Lonely, im so lonely...
I have the DeskCNC program and i would like to know two things about that program.What is Tool Length Offset and how that affects the selection of an endmill?
Did anyone know what the "buffer output" selection at the Machine setup window of DeskCNC does???
Thanks in advance!
Lonely, im so lonely...
Tool lengths may vary, but when you write a program to cut a part, you do not want to be concerned with this troubling matter. For the most part, your program will be written assuming that all tools are the same length, so that when you command a move to Z0, that is where the tip of any of your tools will touch.
Tool length offsets are an internal feature of the controller software which offsets the Z axis (on a mill) so that the differences in actual tool lengths are mathematically subtracted from the Z axis position, relative to a master tool.
To do this, the controller has a table of tool lengths, into which the machine operator enters length values associated with each tool. Typically, he assumes one of the tools is the master tool, and the rest of them are set relative to that one. Various means are used to measure the differences in lengths, but this must be accurately done for satisfactory machining operations later on.
First you get good, then you get fast. Then grouchiness sets in.
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
Thank you for the information.
But from where do you measure tlo?from the collet to the tip?(A section)
or the cutting portion?(B section).Because if your endmill has body diameter 6mm and the cutting portion has 3 mm diameter,i believe you have to take into account the B section.I know that TLO helps in tool changing but,if you can explain what do you measure to find TLO i will be glad!!!Do you need the probe for that job?
Give Me Knowledge!!!
And I Will Use It With Wisdom!!!
You can set your offset to anything you want. It's only a relative dimesion, not an absolute.
And it won't matter unless you have a way of holding your tools that are repeatable in length, like the Tormach Tooling System.
Here is the real TLO scoop. When you set up a CNC Mill, you must have a z home position to reliably use TLO. This requires a home switch on the top of the Z axis travel and establishes Z zero on startup. The next thing that you must establish is what surface you wish to reference all measurments. this surface can be the machine table or a fixture plate. You must also devise some way of holding your tools in a repeatable manner. This can be done by installing stop collars on your cutters. Once this is done, you home the machine then zero Z. Next you install each tool in turn and run the Z down until the tool tip contacts the table or fixture. Use a thin piece of paper to feel when contact is made. Note the travel distance for each tool and set up these distances in the TLO table. Now when you call a tool with G43 the controller compensates for the different Z distances to reach the table or fixture. The next thing you must program is the work coordinate offset (WCO) table to allow for various material thickness. The WCO distance moves Z Zero in the opposite direction to allow for the material being cut. Another option that does not use WCO is to set the TLO of the shortest tool to zero and use the length difference for the rest of the tools. When you begin to work, you touch the top of the material with tool #1 then zero Z. install the working tool and call up the appropriate offset with G43 T# and run. This method does not require home switches.
I hope that I have been of some help.