TURNING - Negative-X Multi-Function Tools (Oh My!)

[spumco]

Didn't even see this preview feature until someone pointed it out in as an "Oh, by the way..."  No mention in the update blogs as far as I can see.

Just had a go in simulation.

TLDR:  Game-changer.

A single multi-function turning tool can now be used to:

• Drill
• Bore ID
• Turn OD
• Face
• Thread ID*

Just like the tool manufacturers advertise.

* - Only tool I know like this is the Iscar Picco-MFT series.  There may be others.

I can't find any explanations or documentation, so I'll post some notes from sim testing.  Keep in mind I haven't even posted a program yet so YMMV.

• Library
  • Set up 4 separate tools in a new "MFT" library so they don't get mixed up or lost in other folders
  • All have same tool number, but different offsets (depends on lathe control system)
    • T101 (Turret station 1, offset 1 for drill)
    • T113 (Turret station 1, offset 13 for ID bore)
  • Drill - pretty standard, nothing complicated here
    • May require some sort of tool offset in control based on the tool MFGR's specs for minmum hole diameter
    • Clockwise spindle
  • ID Bore
    • Square insert
    • Left hand tool holder
    • 0-deg angle
    • Clockwise spindle
  • OD Turn/Face
    • Square insert
    • Right hand holder, 90deg orientation
    • Custom holder w/0.5deg leading & trailing angles (with 0deg it drags on stock in sim)
    • Counter-clockwise spindle
  • ID Thread (for RIGHT hand threads)
    • Triangular insert
    • Right hand holder, 90deg orientation, internal threading
    • Clockwise spindle
• Operations
  • Using this order of Operations
    • Only one spindle direction change
    • After last op spindle is going in the correct direction for subsequent parting tool
  • (Spindle CCW)
  • OD Turn/Face
    • Select OD turn tool, nothing challenging to get a good toolpath
  • (Spindle CW)
  • Drill - nothing challenging here
  • ID Bore rough/finish
    • Edit Op: select TOOL / MODE / "Turn In Negative Diameter"
    • Select ID Bore tool from library
    • Inner Radius should be set to previous drilling Op diameter
    • Edit retracts, clearances, etc. until crashes go away.
  • ID Thread (for RIGHT hand threads)
    • Inside turning mode
    • Right hand thread
• Spindle winds up turning the correct direction for an subsequent upside-down parting tool

Gripes

• In negative-diameter mode, the approach & retract X is in positive values (above centerline) and not adjustable
  • Speculation: "negative diameter" is calculated/invoked after approach and before retract (only for leads and feed moves)
  • Leads to the tool crossing the center-line twice for each operation.  This is not unsafe, but annoying and wastes time/movement
  • Would be nice if the tool control point could be set to X-centerline or X-(neg) diameter + clearance for approach & retract
    • i.e. invoke 'negative diameter' mode At start of toolpath, not at start of lead-in
• Negative diameter does not appear to be available for threading operations.
  • Not sure why anyone would want this, but maybe someone has a particular tool/setup and wants to ID thread this way.
  • Seems like it should be easily added...?
• Tool library is irritating regarding the "Name" column
  • The inset designation comes first, then everything after that is usually cut off
  • Can't override or over-write the ISO insert designation with useful descriptions
• Documentation/explanations/pop-up tips for this preview feature please

Thanks to the F360 team for this.  Those of us with limited tool stations or slow tool changers can now take advantage of the wide range of multi-function tools.

[seth.madore]

Good, I'm glad that you found it and are making use of it!

[spumco]

Cant wait for you all to sneak lathe form tools in...😁

[seth.madore]

Oh man, that's very much at the top of every lathe programmers list, myself included! We are very much aware of the need for that, but I do think it's a bit far out on our timeline (sorry to say)

[Sq_14]

I need to make use of my 20mm left handed (=M4) EcoCut Multitool for outside work but i can't get Fusion to come up with a tool path in negative direction on OUTSIDE profiling.

I have the tool as a third tool number ready, spinning the other way, but If i choose OUTSIDE profiling the negative direction Box disappears and the tool path is generated and simulated with the wrong cutting edge or just works the front of the part as far as the angles allow.

What am i doing wrong here ?

[Sq_14]

that's the tool i'm using ..

