Latest update 15th Oct 2024 - download the latest version of the
Fusion 360 post processor for Tormach
PathPilot. If your browser opens the file and displays it on your
screen instead of downloading, right click the link and select 'Save target
As...' (MS Edge) instead. This isn't a bug as such, it's just that
your browser recognises the file type and thinks it knows what to do with it
15/10/24
Adds the ability to output the work piece size to the
top of the CAM file. Very useful to see when outputting an old design.
Adds the ability to specify a cooling mode to be used
in conjunction with an ETS. If you happen to have a multi mode coolant
system and arrange for air coolant to point at your ETS, then this can be a
good way to clean chips from the ETS before attempting to measure a tool.
Also fixes a couple of bugs associated with optional
CAM operations and the block delete function in PathPilot. Under some
circumstances, in the previous release, turning on the block delete function
could result in the coolant mode not being set properly for the operation
following the optional one. Also, if the last operation in a program
was marked as optional, then turning on block delete resulted in
the program shutdown sequence also being marked as optional. Hence
things like stopping the spindle, turning off the collant and retracting to
the finished location wouldn't happen if block delete was turned on.
No sooner did I release the February version - the
first for 2 years - than someone found a bug that's been there since the
beginning of time. Feed rates have always been output with 1 digit
after the point when working in inches and 0 digits after the point when
working in mm. That works fine for everything, except rigid tapping
very fine threads where it can result in threads being damaged. This
has now been corrected.
There were also a couple of issues with the newly
added ability to add block delete characters, Again these have been
corrected.
A major update. Major enough to give it its own
page, but the highlights are. To see the in depth description of each
new option visit the dedicated page
for this release.
Option to add a delay after flood cooling on to
allow pump to get up to speed
Added support for Fusion's 'tapping with chip
breaking' cycle.
x, y and z coordinates of nominal probe point can
be added to the description output of inspection probing results.
Useful when using a CAM pattern to probe multiple values along a given
feature.
g-code output can be arranged into separate
subroutines for each CAM op. The subroutines are stored at the end of the
output file, so the top of the file consists of a sequence of subroutine
calls. This makes it easier to set a restart location if a program
has to be stopped and restarted.
Fusion's WCS probing cycles now have more probing
speeds than they used to. There's now an option to replace speeds
previously entered as post-processor options with the values specified in
the CAM operation if you wish.
CAM operations marked as optional are output with
the leading '/' character on each line to enable the block delete
function.
The 'optional' property of some Manual NC CAM
operations are not visible to the post-processor. To get round this
and enable block delete on ETS tool setting commands, there's now a
post-processor option to output all tool measure and tool check options as
optional.
A major revamp to the way coolant modes are
handled. There's a new post processor setting to allow you to
specify the type of coolant setup you have and, depending on your
selection, Additional coolant modes specified in the CAM operations can be
handled. (air, mist, flood and mist + flood).
Corrects the handling of a situation where
consecutive operations use the same tool number but with different tool
length offsets, In the past, the 2nd op wouldn't generate the
required tool change code.
The retract options for 'Retract on WCS change' and
'Retract on work plane change' (3+1 machining) were turning off the
spindle and coolant and then turning them on again after the move.
this was unintended and is now removed. This will speed up the code
slightly.
An update to Fusion 360 revealed that there was a
mistake in the post-processor code. The new version of Fusion raised
a warning when posting code, indicating there was a problem, but the post-processor worked
correctly anyway. The post-processor is now modified to prevent the
warning being raised. The generated code should be unchanged.
10th May 2021
The way in which custom post-processor properties
are defined has been updated to match the latest posts from Autodesk.
When viewed in the 'NC program' setup, the properties are now arranged in
groups with group titles. Makes it a little easier to navigate.
If you have a 'Manual NC - comment' immediately
before a 'Manual NC - Stop' operation, the comment will be output on the
same line as the M0 (or M1 for optional stop). This will cause the
comment to be displayed as a banner across the bottom of the screen.
If the comment happens to be the name of an image file, or video, then the
contents will be displayed where the toolpath preview normally is.
Added support for left hand tapping - sadly this
doesn't work in the current release of PathPilot. It's beign worked
on!
Added a 'Retract on optional stop' to match the
'Retract on Manual NC stop' option that's been there for a while.
For people with ATCs, there a new pair of
properties to allow you to ask for an extra tool change at the end of a
program. Re-loading the first tool in a program can save a little
time if you're running the same program for multiple parts one after the
other.
18th Feb 2021
Added support for Manual NC commands to turn
inspection probing on and off. When inspection probing is on, WCS
probing routines do not in fact update the WCS. Instead they write the
results of the probing operations to a text file named 'inspection.txt' in
the user's file area.
This feature is turned on and off by adding a 'Manual
NC' operation with an operation type of Action. Set the action
text to Inspection on to enter inspection mode, set the action text
to Inspection off to switch back to regular probing mode.
For examples of how to do inspection reports, watch
the following.
28/10/2020
Added support for partial circle probing operations
(boss and bore). (Path Pilot 2.7 and later)
Added support for position and size tolerance checking in all WCS probing
functions. (Path Pilot 2.7 and later)
Added Manual NC and tool library support for tool setting/checking.
Replaced 'Use G30' and 'Use G28' post-processor properties with much more
flexible properties to control retraction.
Full details of the updates are discussed in this
video.
The XooomSpeed post processor provides a number of
functions not supported by the standard post processor from Autodesk.
