to get 2 numbers for each tool used. 1 for the X axis and 1 for the Z axis. These numbers are the distance each axis must move in order to reach the reference. To do this we will assume the reference is at the end of the stock for the Z axis and is always the centre of the stock for the X axis. Move both axes towards the billet via the MPG s. If using method 1 by entries into the tool table in the G code file. This is recommended for beginners. The range switch can be selected at its highest setting to speed up this operation then slowed down during the finer operations. Once close to the billet, start the spindle and take a light diameter cut. Move the Z axis back away from the stock but don t move the X axis. Stop the spindle and tabulate the reading for the X axis from the display. Using digital verniers, measure the diameter of the cut just taken. Add the diameter to the reading and tabulate this result. This value is the distance from the home position to the centre of the stock. The Z axis is a little easier. Using a similar technique, start the spindle and take a light facing cut. Stop the spindle and tabulate the reading in the display for the Z axis. (no other measurements for the Z axis are required) This assumes your Z reference is at the end of the stock. If you require the reference to the face of the chuck, simply add the length of the billets face from the face of the chuck to this reading. Note both readings in the display are negative but you only need to enter/add them as a positive number. ED1005 9:13:23 pm 26/06/2014 V11 Page 24

25 Controller Setting up for machining and the manual/offsets page continued. If you are disciplined with your tooling and set-ups, these values need not change for any given tool. Please note however that other tools will have different shapes, so their offsets will be different. As long as your method of location of the tooling is consistent, these procedures need only be done once. The reference for the Z axis does not have to be the end of the stock. In many cases operators prefer the face of the chuck since it is consistent and independent of the billet length. The choice is yours. The values just recorded are then entered into the offsets tool table thus- T1 G50 X Z T2 G50 X Z T3 G50 X92.82 Z T4 G50 X68.42 Z Etc The code wizard generates a table for the first 3 tools. You can add more lines if your program required more tools as per this example with 4 tools. If these values have been run in a program once, they need not be included in another program that requires the same offsets. If your doubtful, you can always include them. Please note however if you do include them, as programs get older and over time adjustments are made due to tool wear or tool replacement, the settings can become old. ED1005 9:13:23 pm 26/06/2014 V11 Page 25

26 Controller Setting up for machining and the manual/offsets page continued. If using method 2 by touching the tool on the stock. While in the Offsets page, Home the axes. In a similar manner to the previous description the axes can be moved to the billet. Take a light diameter cut, stop the spindle and measure this diameter. At this point the ZERO X button can be pressed. The controller will prompt to input the tool number and then for the diameter you have just measured Take a facing cut. Stop the spindle and press the ZERO Z button. The controller will prompt for the tool number and then for an offset length. If your reference is at the end of the stock the value will be zero. If you are making the face of the chuck your reference you will need to enter the length of your stock. Entering these values will then set the offsets for the x and z axis for the selected tool within the controllers memory. This method is easier than the previous method as the operator does not have to tabulate, add values and enter numbers into the tool table. Remember if you have entered values by whatever method, the controller will remember the settings. If you load and run a program with offsets in the G code The values will be overwritten. If you have inadvertently generated offsets and don t want them you can just delete those lines of code from within the G code editor. When downloading, the software will warn that G50 s are present in your program (if they are actually present) and give you the final chance to decide weather or not you want these values to overwrite the offsets. In the real world, the static procedures associated with an offset set-up versus the dynamics of machining, an operator will find the finished dimensions different to what he would expect. This is due to billet flex, overheating incorrect tool height, tool loading, lubrication, backlash and gib wear etc. The beauty of a CNC machine is that these distortions can be managed. Once a part has been machined it can be measured to ascertain these errors. ED1005 9:13:23 pm 26/06/2014 V11 Page 26

