ThreadTracer for GibbsCAM
header_logo
ThreadTracer
Home Features Documentation Media Updates Download Purchase
Additional

MillTracer
MillBlunt

Resellers
Contact

GIbbsCAM Macros

Understood
This website is using cookies for analyzing webtraffic with Google Analytics. More details
ThreadTracer 4 - Online Guide

   Switch interface tabs with the buttons below to view documentation for each tab  
                      Thread Data Fillet / Chamfer Tooling Machining Thread Options Settings Control                                                                        

Trapezoidal Thread \\ Machining (Tab 4):

Roughing Parameters

  • Roughing Engine : Standard and adaptive are available. The standard engine are best suited for Trapezoidal style threads.
  • Roughing Style : Select roughing style
  • - Right-Left : Cycles the roughing cuts from right side to left side in the Z direction.
  • - Left-Right : Cycles the roughing cuts from left side to right side in the Z direction.
  • - ZigZag R-L : Cycles the roughing cuts in an alternating pattern, first pass in right-left Z direction, then left-right on the next pass.
  • - ZigZag L-R : Cycles the roughing cuts in an alternating pattern, first pass in left-right Z direction, then right-left on the next pass.
  • - Center Out : Places the first roughing pass in the center of the thread, and cycles the roughing cuts towards the sides.
  • - Sides Only : This will only do roughing passes along the thread profile.

  • - CT->Right Side : This will do roughing passes from the center of the profile towards the right side.
    - CT->Left Side : This will do roughing passes from the center of the profile towards the left side.
    - Right Side->CT : This will do roughing passes from the right side of the profile towards the center.
    - Left Side->CT : This will do roughing passes from the left side of the profile towards the center.

    The 4 last roughing styles will only rough half of the profile and should not be used for regular threads.


  • Stepdown Xr : Set the depth of cut for roughing.
  • Stepover Z : Set the width of cut for roughing.
  • Roughing Stock : Set the amount of material to leave for finishing.

  • Offset R and Offset L can be used to offset the roughing passes in the Z axis. Positive and negative numbers.
  • Offset R : This will offset all the roughing cuts on the right side.
  • Offset L : This will offset all the roughing cuts on the left side.
  • For example, setting Offset R to -0.2, will leave 0.2 more material on the right side in addition to the Roughing Stock.

  • Avoid Micro Cuts : Filters out small roughing cuts based on a threshold.
  • This option will compare the previous depth of cut to the current depth of cut, and if the amount is smaller than a certain amount, it will skip and move to the next roughing cut.
  • Skip Small > : Threshold value used for Avoid Micro Cuts. Any cut size less than entered here will be skipped when generating the roughing cuts.

  • Adaptive Level : Set the level of detail for adaptive cuts.
  • Default is Coarse and should be sufficient for most cases. It can also give good results with setting a high detail level and keep the 'Avoid Micro Cuts' on.
    A more in-depth look at the advantages of Adaptive Roughing here : (Adaptive Roughing)

  • Force Last Root Cut : This will force roughing the root of the profile.
  • If there is a tiny amount of material left along the root of the profile, the roughing cycle can often skip this.
    Enabling this will always make roughing cuts along the last portion of the profile.

    Finishing Parameters

  • Target Surface Ra: Set the surface roughness for finishing passes in Ra.
  • Ra is calculated as the Roughness Average of a given surface. Lower Ra number produces higher number of finishing passes, higher Ra number produces less finishing passes.
    If the surface requirement is given in RMS, you need to convert it to Ra.
  • Contour Stock : Set an amount of stock for finishing passes.

  • Contour Offset

    Contour Offset R and Contour Offset L can be used to offset the finishing passes in the Z axis. Positive and negative numbers.
  • Contour Offset R : This will offset all the finishing passes on the right side of the profile.
  • Contour Offset L : This will offset all the finishing passes on the left side of the profile.
  • These can be used to adjust the width of the profile when finishing.
    Note : Tool Monitoring needs to be turned off (in Control Tab) in order for the tool to go outside the thread profile.

    Material Control

  • Upper Limit Xd : Set the upper limit diameter for both roughing and finishing cuts.
  • Lower Limit Xd : Set the Lower limit diameter for both roughing and finishing cuts.
  • Any cuts outside these limits will be skipped. Use this to control where to machine.

    For example, if you want to run finishing passes for the last 1/3 of the profile, set the Upper Limit to 1/3 above the Minor Diameter.
    Material Control will only be active if the 'Material Control' is enabled (red outline)

    Material Control will also automatically turn on if any tool is too large to fit the profile. If the tool is too wide to reach the root of the thread, it will allow the tool to go as far as there is space.
    When stopped the Material Control will set the Lower Limit Diameter to where it stopped and ThreadTracer will outline red borders around input boxes that needs to be adjusted.


  • Thread End Z : Set where the theading cycle stops.
  • Thread Start Z : Set where the theading cycle starts.
  • Cutting Speed : The surface cutting speed for machining. The RPM will be calculated based on this and the diameter of the thread.

  • Auto Clearance
  • Make sure to confirm the Auto Clearance setting in the Document Control window, and that the value is sufficient compared to the thread height.

    If Auto Clearance is set to lower than the thread height, it can cause the tool to not properly exit the thread between passes.


    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 : 164 times