PDA

View Full Version : Fusion 360: Exporting to Mach 3 Turn?



Doc Nickel
12-17-2016, 06:23 AM
I've been practicing with both Fusion 360's CAD and CAM, learning how to utilize the toolpath generation. I've whipped up a simple test part, basically a gentle profiling of a simple 1" bar and after all too many tries I think I came up with a workable toolpath.

I want to export the G-code in a format that works with my lathe running on Mach 3. However, I'm only given the options of Mach2Mill or Mach3Mill, and when I try to export, it tells me the format isn't compatible and fails.

I'm only given a few options for turning- Fanuc, Siemens, Tormach, etc. No Mach 3. Am I missing something simple, or do they simply not support Mach 3 on the lathe?

Doc.

DICKEYBIRD
12-17-2016, 08:29 AM
Hey Doc, check out this thread: http://forums.autodesk.com/t5/computer-aided-machining-cam/fusion-turn-fanuc-post-fpr-g95/td-p/5761817/page/2 There's a link down the thread to a modified Fanuc post that allegedly works. Be careful & do air cutting before committing to real tools & stock!

Good luck!

DICKEYBIRD
12-17-2016, 08:52 AM
It didn't dawn on me 'til just now; we've uncovered the Holy Grail: free Mach3 lathe CAM that works! (Allegedly) And a forum to go with it!

Doc Nickel
12-17-2016, 04:24 PM
I just love the fact that I've been talking about using Mach on a CNC lathe build for over six months, including in a thread that now has over thirteen thousand page views, and in that time, no one, not one person, even suggested that, oh by the way, there's no real decent CAM solution when using Mach 3 on a lathe.

So I've just spent six months and over a thousand dollars building a lathe I can't use unless I hand-write a program in a code I don't know?

Doc.

elf
12-17-2016, 05:15 PM
It's puzzling why you would use mach3 with its known buggy lathe support when LinuxCnc is available and free.

Doc Nickel
12-17-2016, 05:36 PM
It's puzzling why you would use mach3 with its known buggy lathe support when LinuxCnc is available and free.

-Mach was supposed to be a temporary step. The only "bug" I was aware of was that M3 doesn't handle threading terribly well, and multi-start threads even worse, and as such, I was, in fact, heading towards LinuxCNC because of that very thing.

However, I'm a complete newbie at all of this. I've been a machinist for 20+ years, but I've never owned nor operated anything CNC, and so virtually all of it- CAD, CAM, G-Code, etc.- is entirely new to me.

The the problem with Linux was that I'd essentially need to learn Linux, then learn LinuxCNC, on top of learning CAD and CAM.

It was suggested that, since I already had a prebuilt controller and power supply, and a functioning PC, that a free demo copy of Mach 3 would get me up and running, at least for experimenting and practice if not actual use, and I could then switch to LCNC later. (Or even dual-boot and continue to use both.)

I'm having enough difficulties with just Mach 3- again, it's all entirely new to me, so there's a pretty steep learning curve- that I am NOT looking forward to trying to jump into Linux.

Doc.

elf
12-17-2016, 05:57 PM
There really isn't any need to learn Linux with LinuxCNC. The user interface is close enough to Windows that common things like copying files, executing programs, etc. are the same. Once the ini and hal files have been created for your machine, there isn't much to learn about running LinuxCNC. The user interface is quite simple and there isn't much more to it than clicking on a few icons to run the gcode.

Here's my workflow (for a CNC router):
Create the gcode in Fusion 360 on my office computer
Logon to the LinuxCNC machine (no network connectivity)
Copy the gcode file to the linuxcnc folder
Execute LinuxCNC
Open the gcode file in LinuxCNC
Enable execution in LinuxCNC (two icons to click)
Set home positions for X,Y, and Z
Click on the Run icon

DICKEYBIRD
12-17-2016, 06:04 PM
...there's no real decent CAM solution when using Mach 3 on a lathe.

So I've just spent six months and over a thousand dollars building a lathe I can't use unless I hand-write a program in a code I don't know?Au contraire mon frére; nobody said there was no CAM for Mach. There are many, many excellent CAM solutions; just no good free ones (until now?) I was just making (I thought) a humorous reference to that fact until your/our stumbling across a Mach3 compatible post-processor for Fusion 360. You can buy Dolphin CAD/CAM, or (I forget the many others) whatever your wallet can stand that will make that lathe do fabulous things with Mach but they don' t give 'em away and sorry, they too have a learning curve.