500 WCS support
Some bug fixes for Smartcool support in drilling
operations
Integrated WCS probing operations
In process use of electronic tool setter to set
tool lengths and/or check tool lengths for tool breakage
Spindle reversing on PCNC440 (requires a
USB I/O module).
Expanded g-code tapping cycles (Required to use a
tension/compression tapping head on a PCNC440 with non-standard spindle
reversing).
Support for I/O modules in generated g-code. (added
26/06/20)
Some of the above require new custom properties to be
added to the Fusion 360 Post process dialog. These are described
below.
Integrated Probing
Supports all the Fusion 360 WCS probing routines
(except axis rotation). You can use this with either wired or wireless
probes to perform a number of flexible probing routines to simplify your
setup procedures. Watch the following video for a tutorial on how
these work.
Fast probing speed (inch/min)
The feed rate used for the first part
of the probing operation. This is always specified in inch/minute,
nomatter what units are used for the g-code output. Suitable
values depend on the acceleration/deceleration performance of your
machine, but the default is 20 inch/min
Slow probing speed (inch/min)
The feed rate used for the final
probe. This will generally be somewhat slower than the fast probe
speed to ensure good accuracy of the final result. Defaults to 1
in/min
Slow probe distance (inch)
After the first, fast probe, the
probe will retract this distance away from the detected surface before
starting the slow probe. Default vale is 0.040"
In process tool setter support
The in process ETS support allows tools to be measured
using and electronic tool setter during a program run. Tools can
either have their lengths checked against the current settings in the
controller's tool table, or the tool table can be updated with the newly
measured values.
These operations can be performed at the start of a
propgram, when each tool is loaded or unloaded or even after every machining
operation.
Warning
The ETS functions use Tormach's G37 and G37.1
extensions to the standard LinuxCNC g-codes. Before you use these
options, please make sure you have read the G37 and G37.1 documentation from
Tormach and make sure you have the G37 locations correctly set up and the
ETS referenced.
ETS diameter limit (inch)
The maximum diameter tool that can be
measured using the ETS. Generally this is the diameter of the pad
on the top of the ETS. No action will be taken for tools larger
than this except in the case of 'drills' and 'spot drills' which can
always be checked irrespective of their diameter. Likewise, probes
are never measured by the ETS routines.
Tolerance for ETS checks (inch)
For 'check' operations, this is the
allowed error between the measured tool length and the tool length in
the PathPilot tool table. It is the value of the 'P' word supplied
to G37
ETS op before start
What action to take before the start
of the first machining operation. The action will be applied to
all the tools used in the program, so long as they are not a probe and
they have a tool diameter (in the Fusion library) that is acceptable
according to the ETS diameter limit above. Options are 'none, 'check' or 'set'
ETS op before a tool is used
At each tool change, this operation
is performed immediately after a tool is loaded and before the operation
begins.
ETS op after a tool is used
At each tool change -- except the
first - this operation is performed on the tool being unloaded.
This will generally be 'check' in order to detect a tool that's been
damaged and abort the program so as to avoid damaging subsequent tools.
ETS op after every machining
operation
Check/set tool length after every
machining operation. Useful with multiple WCS or CAM pattern
setups. Using the 'Check' option here means that the tool length
is checked after each machining operation. It it's out of spec
(Tolerance for ETS checks) then execution stops. In the case of
multiple parts in multiple WCSs the tool length will be checked after
each operation on each part and execution will stop the first time the
tool is detected to be out of tolerance.
I/O module support
The I/O support options make it possible to signal to
one of our USB I/O modules that various useful
actions are taking place in your program. the pre-configure applets
supplied with each I/O module can make use of these features to trigger
various custom sequences. User written applets also have full access
to this information
I/O ETS in use
Signals to the I/O module that one of
the ETS functions above is about to take place. This gives the
opportunity for the I/O module to open a cover over the ETS and/or
operate an air blast to clean the ETS.
I/O ETS ready
Select an input that PathPilot will
wait for before starting the ETS function. The idea here is that
the I/O module can request a delay to finish opening a cover and
cleaning with an air blast before allowing Pathpilot to continue with
the ETS function.
I/O flood cooling
Turn this output on any time that
flood cooling (M8) is running. typically this would enable
monitoring of a flow switch to verify correct operation of the coolant.
I/O mist cooling
Similar to I/O flood cooling
above, but this output is active with mist cooling (M7).
I/O Program running
The selected output will turn on at
the start if your program and turns off again at the end.
I/O Spindle running
Indicates that the spindle is turned
on (forward or reverse)
I/O tool change in progress
Turn this output on when a tool
change starts and back off again once the tool change is complete.
Tapping for PCNC440
Tapping operations are normally inpossible for a
PCNC440 because spindle reversing is not provided on that machine.
Spindle reversing
Normally set to 'M4', use the other
options to get spindle reversing working on a 440. If your 440 has
a USB I/O module with one of the outputs connected to the F/R and COM
pins on the BLDC drive, then you can have spindle reversing by
outputting one of the other options depending on which USB I/O channel
you've connected.
Use M3 M64 P0 if you have used channel 0 of
the USB I/O module to control the spindle direction and son on for the
other I/O channels.
Expand tapping
This will work on all the mills, but
is essential on the 440 with non-standard spindle reversing. Instead of outputting tapping ops as a
canned cycle, this outputs long hand g-code to do the job. When
tapping is done in this way, the spindle direction is controlled using
the Spindle reversing options above.
