⇩ Use mouse and click in the interface to jump down to the relevant section for any spesific element ( tabs,buttons or options ) ⇩
Acme Thread \\ Fillet / Chamfer Tab (Tab 2):
Set the radius or chamfer size on corners of the thread profile.
Fillet/Chamfer : Value here is the calculated radius/chamfer for the thread defined in Tab 1.
Chamfer Angle : Angle of chamfer. Click the radio button to switch to chamfer. The value in the Fillet/Chamfer input box will then be used as the size of the chamfer.
For Acme threads, the Crest values for both sides must be equal and the Root values must be equal.
Control buttons at the bottom (Back to top)
Use the buttons at the bottom of the ThreadTracer dialog to turn on or off actions to make.
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 (Calculated) (Back to top)
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.
Material Control ( Checkmark On/Off ) (Back to top)
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.
You can change upper and lower machining limits for Material Control in the Machining Tab.
Do Roughing ( Checkmark On/Off ) (Back to top)
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 when pressing the 'Do It' button.
Do Finishing ( Checkmark On/Off ) (Back to top)
Do Finishing : This will enable finishing of the thread. When enabled it will run the finishing of the selected thread with the set parameters when pressing the 'Do It' button.
Process Ops ( Checkmark On/Off ) (Back to top)
Process Ops : This will enable the creation of GibbsCAM threading operations for all the calculated thread coordinates when pressing the 'Do It' button.
Everything in ThreadTracer is controlled by the 'Do It'
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.
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.
Page accessed : 443 times