I didn't download & try the Fusion post since I don't know diddly about Fusion; did you try it? Fusion users on that thread I posted mentioned having good success with the one attached to the last post in the thread.

"Stop with the negative waves, Moriarty." You'll get there! I feel your pain but I know you have what it takes to get this working. It doesn't happen with a couple simple mouse clicks though.

EVguru
12-17-2016, 06:14 PM
The the problem with Linux was that I'd essentially need to learn Linux, then learn LinuxCNC, on top of learning CAD and CAM.


There's no more need to 'learn' linux, than there is to 'learn' windows. I recently upgraded a Denford Orac and initially ran LinuxCNC straight off the image downloaded to the USB thumbdrive.

Configuring LCNC for the drives and breakout board was not much different and certainly no harder than configuring Mach.

Since Tormach's Pathpilot is built from LCNC, the Tormach Slant-Pro lathe post processor in Fusion 360 worked OK (I had to edit the tool numbers, that's all).

Doc Nickel
12-17-2016, 06:31 PM
There really isn't any need to learn Linux with LinuxCNC. The user interface is close enough to Windows that common things like copying files, executing programs, etc. are the same.

-Once it's already loaded into your machine. Hell, just downloading LCNC involved doing something with a batch file just to make sure it downloaded correctly.


Once the ini and hal files have been created for your machine[...]

-Yes? And just exactly what are those and how does one 'create' them?

That's been part of my problem- half the responses I get to (what are almost certainly very simple, if not outright stupid) questions make the assumption I know what certain things are, what they do, and how to move, modify, load or otherwise utilize them.

Yes, there's tutorials and YouTube videos galore, but more often than not I'll spend several hours searching, reading and watching, and at the end likely wind up knowing less than when I started.


[T]here isn't much to learn about running LinuxCNC. The user interface is quite simple and there isn't much more to it than clicking on a few icons to run the gcode.

-Yeah, and that's almost exactly what I was told- even here on this very board- about Mach 3.


Create the gcode in Fusion 360 on my office computer[...]

-Which version of G-code? On my copy (which should be the same as pretty much everybody's copy) you're not given the option of "plain G-code". It's all flavors- Simonds, Fanuc, Tormach, etc.

I'm assuming the only significant differences are codes for things like turrets, spindle speed feedback, and other features I don't yet have, that vary from machine to machine, but I'm still green enough I have no idea if that's true, what any particular differences are, or how to change them. And I'd rather not just go down the list trying them at random until something works- if it ever does.

Doc.

Doc Nickel
12-17-2016, 06:46 PM
Au contraire mon frére; nobody said there was no CAM for Mach. There are many, many excellent CAM solutions; just no good free ones[.]

-Considering how much I've already spent on cards people recommended to me that I can't use, steppers that were recommended to me but proved an easy 50% oversized, power supplies that were the wrong voltage for my application, and free software that turned out to not be able to do what it was recommended to me as being able to do, I am NOT looking forward to spending $50 to $500 a pop on paid software until I find one that does what I need it to do.


I was just making (I thought) a humorous reference to that fact until your/our stumbling across a Mach3 compatible post-processor for Fusion 360.

-Despite my total lack of familiarity with any CAD program, Fusion has proven to be surprisingly easy to use, and there's already a pile of useful tutorials out there. Part of it's popularity is that it has a powerful and capable CAM built in, and switching from one to the other is seamless.

But, of COURSE, it doesn't support the one combination of software I'm using.


You can buy Dolphin CAD/CAM, or (I forget the many others) whatever your wallet can stand that will make that lathe do fabulous things with Mach but they don' t give 'em away and sorry, they too have a learning curve.

-I don't mind the learning curve. It's frustrating, sure, but I fully realize the task is a complex one. It might not be brain surgery, but it's not just gapping a spark plug, either.

I am NOT, however, at least for the time being, going to spend $500 on something like Dolphin. At the moment, I'm leery about spending $50 on some software I haven't tried and don't know if it will do what I want.


I didn't download & try the Fusion post since I don't know diddly about Fusion; did you try it? Fusion users on that thread I posted mentioned having good success with the one attached to the last post in the thread.

