If the threading operations are made in the wrong plane, clicking the 'Repair' button will try to restore the GibbsCAM threading dialog to a working state.
If a repair has been done, all the current threading operations needs to be deleted and redone.
NC Postprocessor : Enable this to post the current thread with the internal post processor.
You can select what machine configuration to post for in the dropdown list.
The machine configurations can be edited with selecting 'NC TRACER POST PROCESSOR CONFIG' as thread type and pressing the 'Switch' button.
If you post with the internal post processor, it will ask where to save the NC-code file and open the file in Notepad.exe when its done.
You can also configure NC Tracer to paste the NC-code directly to the clipboard, and paste it directly to your preferred editor.
To read on how to setup NC Tracer for your machine, click here : Nc Tracer Setup
Used for roughing cuts, and if using one of the Special Roughing Style, as CT->Right Side, CT->Left Side, Right Side->CT or Left Side->CT
Will use an angle for the center stepdown positions to prevent the tool to rub against the same sidewall throughout the cycle.
Use boundaries for Finishing Cuts : This should always be enabled for safety.
When calculating finishing passes, it will only follow the geometry of the thread profile without checking distance to neighboring profile geometry.
This will first scan through the thread profile and calculate internal boundaries for all the finishing passes.
Add Finish cuts over Crest flats : This will add finishing cuts over the crest of the thread profile.
This can be useful for threads with tight tolerances as all surfaces will be relative to the same tool offset.
Enable this to select what features to run finishing passes on.
The finishing passes will run on the features selected on the thread profile geometry.
Select individual features with holding CTRL button and select with the the mousepointer.
This can be useful for a large thread where you only need to re-run finishing on selected features to save some machining time.
• Select features of the thread you want to finish. • Enable 'Use Custom Finishing Order' in the Control tab
• Clicking 'Do It' will generate finishing for selected geometry only
Enable this to monitor the insert geometry against the thread flank walls or sides.
If the sides of the insert gouges or crosses the thread profile, it will trigger an alert and not output or generate threading operations. The insert profile will be drawn in red if alert is triggered.
Note : False positives might occur due to small mathematical rounding errors, disable Tool Monitor if you can visually confirm that the tool clears the profile correctly.
Tool Monitor Strict Mode (Back to top)
This will monitor the thread flank walls upto the crest diameter, and ignore the crest corner radius or chamfer.
• Ratchet thread and VBMT insert that gouges thread profile
• Ratchet thread and VBMT insert pointing down, no gouges
• Acme thread and VBMT insert that gouges thread profile
Nested Toolpath option will combine all roughing passes or finishing passes into a single threading operation.
A Nested Toolpath looks similar as a normal threading operation in GibbsCAM and uses only one operation tile.
It will seperate roughing and finishing into each seperate operation tiles. As any nested toolpath is built internally by ThreadTracer, you cannot Redo these operations in GibbsCAM.
For machining threads in long-chipping materials, like different plastics, titanium, aluminum and some steel alloys.
Wave Chipbreaker can be used on any thread and will apply oscillating movements to the X axis while threading as an attempt to break up long strings of chips.
Advantage is preventing long strings of chips to coil around the chuck, tools or the part. Disadvantage is longer machining time, as these oscillating thread passes needs a straight cleanup pass.
For automated machining solutions, good chip control is critical for a reliable process. Picking up a part with a robot or a sub spindle in the machine can cause problems if long strings of chips are curled around the part.
Wave Chipbreaker can solve problems with chip control in scenarios like this and can help the process to be accurate and more reliable.
Wave Chipbreaker was inspired from Sandvik Coromant OptiThreading™ - a new software module in their CoroPlus Tool Path.
All credit to Sandvik Coromant for coming up with this method for chip control. Read about OptiThreading™ here.
Wave Chipbreaker is only available when using Nested Toolpath.
Wave Chipbreaker thread pass with a following straight cleanup pass
Machining 4-TPI thread with a 2mm grooving tool. Top corner shows NC-code running while machining.
Set the amount of segments per wave. 2 segments produce a saw tooth wave and requires the least amount of lines in the NC-code.
More segments produces a more detailed wave and requires more lines in the NC-code to complete the wave.
See example NC-code below for difference between 2 segments and 6 segments (Expandable buttons).
Click the buttons below to expand and display example NC-code snippets for differences between 2 and 6 segment wave.
