Re: Fusion 360 Mill Post Processor for Acorn with additional Features
Posted: Mon Mar 02, 2020 10:04 pm
by slodat
Figured it out.. the M30 is turning everything off. Vectric does an M5, too. I thought it was needed. Everything works as you wrote it. Only problem was me
Re: Fusion 360 Mill Post Processor for Acorn with additional Features
Posted: Sun Mar 22, 2020 4:30 pm
by swissi
A new version of the Fusion 360 Post Processor has been posted.
These new features have been added:
* Select Safe Retract Position for Z-Axis
* Support for Smoothing Profiles
* Inverse Time Feedrates (G93) now used for moves involving a Rotary Axis
Check the first post of this thread for the download link and a link to the updated user manual.
Please report here if you find any issues with the new version.
-swissi
Re: Fusion 360 Mill Post Processor for Acorn with additional Features
Posted: Mon May 11, 2020 6:43 pm
by qjones
Hi swissi this is really good work. I see you have made a lot of progress on your post processor. I just recently acquired an electronic probe. I am curious if you have put any thought into supporting the probing routines from F360? This is something I may just tackle myself as well just curious if you had run into any gotchas that made the implementation not worth it.
Thanks,
Re: Fusion 360 Mill Post Processor for Acorn with additional Features
Posted: Tue May 12, 2020 9:10 am
by swissi
qjones,
Fusion 360 currently supports WCS, Geometry and Surface Inspection Probing. Supported probing moves are:
- Single Axis XYZ Surface
- Circular and rectangular Boss
- Circular and rectangular Hole with and without an island
- XY Channel/Slot with and without an island
- XY Wall/Web
- XY Surface Angle
There are also many options you can select like showing a message when measurements are out of tolerance, adjust tool wear based on measurements and printing results to a log file etc.
Now the easy part is modifying the post processor to output all the codes for these probing routines but when you look at the code lines that are generated, you will notice that subprograms like P9810, P9832 etc are called that do not exist for Acorn (at least as far as I know).
I took it as a challenge to write the probing routines for all these probing moves supporting all the options for WCS and Geometry probing and I’m at a point were these routines are very solid. I created this Probing Model below in Fusion 360 with these probing moves
I created a 3D-print of the model and used the great new KP-3 Touch Probe from Centroid to check the Geometry of the print. I just created a video last weekend showing my machine running through these probing cycles:
The log file of the probing results looks like this:
I spent over 1’000 hours writing all the Fusion 360 probing routines to support all the functionality and I don’t want to give all that work away for free but I plan to make it available for a small donation to the “Keep my Grand Son happy and busy” Fund. I still have to write some documentation but if somebody is interested in these Fusion 360 Probing moves, contact me via PM.
-swissi
Re: Fusion 360 Mill Post Processor for Acorn with additional Features
Posted: Tue May 12, 2020 11:16 am
by cbb1962
So am I understanding the process?
1. You created a 3D part,
2. The part was loaded on your machine,
3. You initiated the probing routine in CNC12 using the new probe
4. The output from CNC12 was imported into Fusion360
5. Your programming voodoo interpreted the output from CNC12 and created a model in Fusion360?
Is that correct?
Re: Fusion 360 Mill Post Processor for Acorn with additional Features
Posted: Tue May 12, 2020 11:51 am
by slodat
PM sent!!
Re: Fusion 360 Mill Post Processor for Acorn with additional Features
Posted: Tue May 12, 2020 12:08 pm
by swissi
cbb1962,
not quiet correct! You setup the probing cycles in Fusion 360 the same way you setup the milling and drilling operations. The post processor will then generate the code for your machine to mill the part and then run the probing routines to measure if the geometric features are within tolerance.
So in a real live scenario you would start with the WCS probing routines to find Part 0 of your stock, then mill a feature, probe that feature for accuracy and the probing routine could automatically adjust the tool diameter based on the measurements if that function was requested in the probing options in Fusion 360. You could also finish your part first and then have the probing routines measure your part for tolerance at the end.
Here's a YouTube video from Autodesk showing the use of the WCS probing functions to setup part 0
So to be more specific of what I did in the scenario I described above, these are the steps:
- I designed the probing model in Fusion 360
- I configured the probing moves to verify the geometry of the part
- Instead of milling the part I just 3-D printed it
- I mounted the 3-D printed part on my mill and ran the probing routines that were generated by the Fusion 360 Post Processor to measure the features
This model in Fusion 360
generated this code with my (not yet official) modified Centroid Post Processor:
As you can see in the code, Fusion 360 just generates calls for P98xx sub-programs that do not exist for Centroid Acorn so I had to write all these probing routines in order to complete the functions they are supposed to do based on all the options selected in Fusion 360.
Hope this explains it better. Let me know if you have more questions.