-Try it? Try what? I read that thread twice and I still don't know what the "fix" is.

Doc.

DICKEYBIRD
12-17-2016, 08:23 PM
OK I downloaded the file. It looks to me like it's what Autodesk says it is: A Post Processor for Fusion 360 CAM that outputs a Mach3 ready G code file. Nothing more, nothing less. I didn't see a lot of talk about how good or bad it might be but if you have trouble, there's good help on their forum.

I would expect that Fusion 360 has a Post Processor list you choose from when you click "Post Process" (or whatever they call it) from within the program. That downloaded PP file has to be loaded into whatever directory Fusion CAM stores the various PP files in. It should then appear as one of the several options to click on when you're ready to post your finished CAM job. I'm not familiar with what Fusion calls these things but CAM programs all do the same sorts of things.

Here's the code that's in the file just so you can see how complex this is and how we have to rely on the knowledge of people that know their stuff and why they (usually) don't do this kind of thing for nothing. I can't try it to see if it works because at 69 years old, I'm not about to learn another CAD/CAM system and besides, it's Sat. night & the kids & grand kids are over for the evening & the pizza & soda (beer for the adults) is flowing. Good luck to you & Merry Christmas!:)


ps: Wow! Had to delete the PP way too many characters to post, trust me it is overwhelming to mere mortals!

Doc Nickel
12-18-2016, 02:22 AM
OK I downloaded the file.

-What file? That .cps file?


I would expect that Fusion 360 has a Post Processor list you choose from when you click "Post Process" (or whatever they call it) from within the program.

-Yes. For turning there's only a few options: Generic Fanuc, generic (their term) HAAS, generic Heidenhain, generic Siemens and Tormach Slant-Pro.

Those are all apparently CPS files, so presumably I'm to somehow load that above file into whatever directory Fusion stores those in? I assume I just open F360 as a folder, and drill down until I find that file, and just drag-and-drop it into place?

Doc.

Doc Nickel
12-18-2016, 03:12 AM
Okay, I got the .cps file dropped in, and it appeared as an option in the post-processor.

I've also been playing with Fusion and made a test part that just gives a slight "wasp waist" to a 1" bar. (If it works, I have a couple pieces that need this kind of cut.)

After at least a dozen tries, I finally got what I thought was a good, viable toolpath, nice and simple. I converted that with the new Mach 3 Turn profile, saved it as a .tap, and since the Logan's computer isn't on the network, sneakernetted it over on a thumb drive.

I got it loaded into Mach just fine, but the toolpath it shows on the demo screen is wildly different from what it's supposed to be. I can see traces of the "right" paths hiding in there, but it's buried under a bunch of big loops and extra zigzags that shouldn't be in there.

I didn't try running it- even with no tool and no workpiece. Without limit switches, it looked like the big loops would run the slides way past limits and likely crash.

Anyone have a clue what I might have done wrong?

Doc.

elf
12-18-2016, 03:16 AM
There is no need to download a post processor file. They're included in the Fusion 360 install. After you create a setup in the CAM module, you create a new turning operation. Once you have the operation created, you generate the post process (gCode). During this, you will select which post processor to use.

You really should read or view the basic documentation for Fusion 360. There are tons of tutorials on the Fusion 360 site like this one: http://help.autodesk.com/view/fusion360/ENU/?utm_id=662996&mktvar002=662996&fgvid=e1306345-a7fb-4458-b134-121f86c47495

Doc Nickel
12-18-2016, 04:31 AM
There is no need to download a post processor file. They're included in the Fusion 360 install.

-Except for one specifically for Mach 3 Turn, apparently.

I'm given no option for "just plain G-code" (if such a thing even exists.) I can only output it in what I'm given to understand is a machine-specific format; IE, a HAAS turning center, a Fanuc turning center, a Heidehain turning center, etc.

If I could just have it post it as 'Generic Fanuc' (their term) and have it work, that's fine, but I don't know that. The part I just tried gave me some wild, drunken, and nowhere-near-correct toolpaths displayed om Mach 3's screen. Is that ebcause of something I did? A bad setting in Mach? A bad toolpath in CAM? A bad post-processing process? I don't know.


After you create a setup in the CAM module, you create a new turning operation. Once you have the operation created, you generate the post process (gCode). During this, you will select which post processor to use.