27 Controller Setting up for machining and the manual page continued. The controller provides methods to optimise the offsets without having to repeat the offsets procedures. For example, if the part has come out oversize on its diameter by 0.2mm. When the controller is displaying its opening page (the page displaying Applied Numeric Control ) Pressing the ZERO X button will enter a conversation to modify the X offset. In the case above, pressing ZERO X will then make the controller prompt the operator to enter the tool number, then the amount by which the offset should be changed, in this case The value the operator enters is added to the internal value and then saved thereby correcting the program. If the part was smaller by 0.2mm the operator would enter 0.2. Negative numbers make the diameter smaller. A similar procedure is used for the Z axis. Note however that this only applies if you are letting the controller remember the settings and do not have the offsets in the program. At the end of the day an operator may need to know what offsets values are actually stored in the controller. When the controller is displaying its opening page (the Applied Numeric Control page) pressing the number 8 key will enter a conversation that will prompt for a tool number. Entering this will then display the actual stored offset values for both axis. It is a good method of checking that the offsets have not been inadvertently changed. The tool height must be correct in any of these installations. See the section of the effect of tool height on machining diameters in the Glossary. Correct tool height can be established my taking a facing cut on a spare billet. There will be a pip of material left on the face if the tool is too low, and if the tool is too high, it will be witnessed during this operation when the tool gets near the centre. See below. ED1005 9:13:23 pm 26/06/2014 V11 Page 27

28 Program Development The D9mac applications primary purpose is to download programs to the controller. It includes a text editor that allows you to write and edit code and a graphical simulator to test the validity of your programs. Programs can come from different sources, either archival, generated from a third party application or hand written. The application has a wizard to generate code for drilling, threading grooving, stock removal etc. The application also has a wizard that produces a default framework based on a selected stock size. This framework can be either internal machining, machining away from the chuck, external machining or a combination of any or all of the above. Generally speaking most machining requires stock removal to machine down to a desired shape or profile. Once the shape is formed final operations like threading, grooving drilling and/or parting off can be coded manually. The focus here is the initial profile. If you click on stock removal in the code wizard you end up with this profile. The code here represents several movements which form a shape. It is headed by the stock removal command. This shape is unlikely to be in accordance with your needs but given that all the code to stock remove to this profile is now present, all that is required is to modify the G codes that follow the stock removal command to your requirements. If you change the values or add or delete lines, the graphic will change in accordance with these modifications. We stress here that these movements only describe the overall shape of your finished product, do not try to get the graphic to show a groove or a drill hole as these are not part of the stock removal canned cycle. ED1005 9:13:23 pm 26/06/2014 V11 Page 28

29 Program Development continued You can have as many stock removal frameworks as you need and they generally fall into 1 of 3 categories. 1 External. Meaning that stock removal (using a right handed tool) works from the end of the billet towards the chuck with the minimum diameter to the right and the maximum diameter to the left. 2 Internal. Meaning that the process (using a boring bar) works from the inside of the billet with the widest diameter to the right and the narrowest diameter to the left. 3 Away from chuck. Typically using a left hand or grooving tool, machines away from the chuck with the narrowest diameter being on the left and the widest diameter on the right. Stock removal only works when the cutting travels from smaller to larger diameters. The final cut will however follow the profile and you must be take care not to cause any damage if using this canned cycle. It is up to you to ensure the depth of the final cut is acceptable. A profile that tapers away as shown below, cannot be completed by stock removal alone. The stock removal code wizard generates code that ends with the ~ character. This character is not part of the G code as such. Its purpose is to instruct the application to draw a line or an arc. A profile is a collection of entities (lines or arcs) joined together. Drawing lines or arcs between points denoted by G codes results in the desired profile being displayed. The! character is also part of the display syntax. The following code demonstrates how the graphics generator works. G00 X10 Z0! G01 X20 Z0~ G01 X30 Z-10~ The first line with the! character at the end of the line instructs the application to move the START of the graphics display to this point. The ~ character tells the application to draw a line from the last point (in this case the point denoted by the! character) to the current point. ED1005 9:13:23 pm 26/06/2014 V11 Page 29