[Sq_14]

nobody got an idea ?

[spumco]

I'll take a closer look later this afternoon, but I've found that you have to define multiple tools in the library to 'trick' F360 in to working with multi-function tools.

So you've got a LH Ecocut oriented in the holder with the insert on top... and you want to OD turn (M3) - is that correct?

[Sq_14]

hey, thank you in advance.

Yes, my machine is setup as you described, LH EcoCut tool, Turret is behind center(=X+ side), and i want to cut on the x- side with the spindle turning forward (=M3)

[Sq_14]

on normal operation, i have two tools in the tool table defined, X-offset 0.0 mm as T0101 for using in drill operation(my machine does not accept an offset >0 for drilling) and 10.0 mm as T0111 for boring/facing operations, both with M4. Does work very well with Fusion.

For use on outside work i defined another T0111 with x offset=10.0 and M3.

[Sq_14]

i wonder how Fusion is handling a tool path with a Post Processor for a tool room lathe (typically set up with an QCTP on X- side) such a normal tool path for this kind of machines .

Does it simulate the tool path on X+ side and negate the X values upon post processing ? 

Gotta be, since an outside tool path would never generate on the x-side... or does Fusion flip the standardized axis orientation in such a case ? 

... strange thing...

[spumco]

Ok, took me a few minutes to get things figured out but I think I've got an answer for you, even if you won't like it much.

• Go to your preferences and turn on "Turn in Negative Diameter"
• Edit your toolpaths and you should now have a "Turn in Negative Diameter" checkbox under Edit>Mode

That sorts out everything but the OD profile toolpath.

I couldn't get the OD toolpath to work below center on your model or on mine.  I've defined my tool as a RH, so my OD cuts are in X+ (not on the far side).

The problem is that if you change the mode to OD Profiling, the "Turn in Negative" option disappears.  All of the facing and ID operations can use it, but not OD.

I think you've found an F360 bug, or  - more likely - a feature that hasn't been implemented.  OD turning below center may not have even been contemplated by the F360 programmers.

Unless someone from F360 is ready fix this right now, I think you're stuck orienting the tool 180 (if possible with the flat?), or switching to RH multi-function tools.  Orienting the tool would allow you to cut below X0 on the ID in M4, and above center on the OD (M3).

Regarding the tool-room lathe or gang-tool back-tools, I think that's defined in the tool and handled by the PP.  I seem to recall the Haas post should use "Turret 0" for front tools, and "Turret 1" for back tools .  Once defined like that, the PP spits out the correct direction that corresponds with X-neg for the tool orientation.  Don't take my word on it, but I'm pretty sure that's the deal.

Or...you could get someone ferociously clever to edit your post so that if you define a tool as Turret 1 (or something other than 0) the post knows to go below center like a gang-tool lathe.  If you can edit it yourself to that degree, let me know because I could certainly use some tweaks on mine.😁

BTW... I like your machine.  I've got an Emco 325-II - you wouldn't happen to know a good place to get VDI16 live toolholders would you?

[Sq_14]

hey, thank you so much for looking into this, it confirmes what we've learned so far, Fusion isn't able to make that cut happen. Seth Madore even confirmed that in another post yesterday https://forums.autodesk.com/t5/fusion-360-manufacture/turning-profiling-below-x0/m-p/11619424/highli...

I'm thinking about rotating the cutter in overhead cutting configuration, milling or grinding the flat on the other side wouldn't be the major problem here, much more to remember the change when pulling up an older job. I might have to change the tool to another tool station and offsets to ensure incompatibly with older files, but that would interfere with my my own set of rules on how to number out stations and offsets.

I've not looked into the Haas PP much, but i think i can try to adapt something for my hacked togehter PP (which started with a already hacked PP for the TM01 control) and make  it compatible for different turret operations.

I'm a hobbyist and could spent some time over christmas and new years holidays to achieve this. It kinda frightens me to know the simulation would not represent the actual movement on the machine. On the other hand, I have some more "fusion incompatible tools" and adapting the PP would open up more options in the long run.

But there's still option 3, just hand coding this simple cut when needed. Might be the 'easiest way' now, but not helping the future.

I'd love to have a machine like your 325-II, it might be hard on the budget, but nearly impossible for the floor space i have available.

