Introduction

In this topic we will cover each of the default post blocks in the Mill post processor. The purpose and use of each block will be explained. It is important to know that the description or name of the block may differ from post processor to post processor as the name (the text to the right of the post block number) is not used by the post processor engine, and is simply a reference to aid in understanding the purpose of the block.

 

The post blocks are organized by numeric sequence. This post blocks themselves may or may not be in numeric sequence in a post processor

Tool Change Blocks

Block 1. Start of File Program Zero

This postblock is not in use and should be removed from all current *BCPst post processors

Block 2. Start of File Standard

This postblock is used to output the 1st tool and any startup commands that may be desired at the beginning of an NC program. This block is only ever called 1 time at the beginning of an NC program. This block where the following should happen:

 

• Initialize the 1st tool and tool offsets (Length and Diameter)

 

• Define current Work Piece coordinate system

 

• Define active working plane

 

• Spindle speed and ON codes for the proper direction

 

• Output initial XY and Z moves for the operation.

 

• Define any Coordinate Rotation, Origin Tracking/Dynamic Work Offsets(DWO) or RTCP/TCP commands. - Each of these commands have special variables and/or blocks that are used to implement these functions. Please see related sections for more details.

 

• Turn on any coolant/vacuum commands

Block 3. Tool Change

This postblock is call at the beginning of an operation where the tool in the spindle must be changed. This applies to all tools after the initial tool at the start of the program. Any operation startup commands and initial position moves for the current machining operation should be output from this block. Below is a list of the items that should be output from this block:

 

• Initialize the new tool and tool offsets (Length and Diameter)

 

• Define current Work Piece coordinate system

 

• Define active working plane.

 

• Spindle speed and ON codes for the proper direction

 

• Output initial XY and Z moves for the operation. 

 

• Define any Coordinate Rotation, Origin Tracking/Dynamic Work Offsets(DWO) or RTCP/TCP commands. - Each of these commands have special variables and/or blocks that are used to implement these functions. Please see related sections for more details.

 

• Turn on any coolant/vacuum commands

Block 4. Null Tool Change

Null Tool Changes are when the NC program is changing from one machining operation to another where the same cutting tool will be used. No physical change of the tool is done, however the new machining operation must establish all of the proper settings for the new cutting operation. Below is a list of the items that should be output from this block:

 

• Initialize the new tool offsets (Length and Diameter)

 

• Define current Work Piece coordinate system

 

• Define active working plane.

 

• Spindle speed codes

 

• Output initial XY and Z moves for the operation.

 

• Define any Coordinate Rotation, Origin Tracking/Dynamic Work Offsets(DWO) or RTCP/TCP commands. - Each of these commands have special variables and/or blocks that are used to implement these functions. Please see related sections for more details.

 

• Turn on any coolant/vacuum commands

Block 5. End of File

This postblock is used to terminate the NC program. This is where commands that were turned ON in the active program should be turned off or set back to an initial state. By terminating commands it will remove possible errors when the next program is started where the new program does not define the proper state for items like active working plane, work coordinate..etc. Below is a list of the items that should be output from this block:

 

• Establish an ending work piece coordinate system.

 

• Move the machine to an end of program position. Commonly used to aid in the operator loading and unloading the parts from the machine.

 

• Load the 1st used tool back into the spindle to speed up the process of running the same program again.

 

• Any special characters needed by the controller to terminate the program.

 

Job Type:

• Mill
• Lathe
• Mill Turn