30 Program Development continued If you want do draw another profile somewhere else you just need another! at the beginning of the new profile. EG- G00 X10 Z0! Start of first profile G01 X20 Z0~ draw a line to this point G01 X30 Z-10~ draw a line to this point G00 X10 Z-50! Start of second profile G01 X20 Z-20~ draw a line to this point G01 X22 Z-10~ draw a line to this point Drawing your desired profile helps in verifying that what you intend on doing looks correct. It is not the only purpose. It can be used alternatively to simulation to confirm that a tool will actually clear a particular part of the job. The! and ~ characters do not effect the G codes and are only used to generate a graphic of the desired profile. The! and ~ characters are not specific to the stock removal canned cycle. They can be left out all together if desired. The D9mac application generates code in accordance with the operators selection from the rich set of menu items. In most cases it also generates a description of what the generated code does. Experiments with these items is the best way to get to know them. The generated code defaults to suitable values based on the stock size and the option to modify these values before generation is given. Even if the code has been generated and needs to be changed, it can be modified as per the users requirements within the editor. If stock removal code is generated, and the options included the graphics directives, or even if code is hand written and contains the graphics directives, moving the mouse close to any of the vertices on any of the profiles will generate a highlight. The highlight is a little square. The line of G code is also highlighted. This makes program editing easier. This last highlighted vertex is remembered by the software and is ready if either a chamfer or a radius is selected from the code wizard menu. Clicking on either of these will modify the G code and will insert either extra G01 or G02/3 to produce either a chamfer or radius. The radius or chamfer length is collected from the value entered in the floating status window. Please note that this feature adds an extra line to the code. If you are stock removing, you will need to increase the L parameter of the stock removal command to encompass this additional line. ED1005 9:13:23 pm 26/06/2014 V11 Page 30

31 Program Development continued DXF input. Another method of code generation is by selecting the vertices of a graphic generated by a DXF input. The D9mac application provides methods for inputting of a DXF file. Once loaded, the graphic of the DXF will show in the display. Note that the colour of this display is different to the graphic generated by the graphics directives discussed earlier. Moving the curser near the vertices of the DXF graphic will generate a highlight square. Left clicking, while the curser is still near the highlighted point, will generate code of that point in the G code window at the caret position. The file always contains the DXF information and is saved with the G code. Please note that the chamfer and radius commands are only able to modify G code graphics directives and NOT dxf profiles. The word here is that the DXF file must be as you require it when you download it. The application provides a CLEAR DXF function which allows re loading of different DXF files. DXF format has evolved over the years and as CAD has graduated to solid modelling, DXF files have grown with them. A lathe is predominantly a 2 dimensional machine and as such the DXF file must contain only 2 dimensional lines and arcs. There is nothing else in the data that is of any use to the application. There are processes within most modern CAD packages to strip complex data, thereby reducing the required profile to 2 dimensions. Alternatively a simple CAD package like Autosketch produce ideal DXF files. Once a drawing has been made, the point of the drawing that is required to be the reference is moved to the zero reference of the CAD sheet and then saved as a DXF file. The point here is that the cad package is used to produce the drawing then imported. Modification of the drawing generated by DXF input in D9mac is beyond the scope of the application. Finally G code can be imported from existing.txt files using the import text file menu item. ED1005 9:13:23 pm 26/06/2014 V11 Page 31

32 Axis directions. Glossary Generally speaking for the external machining of a billet, any movement that makes the billet smaller is a negative direction. So if we go from X20.0 to X15.0 we have gone in a negative direction. Similarly if we move from Z0.0 to Z-10 we have gone in a negative direction. Both of these movements would have reduced the size of the billet. This is a most notable point particularly when the X axis of some machines actually approaches the billet from the far side. Billet/stock/tool reference. The point on the billet from which the distances for each axis is referred. If you look at a technical drawing of the part you intend on manufacturing there should be a reference point to which all of the features of the part are referenced in the dimensioning. Some drawings don t assume any particular sort of machining and may have obscure dimensioning possibly from both ends of the stock. In this case the person responsible for producing the CNC code will have to translate all of the features of the drawing to one reference point on the billet. Another instance is if a cad drawing is used to generate code, it too will have a reference point. ED1005 9:13:23 pm 26/06/2014 V11 Page 32

