Keyboard Shortcuts
ctrl + shift + ? :
Show all keyboard shortcuts
ctrl + g :
Navigate to a group
ctrl + shift + f :
Find
ctrl + / :
Quick actions
esc to dismiss
Likes
Search
(unknown)
|
G43 is tool length offset. Not sure on G44
toggle quoted message
Show quoted text
Tim [Denver CO] -----Original Message-----I consider this to be a sister site to the CCED group, as many of the same members are there, for OT subjects, that are not allowed on the CCED list. NOTICE: ALL POSTINGS TO THIS GROUP BECOME PUBLIC DOMAIN BY POSTING THEM. DON'T POST IF YOU CAN NOT ACCEPT THIS.....NO EXCEPTIONS........ bill List Mom List Owner |
|
stevenson_engineers
--- In CAD_CAM_EDM_DRO@y..., "Tim Goldstein" <timg@k...> wrote:
G43 is tool length offset. Not sure on G44Tool Length Compensation Syntax - G43 Hnn* ; tool length comp. away from the part G44 Hnn* ; tool length comp. toward the part G49* ; cancel tool length compensation The parameter nn for the H code is the identification number of the associated tool. This value is the tool number displayed on the left side of the screen in the Tool Size window. G43 - Tool Length Compensation Away From The Part G43 assumes zero length tools, meaning the G-code tool, or z-axis, coordinates will specify the length from the quill face to the desired destination position. The offset associated with the tool will then be added to the tool axis destination position. The tool offset data for this command will be the actual length of the tools. Example: If the distance from the quill to the destination position is 10 inches towards the part for the rapid move and 10.5 inches for the feedrate move, and you want to apply tool length compensation away from the part for tool number 0, the G-code commands will be: G43 H0* ; enable tool length compensation for tool number 0 G00 Z-10.0 G90* ; lower the tool at the rapid rate in G90 absolute mode G01 Z-10.5 F10.0* ; lower the tool to the cutting position at 10 ipm If the z axis starting position was at 0 and the offset length assigned in the Tool Size window for tool number 0 was 7.5 inches, the actual length of the G00 move in this case will be 10.0 - 7.5 = 2.5 inches. The offset length is always subtracted when G43 compensation is active. The next command will move the tool down an additional .5 inches, at a feedrate of 10 inches per minute. If a tool change was required at some later point it would only be necessary to cancel the current tool length compensation, retract the tool to the tool change position, and re-enable the compensation while specifying the tool to use for the operation, using the 'Hnn' parameter. However, the offset length must have been previously assigned for this tool before the file is executed. These additional commands might be: G49* ; cancel tool length compensation G00 Z0 G90* ; retract to tool change position M01* ; program pause for the tool change G43 H01* ; re-enable compensation for tool number 1 G00 X2.0 Y1.0* ; position the tool G00 Z-10.0 G90* ; lower the tool at the rapid rate G01 Z-10.5 F10.0* ; lower the tool to the cutting position at 10 ipm The last 2 commands simply continue the sequence of tool axis moves in a similar way as before. Even though the lengths of the two tools may be different, the G-code commands to move the tool to the same destination position remain the same as long as the offset length for each tool is specified properly. Remember that the offset length specified in the Tool Size window, must be the actual length of the tool when using the G43 command. It can be seen from these examples the danger in using the G43 compensation command. Because this command compensates the tool away from the part and assumes a zero length tool, the coordinates in the tool axis moves are all longer than actually desired. The compensation actually reduces the length of travel by the amount assigned in the Tool Size window for the offset length for the specified tool. If this value is assigned a zero the tool move will travel too far, possibly resulting in a collision with the part or table. Please make sure you dry run the program from the Main Screen before execution, if you use the G43 command, to check the proper display position of the z-axis coordinate. Never assume the Tool Size data still exists or have the same data the was previously assigned. This data is stored in DOS files which can easily be deleted, overwritten or otherwise corrupted. At the very least you should check to make sure the Tool Size data is still valid before you run G-code files containing tool length compensation commands. G44 - Tool Length Compensation Toward The Part G44 assumes that when creating G-code commands, the tool axis coordinates are assigned based on a standard length, for an imaginary tool, which is longer than any of the tools in the system. The tool offset length data in this case will be the difference in length between each tool and the standard tool length chosen by the programmer. The offset for this command will be subtracted from the tool axis destination position. An extra calculation is required when using the G44 command, since after the tool length is measured it must be subtracted from the chosen standard length, to obtain the desired offset. It is this difference that is stored as the offset length in the Tool Size window for each tool which will be used in a G44 tool length compensation operation. This method of tool length compensation is actually safer than using the G43 method, since the coordinates for tool move commands will be programmed with a shorter value than is desired. If an offset has not been assigned for the selected tool the resulting move will be shorter than desired and a collision with the part or table should not occur. Example: If the distance from the tip of the standard length tool and the destination position is 2.0 inches towards the part for the rapid move, and 2.5 inches for the feedrate move, and you want to apply tool length compensation toward the part to tool number 0, the G-code commands will be: G44 H0* ; enable tool length compensation for tool number 0 G00 Z-2.0 G90* ; lower the tool at the rapid rate in G90 absolute mode G01 Z-2.5 F10.0* ; lower the tool to the cutting position at 10 ipm If the z axis starting position was at 0 and the offset length assigned in the Tool Size window for tool number 0 was .5 inches, the actual length of the G00 move in this case will be 2.0 + .5 = 2.5 inches. The offset length is always added when G44 compensation is active. The next command will move the tool down an additional .5 inches at a feedrate of 10 inches per minute. As with the G43 command, additional tools could be used at later points in the G-code program. As long as the tool length offsets were properly assigned, the tool axis coordinates would simply reflect the length of the standard tool, and the program would compute the actual destination positions for the specified tool. Since the tool length compensation commands allow the programmer to create G-code programs that are not dependent on the lengths of the various tools that will be used, the programs will be easier to write and maintain. With this greater flexibility and freedom comes additional danger and risk if the commands are not used properly. This is especially true with the G43, compensate tool away from the part, command. If you decide to use these commands please take extra precautions to verify the correctness of the program before actually driving an expensive power tool. G49 - Cancel Tool Length Compensation The G49 command is used to cancel any active tool length compensation operation. If you want to perform a tool change you will almost certainly want to include a G49 command before the retract move is made. If this is not done the retract operation may not be moved to a point that provides adequate clearance for the tool change operation. After the specified tool change or pause command, the previous tool compensation command should be included, to re-enable this operation for the new tool, if so desired. be a-----Original Message-----I consider this to sister site to the CCED group, as many of the same members arethere, for OT subjects, that are not allowed on the CCED list.THEM. DON'T POST IF YOU CAN NOT ACCEPT THIS.....NO EXCEPTIONS........ bill |
to navigate to use esc to dismiss