Post Processors - Solidworks with HSMXpress
- Thread starter psyko62
- Start date
Please use this post while we get our post made for fusion360.
homebrew_cnc
homebrew_cnc
@masso-support Is this post complete? I've seen one available on autodesks website-which I downloaded and tried, but it doesn't work for probing. Is it usable for milling?
never used gcode from fusion for probing, been writing manual gcode for probing, will be interesting to see how it can be done via fusion.
@homebrew_cnc what's your plan/application for probing using fusion? this is new for us.
@homebrew_cnc what's your plan/application for probing using fusion? this is new for us.
homebrew_cnc
homebrew_cnc
@masso-support To answer your question, it's really just what @testyourdesign is working on: I just want a reliable method of referencing tops and corners of stock or centers of bores/shafts to reliably setup WCS. I used probing ALL the time on mach3 to find corners and stuff and it was a lifesaver so many times. If I break a tool or anything that causes me to lose my work offset, then I could just probe the corner or center back in, and keep going and it was within .001 easily. It's especially useful when flipping or doing multiple ops on parts because you could use machined features as your WCS and you knew it was dead on. Now I have to use a manual edge finder which doesn't help with finding the Z, and they're just frustrating to use.
Please don't take this as a gripe, because I'm still SOOO happy with the Masso, and your work to make it better everyday. You guys have made an amazing product and anyone that asks, I constantly recommend it. I'll say though, it's kind of frustrating that probing isn't fully supported yet. I asked in an email before I ever bought my Masso, if probing was supported and I got a yes, with a link to your probing page. My fault, but I just assumed that the site wasn't up to date, but the link I got isn't probing, but just tool length management. Don't get me wrong, that's an awesome feature to have, but these are CNC machines; there's no reason we shouldn't be able to use electronics to find our corners and centers, or even go as far as verifying sizes of parts and features while the part is still on the machine.
I've tried experimenting with the MASSO post and probing but I can't even get it to give me G-code. Every other post that I've tried (Haas generic and Fanuc generic) gives me G65. That to be the probing standard from what little I've looked the last couple days-even for Haas and Fanuc, as I can't find much on G38.2
Please don't take this as a gripe, because I'm still SOOO happy with the Masso, and your work to make it better everyday. You guys have made an amazing product and anyone that asks, I constantly recommend it. I'll say though, it's kind of frustrating that probing isn't fully supported yet. I asked in an email before I ever bought my Masso, if probing was supported and I got a yes, with a link to your probing page. My fault, but I just assumed that the site wasn't up to date, but the link I got isn't probing, but just tool length management. Don't get me wrong, that's an awesome feature to have, but these are CNC machines; there's no reason we shouldn't be able to use electronics to find our corners and centers, or even go as far as verifying sizes of parts and features while the part is still on the machine.
I've tried experimenting with the MASSO post and probing but I can't even get it to give me G-code. Every other post that I've tried (Haas generic and Fanuc generic) gives me G65. That to be the probing standard from what little I've looked the last couple days-even for Haas and Fanuc, as I can't find much on G38.2
Attachments
thank you @homebrew_cnc for the detailed explanation, will email autodesk and see how they can help us on this.
@testyourdesign any ideas or contacts at autodesk who can help on this?
@testyourdesign any ideas or contacts at autodesk who can help on this?
testyourdesign
testyourdesign
@masso-support
Sorry for not being as active these days. I am so swamped with work that I can't break free to comment as much as use to.
As you might have guessed programming for Probing in Fusion360 requires a custom post processor for each machine controller. So far they only provided Post Processors for Probing on the large CNC machines which use like HAAS. I was able to get an output from Fusion360 without any errors using the HAAS, HEIDENHAIN, and OKUMA post processors. Those controllers use custom macros written to make use of the functions in the machine controller and a Renishaw probe.
I think that @masso-support will need to develop the Macro's needed for them to implement this function in the post processor. Lars suggested reading the Fanuc CNC Custom Macro's book for insight on how to do this if you are not familiar with it. Take a look at the G-Code generated by the OKUMA posts to see the custom macro calls below...
(Okuma Probe1)
N4 T3 M06
N5 T7
N6 G15 H06
N8 G00 X0. Y0.
N9 G56 Z6.2 H03
N10 G65 P9832
N12 G65 P9810 Z0.2 F10
N13 G65 P9812 Z-0.12 X12.0485 R0.24 Q0.4 S1.
N14 G65 P9812 Z-0.12 Y3.7808 R0.24 Q0.4 S1.
N15 G65 P9810 Z6.2
N16 G65 P9833
N17 M05
N18 G90 G00 Z400.
Here are some good lessons to learn how to use the Probing Function in Fusion 360 CAM but the Fusion360 post processor for Masso does not support it at this time.
Lars Christensen Explains Probing in Fusion 360
Fusion360 Mastering WCS Probing Videos
Fanuc Custom Macro Programming
Cheers, Stephen Brown
Sorry for not being as active these days. I am so swamped with work that I can't break free to comment as much as use to.
As you might have guessed programming for Probing in Fusion360 requires a custom post processor for each machine controller. So far they only provided Post Processors for Probing on the large CNC machines which use like HAAS. I was able to get an output from Fusion360 without any errors using the HAAS, HEIDENHAIN, and OKUMA post processors. Those controllers use custom macros written to make use of the functions in the machine controller and a Renishaw probe.
I think that @masso-support will need to develop the Macro's needed for them to implement this function in the post processor. Lars suggested reading the Fanuc CNC Custom Macro's book for insight on how to do this if you are not familiar with it. Take a look at the G-Code generated by the OKUMA posts to see the custom macro calls below...
