Fusion 360 - Lathe Post ??

More
05 Oct 2021 23:21 #222319 by currinh
Replied by currinh on topic Fusion 360 - Lathe Post ??
OT-CNC:

I think you're right G96 and G97 are modal, you can have G96 or G97 active. These effect spindle speed, G97 for constant rpm and G96 for CSS. The trio of G93, G94 & G95 effect feed. G94 is just constant feed rate, units/minute. G93 is the same but inverse, minutes/unit, and G95 is a synchronized motion, inches/rev. I believe these are modal, selecting one cancels previous selections. At least this is what I gather from the documentation.

I agree with your G30 and G53 comment. Tormach using G30 makes sense if that is part of their tool change. I would likely change the Post to give G53 G0 motions if it wasn't already implemented. I don't trust myself to keep stray values out of the G30 memory locations, and I'm used to G53 motions to machine zero on my mill. I'll likely set machine zero with X retracted, largest diameter, and Z furthest from the chuck (full right). This seems safest. Also use this for manual tool changes (unless motion that far is "too" slow, my parts a typically small).

Thank you for the help.

Hugh

Please Log in or Create an account to join the conversation.

More
06 Oct 2021 13:12 #222353 by andypugh
Replied by andypugh on topic Fusion 360 - Lathe Post ??

 G93 is the same but inverse, minutes/unit, 

That's not true. G93 allows you to specify how long a line of G-code should take to run, so for the same F number in G93 a longer move will feed faster. 
Also, G93 needs an F-number on every line. 
Why it is inverse-time is a mystery to me, maybe just so that larger numbers = faster? Or perhaps to account for integer F-word limitations on old controls?

Please Log in or Create an account to join the conversation.

More
06 Oct 2021 14:39 #222363 by currinh
Replied by currinh on topic Fusion 360 - Lathe Post ??
Andy:

You are right. Thank you for the correction. I swear I will learn to read soon.

Hugh

Please Log in or Create an account to join the conversation.

More
06 Oct 2021 18:51 #222389 by Muzzer
Replied by Muzzer on topic Fusion 360 - Lathe Post ??
Have a look at how VCS handles Fusion post editing and be prepared to be rather impressed. I'm no Javascript expert but this helped me to develop a custom post processor.
knowledge.autodesk.com/community/screenc...334842276.1561580970
This guide is also pretty helpful
cam.autodesk.com/posts/posts/guides/Post...Training%20Guide.pdf

Please Log in or Create an account to join the conversation.

More
07 Oct 2021 00:18 #222414 by currinh
Replied by currinh on topic Fusion 360 - Lathe Post ??
Muzzer:

Thank you. spumco mentioned Visual Studio Code above. I found more information through Google and downloaded a copy. Have been having trouble getting it to run as advertised though.

I also just found the Post Training Manual/Tutorial you mention. In a YouTube video by Russtuff he mentioned it. I'm hoping it has the info I need to get VSC working well. I just need to find the time and energy to study it.

From videos of what VSC can do, it sure would make modifying posts for Fusion easier.

But I fear neither will answer the burning G95 question.

Thanks.

Hugh

Please Log in or Create an account to join the conversation.

More
07 Oct 2021 10:29 #222440 by Muzzer
Replied by Muzzer on topic Fusion 360 - Lathe Post ??
Well the LinuxCNC documentation doesn't really seem to clarify G95 usage. Why not do some testing yourself to see if your suspicions are justified? You can always modify the PP if you think that is appropriate. Perhaps the finishing instruction section generated by the std PP doesn't reset it when it should. Presumably this issue would only happen if you invoked a specific move in MDI anyway, which may be unlikely unless you really know what you are doing.

I'm away from my home and workshop ATM but may look into this tomorrow when I get back.

As you may have noted, Path Pilot is built on LinuxCNC, so perhaps there is better documentation available from Tormach?

VCS seems pretty solid and has great add-ins. You may benefit from talking the time to learn how it is used, otherwise many of the features may pass you by. The add-ins are held in a sort of app store, if you know how to find that from the GUI.

Please Log in or Create an account to join the conversation.

More
08 Oct 2021 03:27 #222515 by currinh
Replied by currinh on topic Fusion 360 - Lathe Post ??
Muzzer:

I may do a little testing. I'm curious what the Post does (regarding G95) with operations other than threading. I have little idea what I'm doing, but I use jog and MDI a lot on my mill as a substitute for a manual machine. I suspect the lathe will be the same.

I may post my inquiry on the Fusion 360 Post Forum. I searched that forum for LinuxCNC Lathe Post and did find some information, but nothing on G95. I'm sure someone there wrote the LinuxCNC Lathe and Tormach Slant Bed posts.

I'd like to get a handle on VS Code before doing post testing though. I think it will help a lot. To get there I'm working through Autodesk CAM Post Processor Guide. I'm also in the middle of converting a 10" lathe and it's not ready yet. Although, my Sherline Lathe would work for this testing.

Thank you for your help. I'll let the list know if/when I make any progress.

Hugh

Please Log in or Create an account to join the conversation.

