How the heck does G28 work

How the heck does G28 work?

G28, Fanuc's zero return command, tends to be one of the more misunderstood Fanuc programming words. The zero return position is, of course, the machine's reference position. A light (axis origin light) will come on for each axis that is sent to the zero return position. The zero return position is quite important: most programs begin from this location, most machines require that you (manually) send the machine to this position as part of powering up, and it's a point of reference for fixture offset (machining centers) and geometry offset (turning centers) entries. Admittedly, G28 is among the most complicated programming words. Here we attempt to clear up the confusion.

G28 is a two-step command. In a way, it's like a canned cycle. Two things will happen whenever a G28 is commanded. First the machine will move (at rapid) the axis or axes included in the G28 command to an intermediate position. Then the machine will rapid the axis or axes to the zero return position. At this point the related axis origin light/s will come on. By the way, if you have the single block switch on, you actually have to press the cycle start button twice to complete the G28 command - once for the intermediate position move, and a second time for the move to the zero return position.

The intermediate position is what confuses most people. In absolute mode, which most programmers prefer for general purpose programming, the intermediate position is specified relative to program zero. In incremental mode, it is specified relative to the tool's current position. Maybe the best way to gain an understanding is to give a few examples.
For machining centers:

Consider this command.

* G91 G28 Z0

In step one of G28, the tool will move to an intermediate position that is incrementally nothing (zero) from its current position in Z. In step two, it will go to the zero return position in Z (only). Note that X and Y will not move. For all intents and purposes, we're telling the machine to move the tool straight to its zero return position in Z.

* G91 G28 X0 Y0 Z0

In step one of G28, the tool will move to an intermediate position that is incrementally nothing (zero) from its current position in X, Y, and Z. In step two, it will go to the zero return position in X, Y, and Z (together). For all intents and purposes, we're telling the machine to move the tool straight to its zero return position in X, Y, and Z.

* G91 G28 X0 Y0 Z3.0

In step one of G28, the tool will move to an intermediate position that is incrementally nothing (zero) from its current position in X, Y. But in Z, it will move up three inches. Maybe the tool is in a pocket you need to clear before moving in X and Y. In step two, it will go to the zero return position in X, Y, and Z (together).

Watch out! Here's what can happen in absolute mode. Consider this command.

* G28 X0 Y0 Z0

Assuming the machine is currently in absolute mode (G90), step one of G28 tells the machine to move to the program zero point (probably a crash). Then, in step two, the machine will move to the zero return position (if it still can).

Some programmers don't like to program (ever) in incremental mode. While I don't consider using the incremental mode with G28 to be straying too far from absolute programming, there is a way to stay in the absolute mode when using G28. Consider these commands.

* G90 G00 X1.0 Y1.0 (Rapid to hole position)
* G01 Z-0.5 F5.0 (Drill hole)
* G00 Z0.1 (Rapid out of hole)
* G28 Z0.1 (First, stay right where you are in Z, then go to the zero return position in Z)

While this works, I don't like it. I show it just for the sake of explanation. Essentially, we're looking back in the program to the tools last absolute position so we can include it in the G28 command. Again, this does work, but someday you'll probably change a tool's last position. In this case you better also remember to change the related G28 command or you'll be in for a big surprise!
For turning centers:

Consider this command.

* G28 W0

In step one of G28, the tool will move to an intermediate position that is incrementally nothing (zero) from its current position in Z. In step two, it will go to the zero return position in Z (only). Note that X will not move. For all intents and purposes, we're telling the machine to move the tool straight to its zero return position in Z.

* G28 U0 W0

In step one of G28, the tool will move to an intermediate position that is incrementally nothing (zero) from its current position in X and Z. In step two, it will go to the zero return position in X Z (together). For all intents and purposes, we're telling the machine to move the tool straight to its zero return position in X and Z.

* G28 U3.0 Z0

In step one of G28, the tool will move to an intermediate position that is incrementally nothing (zero) from its current position in Z. But in X, it will increase in diameter by three inches (1.5 inch move). Maybe the tool is below an obstruction (like a tailstock) you need to clear before moving in Z. In step two, it will go to the zero return position in X Z (together).

Watch out! Here's what can happen in absolute mode. Consider this command.

* G28 X0 Z0

Note that now we're commanding G28 in absolute mode. Step one of G28 tells the machine to move to the program zero point (probably a crash). Then, in step two, the machine will move to the zero return position (if it still can).

Some programmers don't like to program (ever) in incremental mode. While I don't consider using the incremental mode for G28 to be straying too far from absolute programming, there is a way to stay in the absolute mode when using G28. Consider these commands.

* G00 X3.2 Z0.005 (Rapid to facing position)
* G01 X-0.06 F0.012 (Face part)
* G00 Z0.1 (Retract in Z)
* X3.2 (Retract in X)
* G28 X3.2 Z0.1 (First, stay right where you are in X and Z, then go to the zero return position in X and Z)

While this works, I don't like it. I show it just for the sake of explanation. Essentially, we're looking back in the program to the tools last absolute position so we can include it in the G28 command. Again, this does work, but someday you'll probably change a tool's last position. In this case you better also remember to change the related G28 command or you'll be in for a big surprise!
What about G53?