In regards VDI16, well that's a not so common size in general and even more with live tooling. I happen to live an hour drive away from Sauter, EWS and Zuern tools, but live tooling depends also on your turret.

Here's where i would look:

if you have a Sauter Turret:

https://www.sauter-tools.com/?tool__product_group=Angetriebenes%20Werkzeug&tool__shaft_size=16&tool_...

Baruffaldi Turret

https://heimatec.com/file/get/b7bec5a1-d31d-e811-8290-001c42bcb3bc/en-US

EWS has A LOT of tooling, but not cheap ...

https://ews-tools.de/en-DE/category/driven-tools/667?&search=undefined&page=1&items=10&filter=%5B%7B...

Zürn also has some VDI16 tooling

https://www.zuern-tools.de/Werkzeughalter%20DIN%2069880

I'm sure there are tons more vendors, but these four make a good starting point for exploring this VERY WIDE field of tooling options for me. If you have a specific tool in mind, i can ask a friend who is hand coding live tooling lathes at a big facility, he might be able to throw in some of his knowledge.

[spumco]

Thanks for the tip on the toolholders - I've got a Sauter turret with the DIN5480 drive.  Emco's are rare in the US, and they're presence here has dwindled over the years for some reason.  And a 325-II with live tooling...well, I'd be surprised if there are more than 20-30 working machines in the country.  So VDI16 is not something I can just pop on ebay to grab.

If you do wind up modifying your post please report back.  I'd be interested in seeing if I could incorporate something like OD turning below X on my machine.

[Sq_14]

I know EMCO hasn't sold that good in US, probably looked at 'under par' within their rather expensive price range at the time of purchase, but they are really good machines and long lasting. I'm willing to bet, most 'better' machines  from back then are into their second or even third life after being scraped.

Mine is from 1988, came originally with a TM01 control, was upgraded to a TM02 (which makes it a 242) some years later and still does a fine and accurate job. I love this machine, but I would love to have a c-spindle/live tooling machine, so much more options. If the control should break down one day, i'll upgrade it to Centriod or LinuxCNC.

Sure, i'll report if the PP adaption will happen. If at all, it'll be begining of the new year, that's for sure.

[Sq_14]

some half good news ...

I looked into the Haas PP and, after some fighting with the PP and some brute force against the PP using polar coordinate system more often than not, it seems, turning in X- and returning to X+ work with the next tool,  my modyfied PP works. 

The only thing i don't know, because i'm a G2/G3 illiterate, is if the arcs turn in the right direktion with the direction inversion the PP does. It should be fine, but until not hot tested, i'd hesitate to cut something else than air or plastic. Unfortunately, i don't have a GCode Viewer or simulator to verifiy the arc movement.

If that works in the modded PP, i'm quite confident I can transfer the related code into my PP.

[spumco]

Well done! And rather fast, too.

Shouldn't be too hard to post a little test file and run it in air to make sure G2/3 work as intended.

[Sq_14]

quick update ...

the brute forced Haas Post DOES NOT work with the classic XYZ Axis Coordinate System, i guess that's why they used polar coordinates 

In regards to inverting the values, not only the way points need to be negated, but also the called arc. I. e. a G02 must be converted to G03 during processing.

I got my modyfied PP in radius mode now up and running as it should, but it needs some clean up and i have to look into some currently not used aspects inside the post before calling it done.

For one i need to find out how to initiate a 'change tool' (better said change tool offset) when only the tool offset or even spindle direction is different to the current tool.

The function is solely based on toolnumber, but thats asking for trouble with this MultiTool sooner than later.

I.e.:

   tool as drill = turret 1 -  X-offset=0.0 = T0101 - M4

     boring bar = turret 1 -  X-offset=10. = T0111 - M4

face/outside  = turret 2 -  X-offset=10. = T0121 - M3

If anyone got an idea on how to implement this in a smart way, I'm all ears !

[tacticalkeychains]

Been using this tool for many years, I actually do this but with different tool numbers. (Gang Tool)

I'm thinking a quick edit to the post may allow us to get rid of that + move at the beginning when internally boring.

Have you dug into this anymore?  Is this something that will eventually be included in fusion?

This tool is used by many as it's a huge time saver and wears very well.