More
09 Oct 2021 14:09 - 09 Oct 2021 14:09 #222642 by Muzzer
Replied by Muzzer on topic Fusion 360 - Lathe Post ??
Looking into this a bit more closely, there may not be much of a mystery here. G95 (per revolution feed) is pretty much the default setting for lathe operations, while G94 (per minute feed) is the default for milling. When you generate lathe g code from Fusion, most (all?) of the files start with a G95, with not a G94 to be seen. Looking more closely at the post processor code, I don't see how it would actually generate G94. Put another way, there's no reason to ever use G94 on a lathe. You were concerned that manually issuing an F feedrate when G95 is active could cause a problem if you believed G94 to be the default. Apart from the fact that it's not clear when / why you'd do that, it would also seem to be quite unconventional.

I don't know when the LinuxCNC g code set was defined and by whom but they appear to conform to the "Fanuc Group Type B" - and within that, G94 and G95 exclusively occupy "modal group 5". In other words you can only have G94 or G95. It seems you can set an initial  default by configuring the "RS274NGC_STARTUP_CODE =" line within your ini file. Mine simply has G7 (diameter mode) and G18 plane select) ie no G94 or G95. Note that the G33 / G76 cycles are not defined in the original RS274/NGC definition, so have been implemented subsequently in LinuxCNC. linuxcnc.org/docs/2.6/html/gcode/rs274ngc.html.

Interestingly, the LATHE-G76.NGC example file provided within the AXIS sim examples doesn't specify either G94 or G95. I guess feed per rev is perhaps implicit in the command itself.

On the matter of G33 vs G76, I can't seem to force Fusion to generate a G76 threading operation, no matter which options or tick boxes I change within Fusion. I wondered if I was getting G33 due to having selected variable depth of cut / engagement but that doesn't change the result (LinuxCNC calls this "depth degression"). Furthermore, if I select the "use cycle" tick box, Fusion generates the toolpath but the post processor subsequently fails to process the resulting intermediate file. I don't understand how you are generating G76 if you are using the linuxcnc-lathe post or the Path Pilot version of the same.

Bear in mind I'm far from expert in lathe operations, as I am new to it too. Until recently my experience has been limited to milling.
Last edit: 09 Oct 2021 14:09 by Muzzer.
The following user(s) said Thank You: alkabal

Please Log in or Create an account to join the conversation.

More
09 Oct 2021 16:23 #222660 by currinh
Replied by currinh on topic Fusion 360 - Lathe Post ??
Muzzer:

That actually makes sense. I never thought the feed might change in lathe work. But historically for a lathe the change gears sets feed in units/rev. It would make sense this would carry through to CNC. But, if this were true, then the G95 in the above example should be in the program start. Up there with G7 and G18, not in the "THREAD" operation.

The only other lathe CAM I've used is in CAMBAM. It is rudimentary only doing external profiles (no boring or threading). It doesn't specify G94 or G95. I've used it with G94, set before starting the G-code program, and it worked fine. But the feed is an input and I input as in/min.

SOLVED: I just ran a few examples in Fusion. This time I started with a 1/2" bar, faced the end, turned down to 1/4", and threaded. And out popped the solution. The facing and turning asked me to define the feed, in/min or in/rev along with a value. Each operation had the G94 or G95 I requested with corresponding feed. For threading it didn't ask, but threw in a G95 just 'cuz. It does fall off the end of the program with G94/G95 as set in the last operation.

I'm convinced G76 and G33 don't depend on G95. G76/G33 grab the encoder singnal and sync to it independent of feed mode.

I ran this program with and without "use cycles" checked. With it checked it gave a G76 cycle, without it gave a series of G33 commands. I can't verify if it generated the intermediate code (*.cnc ?) but I suspect it had to to make the NC code. This was using the LinuxCNC-Lathe post. I could send you the Fusion model but not sure how to go about this. If this might help let me know and we can work through the details.

So thank you. You've solved the G94/G95 question for me. I may add a G94 (or maybe G95) in the closing so the machine is in a known state. But I at least know what Fusion is doing.

Thank you.

Hugh
The following user(s) said Thank You: alkabal

Please Log in or Create an account to join the conversation.

More
12 Oct 2021 21:12 #222973 by Muzzer
Replied by Muzzer on topic Fusion 360 - Lathe Post ??
As you say, it makes sense when you look into it. I've now got my lathe threading, having connected the encoder the right way round(!) but I'm completely unable to make it generate a G71.

To edit the post processor to include a G94, I think you'll want to add it to the "onClose" section which is executed at the end. You'll be able to see the M30 in there. Javscript isn't very hard to understand.

You can save a Fusion file by cicking the file menu (folder icon at top LHS of screen) and selecting "export". This saves it in .f3d format which you can share as an attachment. You could also create a sharable link but that's less portable perhaps.

Another issue I've found with Fusion is that when I change the thread pitch in the model, it doesn't want to change the pitch in the CAM dialogue or the G33 output itself, even if I remove and reselect the geometry. I don't believe this was deliberate but it resulted in my first test piece having a non-std pitch!

Please Log in or Create an account to join the conversation.

Moderators: Skullworks
Time to create page: 0.432 seconds
Powered by Kunena Forum