Kmotion CNC on a lathe...

[mmurray70]

Hi Everybody,

Im thinking about upgrading to a larger cnc lathe. I've mostly been looking at running machines, but also keeping my eye open for something with electrical trouble that could be bought for cheap and retrofitted. But I had a few questions about kmotioncnc on a lathe. Mostly wondering how complete Kmotioncnc is for a lathe? Is constant surface speed hard to setup? Does the G50 max spindle speed work? Will all the lathe roughing cycles like g71 work properly? Tool nose radius compensation?

Anything else important that might be missing? I'm not really sure what else I would need, never actually programmed a lathe in G-code before. I spend most of my time by far on mills and my limited lathe experience is with Mazaks Mazatrol. I wouldnt mind learning and using the lathe specific G-codes but want to be sure all the common Fanuc functions are supported.

How many people here are using kmotioncnc on their lathes? How do you like it? Thanks.

Mark

Similar Threads:

• lathe post processor help for kmotion cnc
• Need Help!- Kmotion cnc
• KMotion CNC.net
• Kmotion disconnecting
• Need Help!- Need to know if KMotion has a Lathe Default Tool Table? Like Lathe.tbl

[Need TECH Help!]

Hi Mark,
I have a old SBL Magnaturn that uses KMotionCNChttps://www.cnczone.com/forums/dynom...-retrofit.html. There is some others that have CSS working, but i gave up on it, the machine was to tied up to keep trying to get CSS working. Currently the Fanuc cycles are not supported, unless Tom has recently released a test version. The way KMCNC is programmed is more like a mill. As it does not support certain things like tool offsets calls, like most lathes. Most lathes will apply offsets like this T101. Which is Tool1 offset 1. KMCNC lathe is like the mill M6 T1 with a G43 G0 H1 Z1. Right now i use Fusion360 to program lathe. Also have latest BobCad with lathe that works nice also.And just recently purchased Ecam https://v4.e-cam.it/, have not used it much but so far is really nice for programming lathe.You can also use it for free on the weekends.

Troy

[TomKerekes]

Hi Mark,

CSS works well. The max spindle speed is specified in the G96 D parameter. See also here.

Will all the lathe roughing cycles like g71 work properly?

No g71 is not implemented.

Tool nose radius compensation?

Radius Compensation only works in the XY plane

[Jim Dawson]

I did a retrofit on my Hardinge Conquest 42 with live tooling. Originally equipped with a Fanuc OT controller. I have to say that that a controls retrofit on a lathe is an order of magnitude more complex than a mill. There is a lot going on there, so be prepared for a project.

You only really need the rigid tapping and threading canned cycles, G84 and G32, everything else can be done from the CAM software. For the threading cycles the spindle and the Z axis need to be electronically geared together, hence the need for the canned cycles for these operations.

The canned cycles were designed to minimize the G code file size for old controllers with limited memory. Modern PC based controllers can handle a million or more lines of G code so this eliminates the need for compact files. I use Fusion 360 and have found I can easily set up any tool paths and cutting strategies needed for any normal lathe operation. The Haas Turn post works well on my lathe.

I don't know anything about Kmotion so you will have to determine if the G32 and G84 are supported.

[mmurray70]

Hi Mark,

CSS works well. The max spindle speed is specified in the G96 D parameter. See also here.

No g71 is not implemented.

Radius Compensation only works in the XY plane

Tom, Is G95 feed per rev working properly and in sync with the spindle as it speeds up and slows down with the CSS? Looks like CSS is working well in the video, but appears to be feeding the same rate throughout that video which wouldnt be good. Hard to say for sure from video though.

Tool nose radius compensation on a lathe is a little different then regular radius compensation. Its only used on tapers and arcs as cuts in the X or Z axis only will still cut to size even with a radius on corner of tool.

[TomKerekes]

G32 is supported. The Spindle must have a quadrature encoder.








G84 Rigid Tapping is supported. See also here.

[TomKerekes]

Hi Mark,

Is G95 feed per rev working properly and in sync with the spindle as it speeds up and slows down with the CSS? Looks like CSS is working well in the video, but appears to be feeding the same rate throughout that video which wouldnt be good. Hard to say for sure from video though.

Yes that should be correct. They should work independently. G95/G32 feeds synced to spindle speed. G96 CSS controls spindle speed based on X position (radius).

Tool nose radius compensation on a lathe is a little different then regular radius compensation. Its only used on tapers and arcs as cuts in the X or Z axis only will still cut to size even with a radius on corner of tool.

You will need your CAD/CAM to do this.

[mmurray70]

Ok, looks like it will do everything I need assuming I use CAM. Hand writing code doesn't seem to be an option without roughing cycles and tool nose compensation. I'll have to do more homework on lathe cam software, you never seem to see much discussion about CAM software for lathes. Most people in industry seem to either use Mazaks with Mazatrol or write code by hand. Troy that Ecam looks interesting. I might try the free weekend and see how it works.

Troy/Jim, any videos of your machines running?

Jim, Why do you say its so much harder? I cant see why it would be much different then setting up a mill with toolchanger, rigid tapping etc. What are you using for control software?

[Jim Dawson]

Jim, Why do you say its so much harder? I cant see why it would be much different then setting up a mill with toolchanger, rigid tapping etc. What are you using for control software?

Here is a really poor quality movie that I took of it making a part. But it's the only one I have. This is about the first or second part I made after the retrofit, was still figuring out how to run the machine.


There is about 3 times as many wires connected to stuff in the lathe as there is in my 4 axis mill. The amount of electrical hardware in the system can be a bit intimidating at first, there is a lot going on there. On the other hand, I have done a few mills and routers, including tool changers, but this was my first lathe. Due to the much smaller working envelope it is a lot easier to crash the machine at 400 IPM rapids and you really don't want to crash a lathe. The 1.8KW axis servos are large enough to do some mechanical damage if they get away from you. Making sure that all of the safety (machine protection as well as operator protection) systems are functional is critical.

I designed and wrote my own control software, as well as building the control system. The heart of the system is the Galil motion controller. The software was the easy part. The nice thing about writing your own software is that if you want another feature it's easy to add it. My software has all of the features that any commercial software has (and a few more) and it's compatible with a Haas or Fanuc post. And what's really nice is that I have Fusion 360 installed on the lathe computer so modifying a drawing and/or reposting the G code can be done right at the machine if desired, even while running parts (don't try this at home ).

Here is the build thread https://www.cnczone.com/forums/hardi...-software.html