How to Set Up a Tool Change
How to perform a tool change in Mach3 with a preset tooling system (Tormach Style Tooling System)
The first step to doing a tool change is to go to the "offset page" in Mach3.
Click On the "save tool offsets" button,
This will bring up the tool table for Mach3, this table and the information within the table is where Mach3 will pull the appropriate info for the tool.
(1) We must set up a master tool, a master tool is a tool with the value of zero, this tool is used as a master tool to measure the difference between each tool we are going to place into the table.
I will generally leave my master tool as the same tool and never change it, I always use my spot drill as my master tool. This is due to the fact that it does not wear or break easily.
Change and hit apply.
Close this window and select tool 1 in the tool window.
We are then going to jog the machine with this tool to the top of your part and touch off the part.
The best way to do this is to hold a regular piece of paper on top of the material to be machined and gently wiggle the piece of paper while slowly jogging the Z Axis down. The goal is to gently pinch the piece of paper with out going totally through it.
Once this is done go to the offset page.
Then press the (Zero Z) button, this will then zero the (DRO) for the z tool.
We will then jog the Z Axis up and insert tool 2, we will say tool 2 is a 3/8 end mill.
We will then touch tool 2 to the top of the part. (Note, do not change the tool to tool 2 leave tool 1 active) this allows us to know the difference in length between tool 1 and tool 2.
Again, the best way to do this is to hold a regular piece of paper on top of the material to be machined and gently wiggle the piece of paper while slowly jogging the Z Axis down. The goal is to gently pinch the piece of paper with out going totally through it.
Once we touch off tool 2 we will see a number in the Z Axis DRO.
This number means that tool 2 is longer than our master tool by .250.
We will then open the tool table and add tool 2 with the exact info that is located in the Z Axis DRO (.250).
Presto, we set up tools for a tool change in Mach3, this method works well for the Tormach style of tooling setup. This is due to the fact that the tools are preset in holders and never change, unless you break a tool.
If you do break a tool you would then put in tool 1 touch off on the part and zero,(make sure tool 1 is active) or a block (anything) jog the axis up and put the appropriate tool in the holder, insert the tool into the spindle and touch off the tool. Again, whatever the DRO says for the height information is the info you will put into the table for that tool number.
M6 Tool change
Once this is done you would call a tool change like this,
Z2.0 (call the z up to a location to change tool)
G49 (cancel the previous tools height offset information)
(base rough 1/8 ENDMILL) (list which tool is to be changed)
M6 T2 (call the tool change and change preset tool, this will also stop the spindle)
M03 S3500 (start the spindle at 3500 rpm)
G04 P5. (give a 5 second pause to allow the spindle to get up to speed)
G43 H02 (apply the tool height information for this tool)
It is important to call the tool height for this tool, or it may crash.
Make sure the G43 (H02) matches your tool number, it is possible to have tool 2 in and accidentally use a height offset from a different tool (ie) (H03).
(copyright) Syil Canada 2009
Do not use with out permission