NC Tracer \\ Built-in Post Processor
NC Tracer is the internal post processor built into ThreadTracer. Its a simple but complete post processor for posting ISO G-code for all threads and options possible in ThreadTracer.
It operates independently and therefore does not use GibbsCAM threading operations or need GibbsCAM post processorsors. Primary used for machine tools in your shop that does not have a GibbsCAM post processor.
It can also be used if your current GibbsCAM post processor does not correctly output code for threading with ThreadTracer.
NC Tracer will also output g-code for multistart thread using the G32/G33 Q parameter, the advantage with this is that it can thread a multistart thread in tight places.
GibbsCAM only supports multistart threads with offsetting the Z start point for each multistart. But if you need to start with the tool in a thread relief with no room to offset,
the Q parameter allows the tool to start at the same Z value, and uses the decoder in the spindle to control each start.
An example would be a lefthand multistart thread, but with only a righthand tool available. Solution would be to start at the end of the thread and run the tool in the Z+ direction and use Q parameters for each start.
10 configurable presets for seperate machine controllers.
All G codes and M codes are configurable.
Outputs multistart threads with Q parameter to set the startangle instead of offsetting every start like GibbsCAM does.
Saves posted g-code to an external text file or copies gcode directly to clipboard.
Output Point-Cloud data file, for milling the thread with MillTracer.
Loading a machine preset
Select a machine preset from the dropdown menu and click the 'Load Machine' button
After a machine preset is loaded, you can start to customize it to the machine controller.
Build up settings for any machine by filling in the G and M codes required with the control.
Consult your machine manual or machine tool distributor for M or G codes, unless you can pick them up from your GibbsCAM post.
Machine Name : Display name of the configuration inside the dropdown menu and inside the output G-code
NC Header :
6 entries or lines available for setting up things before any threading starts.
Insert any required G or M codes here, like code for lower turret, or code for running on sub-spindle.
Machines with custom threading options, like variable spindle speed to help with chatter, insert this here.
NC Footer :
6 entries or lines available for setting up things after the threading is done.
The last line should be used for the 'Program Stop' command.
All CNC controllers needs this to 'end' the program properly.
Usually 'M30' on fanuc compatible controls, most Okuma machines uses 'M2'
Optional Output :
Optional switches, mostly informational output.
'Insert M1 Stops' will output an 'M1' optional stop after roughing passes are done.
'M1 after every cut' will output an 'M1' optional stop after every single cut.
File Formatting :
Post in Metric : disabled, units for posting are controlled by GibbsCAM in 'Document Control'
Post in Inch : disabled, units for posting are controlled by GibbsCAM in 'Document Control'
Prepare as 'Add Gcode'
This will output every line in double quotes, so it can be inserted inside a GibbsCAM program with the plugin 'Add Gcode'
Output to Clipboard
Will skip asking your for a file to write to and copy all G-code output to the clipboard, handy to just paste directly into your preferred editor or DNC utility.
Set file extension for saved files (NCF,EIA,MIN,etc)
Rounds the X/Z coordinate values to set number of decimals (X32.4446445 becomes X32.4446) Metric machines should use atleast 3, and imperial machines atleast 4
G & M Codes :
The G Code for Single Point Theading.
On Fanuc compatible controls this is usually G32. Most if not all Okuma controls use G33.
The letter used for Pitch in the Single Point Theading cycle.
Usually this letter is F.
The M-Code for turning ON coolant for the threading tool.
The M-Code for turning OFF coolant for the threading tool.
The M-Code for Clockwise spindle direction.
Used for Right Hand threads and threading toward the -Z axis.
The M-Code for Counter Clockwise spindle direction.
Used for Left Hand threads and threading toward the -Z axis.
The G-Code command for homing the X axis. On Fanuc compatible controls this is usually 'G28U0.'
The G-Code command for homing the Z axis. On Fanuc compatible controls this is usually 'G28W0.'
The letter used for sequencing, Fanuc compatible controls uses the letter N, some Okuma controls NAT
The letter used for startangle on multistart threads, Fanuc compatible controls uses the letter Q.
The amount of 'units' the C-axis have as resolution. Fanuc compatible controls uses 0.001, so one revolution is 360000
With Angle Increment of 0.001, a 2 start thread would use Q0 for the first start and Q180000 for the second start (180° offset)
Consult your machine manual or machine tool distributor for for the correct format.
Part Clearances :
CAUTION ! All threading clearances used by NC Tracer are taken from GibbsCAM -> 'Auto Clearance'. If 'Auto Clearance' is disabled, it uses the manual Xd clearance set in dialog.
So with auto clearance set to 1mm, the tool will do all rapid moves 1mm from the Major diameter on external threads, and 1mm below the Minor Diameter on internal threads.
Keep this in mind when setting up INTERNAL threads, and the size of your tooling compared to clearance.
Insert the 'T' command to select the tool used, there is one tool for roughing and one tool for finishing.
If you want one seperate tool for running finishing with, select the 'Use seperate Finishing' and enter another 'T' command here.
The finishing tool must be identical as the roughing tool. (same width, same corner radius)
If your toolchange command requires and M Code, you must also include that.
An Okuma Multus uses for example 'TD=010001 M323'
Posting NC code :
Posting a program with NC Tracer is controlled in Tab 7 (Control)
Select a machine preset from the dropdown menu, and click the 'NC Postprocessor' checkmark. Select to do Roughing or Finishing, or both, and click 'Do It'
The resulting G-code file will automatically be opened in with Notepad.exe
Using Toolpath geometry to visualize NC code :
Use the option 'Draw Toolpath Lines' to get an idea on how the NC code will run. The outputted NC code from NC Tracer are identical to what the 'Draw Toolpath lines' will show.
Example output of g-code for an Acme multistart thread with Q parameters for 4 different startangles.
Page accessed : 268 times