-swissi
Re: Fusion 360 Mill Post Processor for Acorn with additional Features
Posted: Tue May 12, 2020 3:31 pm
by Muzzer
Wow - well done, Swissi - that's an amazing result! You must have put in a whole lot of work there.
I spent many, many hours trying to do just this myself before I decided to behave myself. As you say, the task of implementing "WCS probing" requires both a lot of work on the Fusion post processor (JavaScript) and also a whole massive set of Centroid probing macros. I felt able to tackle the first part - and indeed got a fair way along the road. But figuring out the probing moves and assembling them into robust probing macros was turning out to be a massive task, not least to digest the existing Centroid macros to work out how all the variables are set up and used. The Centroid documentation is a bit patchy, so a fair bit of reverse engineering seemed to be required. I managed to implement the simple "boss" probing operation working all the way from Fusion, through the post and into CNC12 but this is the simplest (almost trivial) probing operation.
In the end, I considered the time/cost of taking this to completion (including a fair degree of uncertainty in the timescale) and the likely benefit (being able to pick up WCS references) and concluded that I lacked the appetite and capability to take it to completion. I'm not a software natural, so it's great that there are people like you around who can pull it off.
As I understand it, the more sophisticated "inspection probing" functions are only available in Fusion "extensions" - which are ruinously expensive. These are pretty interesting but as they are hidden from us within Fusion 360, there's little chance of being able to implement them. I see you have some tolerance tests in your log file - do they work without the extensions?
There's a guy up in Scotland (David Loomes) who did all this WCS probing work for his PathPilot / Tormach / Fusion 360 setup, including WCS axis angle correction. http://xoomspeed.com/CNC/FusionAutoProbing.htm That's what provoked me into trying it myself but unfortunately I lack his (and your) software prowess. PathPilot / LinuxCNC uses quite different macro variables and calls subprogram numbers (that P9810 etc), so his work wasn't the head start I'd hoped for. He's taken Cliff Hall's ITTP and made it wireless so that it can be used in an ATC.
I'd love to try your latest post processor. The other features you have already implemented are very compelling and this is an extra level of interest for me. Knowing the effort you must have put in, I'd be very happy to contribute to your fund. I'll PM you to find out more....
Murray
Re: Fusion 360 Mill Post Processor for Acorn with additional Features
Posted: Sat May 16, 2020 7:35 am
by hebs
Awesome work Swissi, the probe functionality looks great! Definitely interested in supporting your “Keep my Grand Son happy and busy” Fund.
Your post processor has really helped me to increase my understanding of Fusion/Inventor post processor editing. I have been using Autodesks 'Post Processor training Guide' to try and learn more but I am stumped, are you able to give me a steer please;
ISSUE
I have recently built a 4th axis and I have successfully machined a few part using both indexed and simultaneous tool path operations. However, I cannot get the rotary axis rewind/unwind to a reasonable state. The post processor sets the WCS in between every operation it can cause long rewind/unwinds.
-Example 1 (attached image). A simultaneous tool path operation followed by another simultaneous tool path operation. Sets the WCS to zero in between and causes a long unwind to zero and then a long rewind again to catch up with the next operation.
-Example 2. A simultaneous toolpath operation followed by an indexed toolpath operation may still need to perform a long unwind just to get to zero (or any other index angle under 360deg).
WHAT I HAVE TRIED
Triggering an unwind macro after each operation. This works well when going to an indexed operation next but only solves half of the problem when going from simultaneous to simultaneous operations because it still needs to rewind again. Removing the WCS set in-between worked for simultaneous to simultaneous but prevented indexed operations from indexing.
I have tried to set the 'reset' parameter to 1 in the createAxis function but it does not appear to make any difference.
.....from the Autodesk guide for the reset parameter:
"Defines the starting position of the axis for a new operation and when the rotary axes need to be rewound and reconfigured due to exceeding the limits. 0 = remember the position from previous section, 1 = reset to 0 at start of operation, 2 = reset to 0 at automatic rewind, 3 = reset to 0 at start of operation and at automatic rewind. This parameter is implemented since R42225 of the post engine.'
I have also tried variations on the cyclic and range parameters but to no avail and have failed to apply logic statements.
WHAT I THINK I NEED TO DO
Option 1 (ideal) - Trigger an unwind Macro (which I have already written) after every toolpath operation but this will only work if the next operation doesn't start off where the last one finished. I need to get each new operation to start from zero rather than where the last one left off.
Option 2 - When setting the WCS, I need to insert logic to decide if the command is displayed or not ('A0' in the attached example).
If current section is not simultaneous then run unwind macro and display WCS
If last sect was simultaneous and current section is simultaneous then don't display the WCS
Is my thinking on the right track?
Re: Fusion 360 Mill Post Processor for Acorn with additional Features
Posted: Sat May 16, 2020 11:21 am
by swissi
hebs,
can you post a report file of your setup. I'd like to look at some of your parameters.
