⇩ Switch interface tabs with the buttons below to view documentation for each tab ⇩
Trapezoidal Thread \\ Control (Tab 7):
Import ThreadTracer data from current open GibbsCAM program.
All the parameters and settings for a thread setup can be stored inside the GibbsCAM file, this allows for loading back the same setup into ThreadTracer if you want to change something later.
Import 3.x Data : This button will check for thread setups made with ThreadTracer 3.x.
Import 4.x Data : This button will check for thread setups made with ThreadTracer 4.x.
If any are found they will be presented and you can choose to load them back.
Switch to another thread type
Choose what thread type to make from the dropdown list.
Switch : Clicking this button will switch the thread setup to the one selected from the dropdown.
Run a repair if thread ops appear in wrong plane.
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 g-code file and open the file in Notepad when its done.
To read on how to setup NC Tracer for your machine, click here : Nc Tracer Setup
Options for toolpath
Enable Angle for Center cuts : This is for roughing cuts, and if the Roughing style is one of the center ones. It will place the center roughing cuts in an angle instead of straight down.
Use boundaries for Finishing Cuts : This should always be enabled. This will first scan through the thread profile and calculate boundaries for finishing passes.
Add Finish cuts over Crest flats : This will add finishing cuts over the crest of the thread profile.
Use Custom Finishing Order
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.
Enable Tool Monitoring
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.
- Tool Monitor Strict Mode : Will monitor the thread flank walls upto the crest diameter, and ignore the crest corner radius or chamfer.
Options for visual geometry
Draw Tool Coordinates as Points : This will create a yellow point for all thread coordinates.
Draw Tool Wireframe for all cuts : This will draw the current tool as geometry for all thread coordinates. This can be useful during setup of the thread.
Keep Tool Wireframe on screen : This will not delete the tool wireframes, and leave every tool geometry on screen.
Draw Texual Thread Data : This will write thread information such as Major/Minor diameter, TPI and Pitch, etc as geometry. (Currently not available)
Draw Profile over whole thread : This will loop the thread profile along the entire thread.
Draw Stock as Red geometry : This will draw the stock profile of the thread, as red geometry. (On as default)
Draw Tool Gouges as Red Wireframe : This is if the Tool Monitor is enabled, if tool geometry gouges or crosses the thread profile, the tool will be drawn as red geometry.
Draw Toolpath Lines : This will draw the toolpaths for all threading passes as geometry, this can be useful to see the toolpath without processing threading operations.
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 : 139 times