-All of which are listed as being machine-specific. I'm not at all sure what that means, but at least logically, there wouldn't be thirty-plus options if there weren't thirty-plus differences in how the code gets posted.


You really should read or view the basic documentation for Fusion 360.

-Not to make this sound too snarky, but thank you for assuming I haven't, and that I just want you guys here on HSM to spoon-feed it to me. :)

On the contrary, I've watched at least four dozen YouTube videos, almost all of the ones on that page you linked, I've gone through half a dozen of the Autodesk hands-on tutorials, and I've read countless posts on F360 and Mach 3 on at least half a dozen different boards.

The problem is, almost none of that has to do with Mach 3 on a lathe. The few videos there are are usually demos of an existing, previously-tested program, and almost none of it has to do with getting it set up, or generating a viable toolpath for it.

Worse, I'm screwing with both at the same time- I still haven't even begun to get the lathe and Mach 3 properly sorted out, and I'm trying to get workable toolpaths for it at the same time. The screwed-up sample part I mentioned above? I have no idea if that's a toolpath problem, an export-to-Gcode problem, or a Mach 3 problem.

Doc.

DICKEYBIRD
12-18-2016, 08:58 AM
Sorry, internet is dead. On my phone and it sucks. Try changing Config/General Config/Distance Mode/IJ mode and Config/Ports & Pins/Turn Options/Reversed Arcs in Front Post. There's no rhyme nor reason to curves & PP's at times! (Hate this phone!)

DICKEYBIRD
12-18-2016, 02:29 PM
Internet's back, yay!

Just to add to the previous post, those extra loops you're getting are called "crop circles" & almost every CAM PP & CNC controller has trouble with it. It has to do with how they interpret those pretty curves you've spent your time making in CAD. It's above my knowledge level to be able to explain it clearly but I got around it by searching "Mach3 crop circles" & trying all the different combos until it worked. There seems (to me) no rhyme no reason to it. Has something to do with "Absolute" and IJ arc modes.

Another thing is that sometimes I have to "explode" arcs into the smaller line segments before saving the CAD file & loading it into CAM. Just another trick that has to be used sometimes.

I assume all these "kinks" aren't there in paid-for high $$ CAM programs but I can't afford them. I bought an old version of Dolphin from my Mach3Turn mentor "Hood" on the Mach Support forum for $75.00 with disc & dongle. Yes it was old enough that it has Post Processor problems with Mach too but I didn't complain bitterly about it. I posted polite questions about it on the CNCZone Dolphin forum & nice Mr. Rodney tweaked a few lines of the PP code & it works...most of the time. I still have fits with ID boring of elliptical curves but I do them so rarely I have to try all my tricks to get a usable code. When it works it's a thing of beauty. When it doesn't I want to stab both eyes with an icepick before it's done.:rolleyes:

I sense your growing anger with all this stuff & I know how you feel but it DOES NOT fix itself. It takes much patience & flexibility. None of them are dead-simple no matter what their glossy ads say. You didn't ask me but I still think at your age & business model you'd be well served to make the decision to borrow enough cash to swing a killer deal with Tormach & in no time you'll be making parts.

Have a great day.:)

EVguru
12-18-2016, 03:19 PM
This was my second test piece for the Orac I've just upgraded; http://a360.co/2hJleAR

Designed in Fusion 360 and toolpaths generated in Fusion 360. Two operations, face and profile. The profile roughed it down with linear moves, then ran a number of passes that followed the curves.

The paths shown in LinuxCNC matched those created in Fusion and it came out near perfect on the lathe.

Fusion 360 has HSMWorks as it's CAM core, so it's actually pretty high end.

A quick video of the Orac during its upgrade; https://youtu.be/eN3a7OW2F38

rubes
12-18-2016, 05:48 PM
Worse, I'm screwing with both at the same time- I still haven't even begun to get the lathe and Mach 3 properly sorted out, and I'm trying to get workable toolpaths for it at the same time. The screwed-up sample part I mentioned above? I have no idea if that's a toolpath problem, an export-to-Gcode problem, or a Mach 3 problem.

Doc.