(Okuma Probe1)
N4 T3 M06
N5 T7
N6 G15 H06
N8 G00 X0. Y0.
N9 G56 Z6.2 H03
N10 G65 P9832
N12 G65 P9810 Z0.2 F10
N13 G65 P9812 Z-0.12 X12.0485 R0.24 Q0.4 S1.
N14 G65 P9812 Z-0.12 Y3.7808 R0.24 Q0.4 S1.
N15 G65 P9810 Z6.2
N16 G65 P9833
N17 M05
N18 G90 G00 Z400.
Here are some good lessons to learn how to use the Probing Function in Fusion 360 CAM but the Fusion360 post processor for Masso does not support it at this time.
Lars Christensen Explains Probing in Fusion 360
Fusion360 Mastering WCS Probing Videos
Fanuc Custom Macro Programming
Cheers, Stephen Brown
homebrew_cnc
homebrew_cnc
@testyourdesign Thank you so much for the time you put into this and your explanations. Please forgive me for not being very familiar with macros, but are those the Pxxxx commands? The results I get from the Haas post are almost identical to that. Would it work if we find/replace G65 with G38.2?
testyourdesign
testyourdesign
@homebrew_cnc
Yeah replacing those lines of code for the G38.2 method should eventually work but it would require a couple additional lines to incremental G91 before G38.2 and set adjust the temporary work offset using G92 in order for G38.2 to work properly.
The P numbers are identifying the macros that need to be executed by the controller. Masso does not support custom Macros this way.
Cheers, Stephen Brown
Yeah replacing those lines of code for the G38.2 method should eventually work but it would require a couple additional lines to incremental G91 before G38.2 and set adjust the temporary work offset using G92 in order for G38.2 to work properly.
The P numbers are identifying the macros that need to be executed by the controller. Masso does not support custom Macros this way.
Cheers, Stephen Brown
thank you @testyourdesign
if more people show interest in this then we can try to modify the fusion post.
if more people show interest in this then we can try to modify the fusion post.
Any progress made towards pragmatically probing with Masso?
This is a feature, I will admit I thought I had when I purchased the controller, but have since then just been watching for it to be implemented.
It would be so useful! Especially for retrofits or more "industrial" machines like the ones I run. Anything trying to meet a precision spec, or implement any form of automation.
swisscoy2000
Member
Well i state that it would be realy practical to use the F360 probing function with the Masso G3 controller for very precise products.
But i dont get it why not more ask for it here.
Maybe the average hobbiest user is happy with the results he gets from his diy or rebuild machine... idk.
It would be realy a powerful "tool" to have, it would push the skill of everybody a quantumstep ahead! a few mouseclicks and 2-5 min invested in a "between cuts probing" and of you are to the mikron races!
You could drive out a lot of flaws from a not so precise build machine.
Bedleveling - probing - cutting - reprobe - recut - perfection!
But i dont get it why not more ask for it here.
Maybe the average hobbiest user is happy with the results he gets from his diy or rebuild machine... idk.
It would be realy a powerful "tool" to have, it would push the skill of everybody a quantumstep ahead! a few mouseclicks and 2-5 min invested in a "between cuts probing" and of you are to the mikron races!
You could drive out a lot of flaws from a not so precise build machine.
Bedleveling - probing - cutting - reprobe - recut - perfection!
breezy
Moderator
MASSO had it in the TODO list but it was low priority, back in 2020, I don't know the current status.
As per v5.09 release notes
And from docs
So these probing features have been added since this thread was started.
swisscoy2000
Member
Ok i will fumble with that around. But those or that function gives me data files.
What i wanna do is have a live connection to the feed from the probe into f360.
Then i can automate many things.
When that interconnection ist established i would to have manualy insert the coordinates i did probe.
And that i would not know how to do at all.
Thy
What i wanna do is have a live connection to the feed from the probe into f360.
Then i can automate many things.
When that interconnection ist established i would to have manualy insert the coordinates i did probe.
And that i would not know how to do at all.
Thy
Same here as well. I don’t want to go through and manually program probing routines into every program I write. I want to use fusion 360 to write them for me and the resulting logic right where I program my toolpaths and see the entire “program” all on one screen.
-Brad
swisscoy2000
Member
Hi Brad.
Good news i wrote Fusion360 a mail we will see what they gone do about that implementation idea. Maybe they are working on it.
Good news i wrote Fusion360 a mail we will see what they gone do about that implementation idea. Maybe they are working on it.
breezy
Moderator
That will never happen.
The best is data is dumped to text file on USB drive.
You need to read the documentation and understand what each probe function will do and how you can use it.
swisscoy2000
Member
Why would that never happen? Why should noone give it a try? It ths certain not impossible.
That isnt the problem, i would need to know where to insert the new probing data in f360.
Regards
That isnt the problem, i would need to know where to insert the new probing data in f360.
Regards
breezy
Moderator
MASSO is a standalone controller without the need to connect to a PC.
Trying add connection software to G3 would lead to all sorts of problems, similar to suitable Touch Screens for G3 and also there are NO ports on the G3 for connection to PC.
Touch Screen Interface
I bought a 19" ZB190TC-591R (https://nl.aliexpress.com/item/32819856199.html). And it works. Out-of-the-box the calibration of the resistive touch screen was off. Not by much, but in the lower-left corner it was hard to hit the shift and 'num' key, for example. iChawk offers Windows (Mac...
forums.masso.com.au
Research Fusion tutorials - Autodesk Learning.