Most current model Fanuc and Fanuc-compatible controls allow G53 - movement relative to the zero return position. For machining centers that allow G53, the command

G53 X0 Y0 Z0

will send the machine (at rapid) straight to the zero return position in X, Y, and Z. Unfortunately, older controls do not allow G53. Since G28 works on all Fanuc and Fanuc-compatible controls, most programmers prefer to use the (complicated) G28 command so they can run their programs on all machines their company owns.

courtesy : http://www.cncci.com/resources/tips/how%20g28%20works.htm

HOW TO CONFIRM MACRO B IS ENABLED ON YOUR CNC

How to check cnc control has Macro B.

In general machine controllers like Haas, Mistubishi, Mazak,supports for macro.


But for most controls, Custom Macro B is an option. It doesn't come standard with the control. However, many machine tool builders include Custom Macro B in the standard package of options they include with the machines they sell, especially if the machine has some special accessory like a probing system.

So how do you tell if a given control has Custom Macro B? One universal way is to perform a simple test in the MDI mode. In the manual data input (MDI) mode, simply enter and execute the command

#101=1

Remember that most Fanuc controls require that you terminate MDI commands with a semicolon (;). If the control has Custom Macro B, it will execute this command without generating an alarm. If it does not, an alarm will be sounded (something like "unrecognizable address").

Additionally, if the machine has Custom Macro B, you should be able to find a display screen that shows the Custom Macro variables. With Fanuc controls, it will either be in the OFFSET or SETTING display screen pages

G code help on Fanuc 15

G code help screen on 15 series Fanuc controls

Here is something you can use with Fanuc series 15 controls that is quite helpful. If you cannot remember the format for the various G codes, the 15 series will give you some help. In the EDIT mode, type G and press INPUT (not insert). The display screen will show you a list of all G codes and their proper format and meanings. You can use the left/right double arrow keys to move up and down the list.

If you want the specific format for a given G code, just type the G code (like G84) and press INPUT. The control will show you the correct format for the G code in question.

Cimco DNC MAX

NC Technologies is a leading Computer Integrated Manufacturing solutions provider in India happily announces its business tie-up with leading giant CIMCO Integration, Denmark as a authorized distributor having various range of products for Computer integrated manufacturing solutions.

NC Technologies offers CIMCO Integration, Denmark products to its various customers in India.

Recently, NC Technologies offered CIMCO products to M/s MVM Engineers, Chennai. The Product includes DNC Max5, CIMCO Edit Professional & CNC Calc with the advantage of Wi-Fi Shop floor networking. The entire module is offered with affordable price. Small and Medium Enterprises can easily invests on this products to gain more productivity and Return of Investment

DNC Max 5 : is a latest version of most trusted CNC communication software with Client / server architecture having remote request and auto receive features. DNC Max 5 provides end to end functionality designed to make every aspect of CNC communications more reliable and efficient.

• Client server concept to eliminate dedicated pc on shop floor.
• Supports all type of controllers(Mazak, Siemens, Fanuc, Hass, Heidenhein…)
• Hardware compatibility with wired and wireless technologies
  
• CNC File Compatibility
• Easy of Use and Administration because of Client / Server interface.
• The main advantage of this DNC Max is its extending power to integrate with other modules of CIMCO.

CIMCO Edit 5 Professional: CIMCO Edit 5 is the latest version of the most popular CNC program editor. CIMCO Edit 5 provides a comprehensive set of essential CNC editing tools, including block numbering, math functions, program translate/rotate mirror, file compare and CNC communication. Side-by-Side File Compare (ENHANCED in v5) - our file compare is fast and fully configurable allowing users to choose whether to view differences one line/section at a time or all at once. Our file compare even supports side-by-side printing for offline review. Excellent 3D Mill / 2D Lathe Open-GL Back Plotter (ENHANCED in v5) - plot your 3-Axis Mill and 2-Axis lathe CNC programs inside CIMCO Edit with step and continuous forward and reverse synchronized plotting. Excellent 3D Mill / 2D Lathe Open-GL Back Plotter (ENHANCED in v5) - plot your 3-Axis Mill and 2-Axis lathe CNC programs inside CIMCO Edit with step and continuous forward and reverse synchronized plotting.

CNC Calc v5 : Calculations for CNC-programs can be both hard and time-consuming. They often include complex calculations of for instance intersection- and tangency points. Traditionally these calculations have been performed using calculators and trigonometrical tables.

CIMCO CNC-Calc 2 is a fully featured 2D CAD solution that works inside CIMCO Edit 5. This add-on is a fast and effective solution for solving problems with complex 2D geometry.

CIMCO CNC-Calc 2 has been designed with usability in mind, which makes it easy and fast to draw contours. Its comprehensive functionality ranges from functions such as the plain "horizontal line" to the complex "circle tangent to three elements". It includes advanced trimming options and a simple point and click approach to laying out tool paths and drill cycles.

CIMCO CNC-Calc 2 imports AutoCAD DXF files and generates toolpaths, drill patterns for ISO and Heidenhain conversational programming. Other features include automatic generation of configurable lead in/out containing lines and arcs. CIMCO CNC-Calc 2 has been integrated with CIMCO Edit 5 so it is easy to edit and simulate the generated tool paths. This helps to ensure that the program behaves correctly and to avoid unnecessary use of time and machine resources.

www.nctech.in