So take ALL that out of your equation!!!! If you couldn't get a simple facing cut code to run, that was generated by the wizard within MACH...why the heck are you complicating things with CAD, CAM and PP's already!!
I hope your not one of those people that thought that once its in CAD that you can just "press a button" and the machine somehow makes the part? There is a reason there are designers that CAD parts, and CNC operators that CAM the parts...completely different animals.

I am one of the "you should learn things from the inside out" people. You should learn some simple g-code and maybe write some simple programs by hand. Here is your simple facing cut that you tried to do with the wizard. It is stripped of everything but the basic moves. copy it into a text file, name it with a .NC (or maybe Mach3 uses .TAP?). then jog the tool to the corner of your 1 inch bar and run. Of course as usual, you should do it in "air" before committing to tools and material just in case.

G18 (select XY plane)
G20 (select inch mode)
G91 (switch to relative coordinates)
S500 M3 (set spindle to 500RPM, start spindle)
F30 (set a feed rate of 30ipm)
G01 X-.5 (move from current position to .5 inch in negative X, toward back of lathe)
G01 X.55 (return to original position plus a little to clear the part)
G01 Z-.050 (move over .050 inch toward the headstock from the current position)
G01 X-.55 (move from current position .55 inch in negative X, toward back of lathe.)
G01 X.55 (retract back out)
G01 Z .05 (return to the original Z position that you were in before running this)
M8 (turn off spindle)
M30 (end of program, rewind and reset modes)

OT...after all the years on this forum, I never realized we cant attach files???

I know your doing this for a business, so "dont have time to piss about" but then like someone else said, you should have bought a running machine ;)
heck, I'm seriously thinking about going to look at this (http://chicago.craigslist.org/sox/tls/5923144018.html)since I will have almost that much into mine when done. But then again, you run into the post processor problem for that controller.

Sparky_NY
12-18-2016, 07:36 PM
I agree with Rubes post. I would add one line in the beginning of the code:

G94 (sets feed per minute mode)

This is because of the suspicion that the machine is in feed per revolution mode now.

Doc Nickel
12-18-2016, 10:36 PM
So take ALL that out of your equation!!!! If you couldn't get a simple facing cut code to run, that was generated by the wizard within MACH...why the heck are you complicating things with CAD, CAM and PP's already!!

Easy. I need the practice on both the CAD and CAM. Even if I don't have a machine to run the drawings on, I still need to, you know, actually DO it. :)

Keeping in mind that up until the past couple of days, I had never once even tried generating a toolpath with a CAM program, of any flavor. I'm totally new at this, so yes, any practice is worthwhile.

Second, I may well be wrong, but I am, for the moment, still operating under the assumption that the issue with the initial simple wizard trial was the lack of a spindle encoder. Later this week I hope to get more shop time with the machine, and I may indeed be proven wrong. The encoder should be in before the weekend, and over the holiday I should have a chance to install it. Even if that proves to not be the issue, I do in fact still need one, so it will not be wasted time nor effort. :)

Third, I may not have managed a successful toolpath, but I did learn something from it. I had never heard the term "crop circles" in this context before, and it is interesting to hear that it is not an uncommon or unique problem.


I hope your not one of those people that thought that once its in CAD that you can just "press a button" and the machine somehow makes the part?

-Hardly. :D I've been a machinist to paintball-playing kids for almost 20 years now, and I've lost count at how many of those kids think they can buy a custom-fitted, hand-made, hand-polished part for about the same price they can get the generic off-the-shelf version for.

I have known of the concepts and techniques behind both CNC operation and production for many years. I know how a toolchanger works, I know how a touch probe works and how it can produce a "point cloud". I understand the concept behind linear and rotary encoders, and have a reasonable, if not exactly conversational, grasp of the differences between a stepper and a servo.

But that's like knowing the concept behind a jet engine and how ailerons work. Doesn't mean I know how to fly the plane. :D


There is a reason there are designers that CAD parts, and CNC operators that CAM the parts...completely different animals.

-Yep, and I'm a one-man shop that doesn't have that luxury. I wear all the hats or the hats don't get worn. It's simple as that.


I am one of the "you should learn things from the inside out" people. You should learn some simple g-code and maybe write some simple programs by hand.

-And I am trying to head that way. I picked up the widely-recommended Smid book on CNC programming, and have been trying to chew my way through it.


I know your doing this for a business, so "dont have time to piss about" but then like someone else said, you should have bought a running machine[.]

