YZ Rotary mode are for rotary milling of incomplete threads in the YZ plane. In this tab MillBlunt will calculate geometry that move the tool simultaneous in the C, Z, and X axis.
To follow the pitch of the external thread, the geometry are angeled in relation to the Z axis to compensate for the helix pitch.
To align the geometry with any C axis value, the geometry are offset in the Y axis. The milling tool moves up simultaneous in all 3 axes to form the blunt.
Geometry for Left-Hand Thread, Front View
Geometry for Right-Hand Thread, Front View
Geometry for Right-Hand Thread, Side View
Select from the dropdown menu the location for machining.
Blunt Start are in front of a thread and move the tool with the selected pitch in the -Z direction. Blunt End are at the end of a thread and move the tool with the selected pitch in the +Z direction.
Its important to select correct location, as this will set the orientation and direction of the 3D geometry in relation if its a Right-Hand or Left-Hand thread.
Pitch of the thread. If the thread uses TPI, the pitch is 25.4/TPI for GibbsCAM in metric and 1/TPI for GibbsCAM in inch.
Pitch = 6.35mm for a 4-TPI thread in metric and Pitch = 0.25 for a 4-TPI thread in inches.
The C axis value of where the thread starts or ends ( where the threading tool entered or exited the material )
The best way to find the C Angle, are to have the C axis engaged and use the jog wheel to position the milling tool right before the feathered edge.
Z position where the mill will start. The Z position are always from the center of the tool, so its best to use the jog wheel to position the mill and use the Z value displayed on the machine display.
Center the mill in front of where the sharp thread starts and the edge of the mill overlaps the feathered edge.
Select if the lead out should be an arc or line. This defines the shape of the blunt.
Set the Lead Out Line length or Arc Diameter in the corresponding input boxes.
If Lead Out Arc is used, set the resolution with number of segments. Segments are for one quadrant of a circle with diameter set in Lead Out Arc.
Segments will only be drawn upto the Exit Thread Height.
Set the number of segments in the main line used for milling.
Segments are necessary if the machine have a parameter set to travel the shortest distance between two points.
The default value of 50 segments should be enough for most cases.
Check this box to automatically select the created geometry and set the machining markers in the correct orientation and on center line.
With Set Machining Markers off, you will need to manually place the machining markers.
For YZ Rotary milling the marker circle must always be in center to place the toolpath on the centerline.
When redoing geometry from MillBlunt with an existing milling process in the process list, the machining markers will be set correctly on the new geometry.
Then you only need to click Redo on the operation, and it will update the toolpath to the new geometry.
Click 'Save Setup' to store the MillBlunt setup into the current open GibbsCAM program.
Any stored data can be imported back into MillBlunt at a later time. All data entries are stored after any existing text here (Programmer notes).
In MillBlunt v2 its not necessary to Save Setups, as all MillBlunt variables are added as a comment to every operation created with MillBlunt, and can be put back with Get From Op button.
After a setup are stored, the button will change state to Update Setup. Pressing Update Setup will update the stored data with the current new one.
All data are stored as lines of text here -> Document Control -> Comments -> Programmer Notes :
Click this button to read thread data from a selected lathe thread operation or a previous created MillBlunt contour milling operation in the operation list.
This allows for a quick setup, as the data from the selected operation will be put directly into MillBlunt.
If the selected operation are a lathe thread, it will read the following data from the operation and insert into MillBlunt :
Select Blunt Start or Blunt End from the dropdown menu before clicking Get From Op and the Tool Z Start will be set approximately at the start or the end of the thread.
Selecting Blunt Start will set Tool Z Start to the Z thread start position from the selected lathe threading operation.
Selecting Blunt End will set Tool Z Start to the Z thread end position from the selected lathe threading operation.
After the lathe thread values have been set in MillBlunt, some input boxes will be indicated with colors.
Input boxes with orange indicators needs to be checked and might need some fine tuning to the Tool Z Start.
Exit Thread Height are automatically set to Thrd Ht Xr + 20% from the selected lathe threading operation and might need adjustment.
Input boxes with blue indicators are the C axis values, these needs to be manually located on the thread and set seperately.
If the selected operation are a previous MillBlunt contour operation, you can read data from the operation and insert everything back into MillBlunt.
Existing milling contour operations created with MillBlunt v2
MillBlunt variables for each contour op are stored in the "Op Comment"
When MillBlunt have read data from an existing contour operation, input boxes will be indicated with green markers.
These variables can be read back again if something needs to be changed.
Using [Get From Op] to edit an existing contour operation (YZ plane)
...
Creating new Process from MillBlunt geometry (Back to top)
For a new part program with no existing MillBlunt operations, you need to first setup a mill contour operation and apply that on MillBlunt geometry.
Type in the known values for the thread. Pressing Do It in MillBlunt will calculate and draw a line like shown in the screenshot below.
The length of the line corresponds to the set diameter and Rotation Length (Deg), so 180° will generate a shorter line, and 360° a longer line.
The line will be tilted along the Z axis, to allow the milling tool to follow the pitch of the thread.
Next, create the milling tool and drag it down to a process tile and make a Contour process. Set the required values for Clearance Plane to be above the Major Diameter of the thread.
Set the Surface and Floor Xr value to half of the diameter you set in MillBlunt. ( All values in GibbsCAM contour in YZ mode are radius )
You can also select an input box in the Mill Contour dialog, then holding down the left ALT key and click on the geometry line, and the correct Xr value will be set.
Its important that both the surface input boxes in the Mill Contour dialog are the same, as the generated geometry extends in 3 dimensions.
Now to create the process, select the Set Machining Markers checkbox and click Do It / Redo in MillBlunt again.
The markers for the milling process will be set correctly in direction and centerline on the new geometry, like shown in the screenshot below.
With the Set Machining Markers checkbox enabled, MillBlunt will close the Contour window and create the contour operation when clicking Do It / Redo in MillBlunt.
After the operation are created, you should see the actual GibbsCAM toolpath (orange) as a curved line wrapped around the part.
