⇩ Switch interface tabs with the buttons below to view documentation for each tab ⇩
Acme Thread \\ Thread Options (Tab 5):
Bluntstart / Quickstart parameters
Enable Blunt Start : This will enable machining of Blunt Start threads.
Stepdown Xr : Set the depth of cut for blunting cuts.
Stepover Z : Set the width of cut for blunting cuts.
Blunt Revolutions : Set the amount of revolutions of thread to remove.
Spindle RPM : Set to use 100% or 50% RPM for blunting cuts. 100% will use the same RPM as roughing cuts, 50% will use half the RPM as roughing cuts
Run-Out Angle : Set the angle the blunting cuts will exit the thread. 0 is straight up and will produce the shortest blunt.
Run-In Angle : Set the angle the blunting cuts will enter the thread. 0 is straight down.
Height to remove : Set the percentage of thread height to remove. 100% will remove the thread down to the root. 90% will leave a tiny amount and often results in a better finish.
Select from the dropdown menu what percentage of thread height to remove. 50%, 60%, 70%, 80%, 90%, 95% and 100% are available.
Mach Style : Select machining style for blunting.
- Right-Left : Cycles the blunting cuts from right side to left side in the Z direction.
- Left-Right : Cycles the blunting cuts from left side to right side in the Z direction.
- ZigZag R-L : Cycles the blunting cuts in an alternating pattern, first pass in right-left Z direction, then left-right on the next pass.
- ZigZag L-R : Cycles the blunting cuts in an alternating pattern, first pass in left-right Z direction, then right-left on the next pass.
- Center Out : Places the first blunting pass in the center of the thread, and cycles the blunting cuts towards the sides.
- Sides Only : This will only do blunting passes along the outside of the thread profile.
Right Offset and Left Offset can be used to offset the blunt in the Z axis. Positive and negative numbers.
Right Offset : This will offset all the blunting cuts on the right side.
Left Offset : This will offset all the blunting cuts on the left side.
This can be used to adjust the width and also the position where the blunting cuts will run.
With moving the blunting cuts towards the end of the thread, its possible to machine away the sharp portion of the thread at the end.
Move the blunting cuts by counting the number of threads / revolutions and multiply this with the pitch.
Lets say for 15 threads / revolutions on a 4 TPI thread, set both Right Offset and Left Offset to 15*6.35(mm) or if you work in inches, 15*0.25(in)
Always remember to use Run-in angle when moving blunting into the thread. Without Run-in all the blunt cuts will rapid into the thread.
Exit Cut : Set feed exit or rapid exit for when exiting out of the thread. Setting this to rapid will use G0 for exiting out of the thread.
Enable Run In / Run Out : This will enable to use a run in and run out for the threading cuts.
Run Out Xr : Set the amount for run out [X axis]
Run Out Z : Set the amount for run out [Z axis]
Run In Xr : Set the amount for run in [X axis]
Run In Z : Set the amount for run in [Z axis]
Enable Tapered Thread : This will enable a taper on the thread.
Taper Xr : Set the decimal Xr slope. An NPT thread has a slope of 1/32 per side.
Enable Full Profile Exit : This option will make the exit cuts follow the thread profile.
This can be used if the thread have no relief groove, or if the thread requires a smooth exit out of the material.
Control buttons at the bottom.
Use the buttons at the bottom of the ThreadTracer dialog to turn on or off actions to make.
Everything in the window is controlled by the 'Do It' button.
You can turn on/off options, generate visual geometry, change cut depths, change tool sizes and everything will be recalculated and updated when you press 'Do It'.
As long as the 'Process Ops' or 'NC Postprocessor' are disabled, no GibbsCAM operations or g-code will be generated.
Set up the all the roughing and finishing of the thread and only enable 'Process Ops' when everything seems correct. With 'Process Ops' enabled it will generate GibbsCAM threading operations.
Material Control : This will enable material control, and keep all threading cuts within the set limits. By default the limits are always set to Major and Minor diameter.
Do Roughing : This will enable roughing of the thread. When enabled it will run the roughing of the selected thread with the set tool parameters.
Do Finishing : This will enable finishing of the thread. When enabled it will run the finishing of the selected thread with the set parameters.
Process Ops : This will create GibbsCAM threading operations for all the calculated thread coordinates.
'Do Roughing' and 'Do Finishing' can be set individually. If only 'Do Finishing' is enabled and 'Process Ops', it will only create GibbsCAM threading operations for the finishing passes.
Click 'Do It' button to start running the options that's selected.
Click 'Save Data' to store the current thread setup into the GibbsCAM program
It will create a new data entry if its a new thread, after the thread setup is stored the button will change to 'Update Data'.
This way you can store and update the same thread entry, and not create a completely new thread entry every time the 'Save Data' is clicked.
If you need to create a new data entry in the GibbsCAM part, you must close ThreadTracer and restart it, and it will now start with a new data entry.
These lines of text can also be copied and pasted into other GibbsCAM programs, to quickly recreate the thread without typing in all the parameters again.
Page accessed : 319 times