T1(Thread Mill Bit)
M39DIAdia[Dd|Zz][Hh]
Spindle ThreadMill macro code (for spindles with threadmill bits),where
dia specifies the outer thread diameter
d specifies the depth to mill to in releation to the surface (+ve down) (where 0 = full through + overshoot)
z specifies the depth to drill to in releation to the surface (+ve up). If neither d or z is specified the it will mill with d=0 (ie full through)
h specified thread type 1 = right hand thread (default), -1 = left hand thread
eg:
for full through
M39DIA100.
to given depth
M39DIA150.D12.
Threadmill Settings in Touchcut
Where:
Spindle RPM (or Cut Speed): Speed of bit at the tip
Horz Feed Per Rev XY feedrate. (Vert feedrate vs XY should be small so vert feed ignored)
Type Thread Mill
Shaft Diameter Diameter of shaft. This diameter is also used to calc the movement required to clear the thread at the end of a cut and where to rapid to at the start (ie the hole blank must be at least the final hole diameter minus the difference between the tip diameter and the shaft diameter).
Tip Diameter The diameter at the outside edge of the tip.
Tooth Pitch The tooth pitch
Tooth Count The number of teeth
Tooth Taper H If the first few teeth are tapered (to allow multi-pass cutting), what is the height of the all the tapered teeth? (ie how much extra overshoot is required)
Notes:
▪If it is a multi-tooth bit then it will start threading with only 1.5 of the teeth above surface height. However if Tooth Taper H is non-zero it will start with all teeth above the surface.
▪Threading will complete when Tooth Taper H + 1.5 teeth are below the bottom of the plate.
▪If taping to a depth, taping will start at least 1.5 revolutions above the final depth.
▪There is no feed override available
Tool Setup in PrimecutNE
Tool Settings
Lookup Specifier
False
Select Code
(Thread Mill) - This is just a comment
T1(ThreadMill) - Assuming the tool specifier is 'ThreadMill'
Start Code
M39%1:s%0:s
%1:s knows to look up the diameter of the circle geometry and %0:s looks up the depth of the hole from the properties window
Could also add a tool parameter for left or right hand thread.
Could also add a parameter for depth per pass. Not sure if this value could be pulled from the depth per pass setting for the bit? if not then could have a tool parameter with a few options.
Machine Settings
Diameter Code (%s).
DIA%s
This is important as by default Primecut will specify diameter with just a 'D'
Adding Tool Parameters for more flexibilty
Adding options to tool paramaters gives more flexibility to the tool. Here is an example of helical milling with 3 bit options and 6 pitch options. You could also add a direction option if required.
Pitch options don't make sense for threadmilling itself, the pitch is fixed so this is using the threadmill to interpolate holes with an endmill- however you just need to do a normal milling process with Movement set to Ramped(Helical) to achieve this now
Select Code
T1($TOOL_PARAM:Bit$)
Start Code
M39%1:s%0:s$TOOL_PARAM:Pitch$
Tool Params
Processing and NC
Bit setup in Touchcut
Where:
Spindle RPM (or Cut Speed): Speed of bit at the tip
Horz Feed Per Rev XY feedrate. (Vert feedrate vs XY should be small so vert feed ignored)
Type: Thread Mill
Shaft Diameter: Diameter of shaft. This diameter is also used to calc the movement required to clear the thread at the end of a cut and where to rapid to at the start (ie the hole blank must be at least the final hole diameter minus the difference between the tip diameter and the shaft diameter).
Tip Diameter: The diameter at the outside edge of the tip.
Tooth Pitch: The tooth pitch
Tooth Count: The number of teeth
Tooth Taper H: If the first few teeth are tapered (to allow multi-pass cutting), what is the height of the all the tapered teeth? (ie how much extra overshoot is required)
Notes:
- If it is a multi-tooth bit then it will start threading with only 1.5 of the teeth above surface height. However if Tooth Taper H is non-zero it will start with all teeth above the surface.
- Threading will complete when Tooth Taper H + 1.5 teeth are below the bottom of the plate.
- If taping to a depth, taping will start at least 1.5 revolutions above the final depth.
- There is no feed override available
See Also