This is NC-code posted with the internal post-processor in ThreadTracer. GibbsCAM post-processors will output same NC-code coordinates for threading.
Wave Length will determine oscillation frequency, or how often it will attempt to break the chips per spindle revolution.
Select from the dropdown between 0.5x pitch, 1.0x pitch, 2.0x pitch and 4.0x pitch
Wave length set to 1.0x Pitch, will move the tool in and out of the material for every revolution.
Wave length set to 2.0x Pitch, will move the tool in and out of the material for every second revolution.
The tool will be in sync with the thread in the Z axis during all wave motions while the X axis moves in and out of the material.
Keep in mind that spindle RPM can affect the ability to accurately run at different wave lengths.
A small diameter and high spindle RPM can cause the machine's X axis to not fully reach the peaks of each wave before it continues to the next wave.
Other factors can also impact this from machine to machine, such as parameters for acceleration/deacceleration or mechanical backlash in the ballscrew.
This can be compensated with a combination of either longer wave length, lower spindle RPM and higher oscillation height.
Oscillation Height is the effective wave height.
Select from the dropdown between 1.25x Stepdown Xr, 1.50x Stepdown Xr, 2.00x Stepdown Xr, 3.00x Stepdown Xr and 4.00x Stepdown Xr.
Stepdown Xr is the cut depth that is set in Machining tab (Tab 4).
Setting the oscillation height to 2.00x Stepdown Xr, the tool will move out of the material with a height twice of the current cut depth (Stepdown Xr).
Wave Penetration will make the tool to oscillate a set amount past the following straight threading passes.
Depending of the material being machined and if chips not breaking properly with the tool, it can help with setting a penetration percentage to better break the chip for the following straigt pass.
Select from the dropdown the amount of penetration. Selecting No Penetration will do the wave movements at the same diameter as the straight threading passes.
Enable to loop the thread profile geometry along the entire length of the thread. From Thread Start Z to Thread End Z in Machining tab (Tab 4)
Due to a limitation set in GibbsCAM, max 100 loops will be drawn.
Draw Profile over whole thread -OFF Draw Profile over whole thread -ON
Enable to draw a red outline for the roughing stock. The red line will be parallel to the thread profile with distance as the Roughing Stock set in Machining Tab (Tab 4).
Red stock geometry is just a visual reference, and will not have any significance to the roughing process.
Draw Stock as Red geometry -ON Draw Stock as Red geometry -OFF
Holds information of the calculated Rough Cuts in the current programmed thread. 'amount of cuts' [ hh:mm:ss ]
Rough Cuts 60 [ 00h 04m 01s ] means roughing the current programmed thread requires 60 threading passes with an estimated machining time of 4 minutes and 1 seconds.
Holds information of the calculated Finishing Cuts in the current programmed thread. 'amount of cuts' [ hh:mm:ss ]
Fin Cuts 112 [ 00h 07m 29s ] means finish machining the current thread requires 112 threading passes with an estimated machining time of 7 minutes and 29 seconds.
Est. Run Time shows the calculated Run Time for machining, for all Roughing and Finishing passes combined.
To improve the time estimate, you can set your machine tool Rapid Feedrate in the Settings tab. Your machines rapid feedrate can be found in the parameters of the machine.
As there are as many rapid moves as feed moves in machining a thread, setting the correct rapid feedrate will allow for a more precise time estimate.
If you work in metric, set the Rapid Feed in millimeters/minute. If you work in inch, set the Rapid Feed in inches/minute.
Default values in ThreadTracer are 12000 millimeters/minute for GibbsCAM in metric and 500 inches/minute for GibbsCAM set to inches.
Everything in ThreadTracer 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.
'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.
As ThreadTracer is an external plugin, there is no 'ReDo' button. If you need to change anything you must delete the threading operations in GibbsCAM and create new ones in ThreadTracer.
If you delete the threading tool instead, all the operations in GibbsCAM that used that tool will be removed, this is often faster than selecting multiple operations with scrolling for deletion.
ThreadTracer will always create a new tool based on tools settings from the Tooling tab (Tab 3) if no previous tool exists.
If you are using NC Tracer to generate g-code for machining, Process Ops should be disabled(off) and instead enable 'NC PostProcessor' in Tab 7.
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.
With version 4.32 and higher its not necessary to use 'Save' button. All thread data from ThreadTracer are written to each operation and retrievable by using 'Get From Op' button instead.