-If I could afford a running machine, I'd have bought a running machine. At the moment I don't have that luxury either.

Doc.

Doc Nickel
12-18-2016, 10:54 PM
Okay, 1" bar, zero at the corner of the work.

G94
G18
G20
G91
S500 M3
F30
G01 X-.5
G01 X.55
G01 Z-.050
G01 X-.55
G01 X.55
G01 Z .05
M8
M30

Save as a text file, rename as .tap, should face fifty thou off the end of the bar.

I'll give it a shot! :D


heck, I'm seriously thinking about going to look at this since I will have almost that much into mine when done.

-If that showed up up here, for that price in that condition, I'd have it in my shop and plugged in within 24 hours. I'd probably have to hock a kidney to do it, though. :D

Doc.

rubes
12-19-2016, 05:02 AM
I need the practice on both the CAD and CAM. Even if I don't have a machine to run the drawings on, I still need to, you know, actually DO it.
Doc.

yeah, I get it. just that it seemed like it was "getting in the way" of progress at this time. I think you can look at it like two separate entities (machine w/control software, and CAD/CAM) that can be learned separately...with the bridge in the middle (post processor) being something that glues them together and learned later. even then...the CAD and CAM can be broken up into separate learning paths too. There are interactions between all of them of course.

I think you are using the best tools available at this time too...Fusion with its built in CAM.

You've done a nice job on the machine...keep at it.

Doc Nickel
12-19-2016, 06:41 PM
I think you can look at it like two separate entities (machine w/control software, and CAD/CAM) that can be learned separately.

-To be honest, at the moment I have to think of it as about five separate entities. :)

CAD, which I basically never did, apart from a Sketchup trial back in 2013, until I loaded up Fusion last year. Basically learning that from scratch.

CAM, which I never did until about five days ago, and really hadn't even read up on. Learning that one from scratch, too.

Post-processing. Again, started from zero just a few days ago.

Then there's the machine controls- getting Mach configured, installing requisite hardware (spindle sensors, limit switches, etc.) and making sure the machine itself works properly before I start trying to throw programs at it. (Or more programs, anyway. :) )

And then there's the actual loading of a program, testing/"cutting air", selecting tools, setting zero, etc.

Yes, it's all one workflow, but it's easier for me to treat it as discrete steps.

Doc.

rubes
12-19-2016, 09:50 PM
As they say...you eat an elephant one bite at a time...I sure hope you're hungry...hahaha

Doc Nickel
12-22-2016, 05:20 PM
Here is your simple facing cut that you tried to do with the wizard. It is stripped of everything but the basic moves. copy it into a text file, name it with a .NC (or maybe Mach3 uses .TAP?). then jog the tool to the corner of your 1 inch bar and run. Of course as usual, you should do it in "air" before committing to tools and material just in case.

-Thanks Rubes, that worked perfectly. 30 IPM was a bit fast, but of course easy to change. It also showed me I had the coordinates set backwards on both axes, even though I know I checked those at least three times. :D

That buddy of mine came over and had helped me set the motor parameters- so that when Mach 3 thinks it moved an inch, it actually moved an inch. (Before it's read out that it'd moved like 2-1/2", when in fact it'd moved about 1/2".) At that time he tweaked a few other things, including remapping the keyboard arrow keys (which I knew needed to be done, I just hadn't read far enough ahead to set them) and I think he may have reset the "+" and "-" values on the axes at the same time.

No biggie, easy change, and once properly set, your little snippet worked perfectly.

With that, and with some other sources, I was also able to successfully make a straight-edged version of the "wasp waisted" test piece I mentioned earlier. I still need a lot of practice in order to make a proper "run day-to-day" code, but it got me started. :D

Doc.

Sparky_NY
12-22-2016, 05:31 PM
Glad to hear you made progress Doc.

DICKEYBIRD
12-22-2016, 06:13 PM
I was also able to successfully make a straight-edged version of the "wasp waisted" test piece I mentioned earlier. I still need a lot of practice in order to make a proper "run day-to-day" code, but it got me started.Yay, another CNC lathe makes chips! Paul's got his ORAC running, you're getting there with the Logan...sa-weet! Congrats!:cool:

rubes
12-22-2016, 06:41 PM
-Thanks Rubes, that worked perfectly. 30 IPM was a bit fast, but of course easy to change. It also showed me I had the coordinates set backwards on both axes, even though I know I checked those at least three times. :D
Doc.