33 Glossary continued The controller assumes the reference is generally always in the centre of the stock for the X axis but can be at either end or anywhere in between for the Z axis. Operator preference prevails here there, is no right or wrong way to do it. It is important however that the operator understands what references are and that the cnc code he generates is appropriate for this reference. The tool also has a reference. It is the point on a tool that moves to the locations referred tool by the G code. This may be obvious for typical turning tools or drills etc. It is worth noting however the reference of a grooving tool is a little more ambiguous. The grooving tool typically has its reference at the outside corner of the tool tip. The point here is that if you wanted to produce a groove at the tool width that is 2.0 mm in on the Z axis you would have to move the tool 2.0 mm plus the tool width to achieve this position. The D9mac software defines a left and a right hand grooving tool. It does this as some operations near the chuck are best served by a left hand tool. In both cases the reference is at the outside corner of the tool tip. The operator has the choice however to set the reference of the grooving tool the wherever he wants when he sets up the machine. If he chooses the inside corner of the tip rather than the outside corner (and there is nothing wrong with this) the movements he makes will appear incorrect in the simulation since the tool reference point of the graphic cannot be changed. Homing. A controller must home its axes in order to reset its internal position counters to zero. This then becomes the absolute machine position. Once this has been done the controller is ready to add the G50 values to these counters in order to make tangible relative movements to the reference. The controller supplied by Applied Numeric Control will home the machine in one of two ways. If the machine has not been homed since it was first turned on or if an error or Emergency Stop condition existed at some time, it will perform a micro switch home. This involves slowly moving the axes to their home positions until a homing limit switch is hit. It then moves back from this switch and a little further until a special precision position signal is reached. At this point the counters within the controller are all reset. During all subsequent operations, calls to home the machine in the manual page or during the running of programs will result in a much faster homing because the controller knows where the home position is. ED1005 9:13:23 pm 26/06/2014 V11 Page 33

34 MPG. Glossary continued This stands for Manual Pulse Generator. These are the hand wheels on the machine that are used in a similar fashion to the hand wheels on a normal lathe. They produce electrical signals used by the controller to move the axes in the manual page or to provide feed rate and spindle overrides in a running program. Profile. A profile is the shape represented by the connection of a number of lines and arcs. Relative and Absolute movements. An absolute movement is a movement to an exact location. A relative movement is a movement that is relative to the machines current position. Eg if the x axis is at 10.00mm and a relative movement of 1 mm is made the axis will move in the positive direction by 1mm to 11.0mm. If this movement was an absolute movement it would move in the negative direction by 9.00mm from 10.0 to 1.0mm. Caret. A caret is a marker within the editor that indicates where the next character that is typed will appear. It is not the mouse curser (which moves as you move the mouse) The caret s position can be changed by moving the mouse cursor to the desired location and left clicking. The code generator will insert code at the carets position. ED1005 9:13:23 pm 26/06/2014 V11 Page 34

35 ERROR messages Error messages are posted in simulation of the D9MAC software and within the controller. These messages are context sensitive for example the simulation makes no assumption as to the size of the machine that will run the code so it will ignore soft limits. The controller however will monitor these conditions. Simulation is always advisable to check programs before downloading. Index pulse out of range. The Applied Numeric Controller has the ability to home its axis on a precision position located at a singular angular location of the lead screw. Every time the machine is homed for the first time every day, this position must remain the same on a day to day basis in order to ensure parts are machined to the correct size. This is an important warning because it lets the operator know if a problem exists. The warning is posted if the controller had to move too far or not far enough (hence the out of range ) from the limit switch to this angular position of the lead screw. This error will most likely occur if an axis crashed or some severe mechanical shock occurred that physically disrupted and end stop, motor coupling or limit switch. It can also occur if swarf got trapped between the limit switch and its striker plate causing a premature actuation of the switch. What to do If the problem is swarf, simply clean it out. Soft limit reached. The DIGI9 controller has soft limits set at pre delivery. It is designed to minimise movements to dangerous positions either beyond the physical limit of the machine or unwanted movements of the tool post too closely to the chuck. A soft limit is a value saved to memory. If an programmed movement tries to move an axis further that the soft limit, this warning will be posted. A movement in the manual page via the MPG s will stop at the soft limit. Warning, a soft limit will not work in the manual page if the axes have not been homed. In such a case it is possible for an operator to move an axis to the end of its physical limit. While the controller will flag an error if this happens because the motor was stalled, it is not advisable as such strains detract from the accurate offset settings. ED1005 9:13:23 pm 26/06/2014 V11 Page 35

36 ERROR messages Start End radius does not match. When an arc move is produced, the start of the arc begins at the end of the last movement. The centre of the arc is a relative position defined by the I and K parameters of the arc command (added to the current positions). The final parameters defined by X and Z of the arc command are the end point where the arc finishes. If the point defined by where the arc finishes does not actually lie on the arc this message will be posted. The D9MAC software generates accurate arcs but in some instances operators can eyeball locations on an arc from within the graphic to derive an arc end point. This method is not 100% accurate but the controller will accept a small error. ED1005 9:13:23 pm 26/06/2014 V11 Page 36