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.
Visual Delay Timer for in between each calculated thread pass.
The Delay Timer can be useful for delaying the visual geometry drawn in GibbsCAM. If something seems off, it can sometimes help track the error with a delay and confirm that every pass is done correctly.
Delay Timer was initially used in development of ThreadTracer, but kept it as it can be useful to slow things down if there is a suspicion of some passes not being laid out correctly.
Online Guide button will open this ThreadTracer documentation in a new web browser window.
ThreadTracer will parse information on what thread style and tab thats currently open, and redirects the web browser to the relevant page.
Clicking the 'Online Guide' while in Stub Acme and Tab 5, will open the documentation for Stub Acme and Tab 5.
This feature is available in all versions of ThreadTracer v4.35 and up.
Advanced Entry & Retract allows you to select the placement of the thread on the part using point geometry instead of setting start and end using numbers.
This can be used for threads that require special placement behind a feature or around an obstacle.
• Part for threading
Surface for threading
Setup the thread profile and place the thread machining positions outside the part using 'Thread Start Z' and 'Thread End Z'
Place geometry points to be used as an extended toolpath for the threading cycle. These points can quickly be placed freehand with mouse with using 'Mouse Point' in the Geometry Palette.
The tool will always start where you placed the thread profile, so place points to guide the tool to the surface on the part.
For this example, the surface that will be threaded are behind this obstacle so we need to place points to guide the tool around.
To designate a point to be an entry or retract point, select the point, right-click a point and select "Change feature from "WALL" to "AIR".
Do this to every point where the tool needs to move in air.
Entry point 1
Entry point 2
Retract point 1
Retract point 2
Thread point 1
Thread point 2
Thread point 3
Thread point 4
By selecting these points in a spesific order, you select the points used for entry, points used for thread surface and points used for retract and return back to start.
All points that have been set to "AIR" (red) will automatically be set and used as entry and/or retract points by ThreadTracer.
Points that are normal (yellow) will be used as thread surface.
Thread point 1 -> 2 will be equivalent to a Run-In angle, therefore you can place Thread point 1 in an angle in relation to Thread point 2.
Thread point 2 -> 3 will be equivalent to 'Thread Start Z' and 'Thread End Z'.
Thread point 3 -> 4 will be equivalent to a Run-Out angle.
Points to be used as thread surface needs to be sets of 4 points.
All red points selected after normal points (yellow) will automatically be used as retract points by ThreadTracer.
Select points by holding CTRL key while you click and select the points in the order you want the tool to move.
With the points selected, pressing 'Do It' in ThreadTracer will bring up a window with information about the points.
The points are automatically sorted and arranged as a new toolpath in the same order as you selected the points.
Confirm to use the points as a guided toolpath by clicking 'Yes' in the window.
The new toolpath will be built with colored lines to visually identify the different features.
Yellow lines represent entry toolpath.
Green lines represent the toolpath for the actual thread.
Red lines represent retract moves for the tool (rapid moves).
Yellow lines will be output as part of the thread, ie tool moves with G32/G33 to keep the tool and spindle in sync.
The new point based toolpath will stay in memory until you close ThreadTracer or select new points again.
Generate roughing and finishing operations or adjust parameters for cutting and recreate operations, and it will use the point based toolpath.
To do multiple surfaces for threading, place points in sets of 4 on the part.
Point 3 and 4 and point 7 and 8 are placed on the minor diameter of the thread.
Point 2 and 5 and point 6 and 9 are on major diameter.
In this example, we want to machine a synchronized righthand and lefthand rope thread on the part.
After selecting the point that will run out of the first rightland thread(pt.5), select the entry point for the lefthand thread (pt.6) and select the rest of the points in Z+ direction. (pt 7,8,9)
If its required for the outer start thread helixes to be oriented equally on the part, start by setting the points 3. and 7. to have a distance relative to the pitch of the thread (whole revolutions).
If the pitch is 0.5", start with setting the distance between points 3. and 7. to whole revolutions. For example 30 x 0.5 = 15", meaning distance between point 3. and 7. to be 15"
If the placement of point 3. and 7. needs to be adjusted, translate the points the same amount in each direction.
Same with the length of the thread surfaces, distance between point 3. and 4. and point 7. and 8. must be identical length.
Confirm to use the points as a guided toolpath by clicking 'Yes' in the window.