Hey, that's great...glad I could help just that little bit. So now if you try it without the G94 (thanx to Sparky for that), it should prove that the CAM was creating code with feed per rev rather than feed per minute. You can then search that out and disable it in the CAM portion of your 7 course elephant meal...hehehe.
Sorry 'bout the feed speed, it was just a wild ass guess.

rubes
03-30-2017, 07:40 PM
Sooo...Whats up Doc?
How goes the conversion and CAD CAM education?
Would love to hear ya got the machine running and making at least simple parts.

DR
03-30-2017, 08:46 PM
.................................................. .................................................. ............................................

So I've just spent six months and over a thousand dollars building a lathe I can't use unless I hand-write a program in a code I don't know?

Doc.

In my experience it is not wise at all to run programs if you don't know Gcode. Gcode is actually very easy to learn. There are only four basic motion instructions G00, G01, G02,03. It's just that simple.

With fusion it's possible to find a post processor near what you need and modify it, but how will you know if the result is right or how to fix it if it's wrong?

Post your drawing, I bet any number of us on here could hand code it in minutes and explain what we did.

Have any teenagers nearby, they learn this stuff so fast it'll surprise you?

DR
03-30-2017, 09:17 PM
So take ALL that out of your equation!!!! If you couldn't get a simple facing cut code to run, that was generated by the wizard within MACH...why the heck are you complicating things with CAD, CAM and PP's already!!
I hope your not one of those people that thought that once its in CAD that you can just "press a button" and the machine somehow makes the part? There is a reason there are designers that CAD parts, and CNC operators that CAM the parts...completely different animals.

I am one of the "you should learn things from the inside out" people. You should learn some simple g-code and maybe write some simple programs by hand. Here is your simple facing cut that you tried to do with the wizard. It is stripped of everything but the basic moves. copy it into a text file, name it with a .NC (or maybe Mach3 uses .TAP?). then jog the tool to the corner of your 1 inch bar and run. Of course as usual, you should do it in "air" before committing to tools and material just in case.

G18 (select XY plane)
G20 (select inch mode)
G91 (switch to relative coordinates)
S500 M3 (set spindle to 500RPM, start spindle)
F30 (set a feed rate of 30ipm)
G01 X-.5 (move from current position to .5 inch in negative X, toward back of lathe)
G01 X.55 (return to original position plus a little to clear the part)
G01 Z-.050 (move over .050 inch toward the headstock from the current position)
G01 X-.55 (move from current position .55 inch in negative X, toward back of lathe.)
G01 X.55 (retract back out)
G01 Z .05 (return to the original Z position that you were in before running this)
M8 (turn off spindle)
M30 (end of program, rewind and reset modes)

OT...after all the years on this forum, I never realized we cant attach files???

I know your doing this for a business, so "dont have time to piss about" but then like someone else said, you should have bought a running machine ;)
heck, I'm seriously thinking about going to look at this (http://chicago.craigslist.org/sox/tls/5923144018.html)since I will have almost that much into mine when done. But then again, you run into the post processor problem for that controller.

Do you need the G18 on a Mach lathe control? Usually lathe controls won't accept a plane select since there's an assumption of only one plane.
It's good practice to rapid G00 to a position off the part's blank. Some controls won't allow a feed move until both X & Z have moved, others require the first move to have both X & Z movement..
Why relative coordinates? Diameter programming in absolute coordinates is much easier to understand. G90 and G72. Most all our measuring of round parts is by diameters so it makes life easier to program that way too.

This is a good example of why reading about programming can be confusing, we both have different ways of (hopefully) arriving at the same result. My way is based on 30 years on 4 different lathe controls.


On edit: here's the way I would program an end facing operation of a 1" bar.

G70 G72 G90 G95 (this line might not be required)
T1
M03 S500
G00 X1.050 Z0.0
G01 X0.0 F.010 (feed per rev, might have to be changed if no spindle encoder)
G00 1.050 Z1.0
M30

I've assumed a few things are defaults in the setup of the control, but if they aren't they could be inserted as the first line, Inch mode G70, diameter programming G72, feed in inches per rev G95, absolute mode G90. I believe the G95 will require a spindle encoder.