spiral / circular interpolation on the front face of a bar in the lathe?

[safiredesignengineers]

Hi Group

is it possible to program fusion 360 using spiral / circular interpolation on the front face of a bar in the lathe?

what i need is for the lathe to rotate the bar and the machining would be by the use of a live milling cutter in the indexer and a very small cutter would start on the o/d of the part and spiral in to the centre whilst the lathe Z axis will move in and out to create a 3d feature required on the end of the bar.

is this possible to do in fusion 360?

A

[seth.madore]

Yes, this should be possible. Are you looking to machine a scroll gear or are you looking for a spiral finish?

[safiredesignengineers]

Hi yes scrolls etc but also full 3d tracing, the idea of 3d spiralling is to save time as opposed to 3d machining the face in a mill as in the lathe you only need to do one half of the part

[safiredesignengineers]

Hi Seth

I know i can run a spiral mill path which would use x y and z but the idea is to machine with a live milling cutter and use the Z axis and x axis on the lathe to do the work on the front face of a bar, so the Z axis will travel in and out and the x axis will be controlling the spiral direction.

like a vynal record playing if that makes sense..

[Anonymous]

Looking at your last two posts, I think you are mixing apples and oranges in regards to only machining half the part.

In polar mode tool only works on positive side of X axis, whenever there is negative X coordinate, C axis is rotated instead of tool crossing center line.

This is equivalent of XY, 2D machining on vertical mill but Y axis is converted to angular coordinate of C axis.

Now in reference to your last post, you cannot do XCZ machining in polar mode, it's 2D function, tool is driven in position by Z axis, polar mode is started and XC machining is executed.

If you want to do XZC machining on face of bar stock, you can do one half, rotate C axis 180 degree and do the other half.

This eliminates assumed advantage of doing only half face on lathe, plus it opens possibility of miss match due to tool deflection at start and end of connecting edges at center line.

If you are looking to face off part using C axis and rotary tool you can create spiral drive curve and use Trace.

If you want to create texture for purpose of bonding rubber element for instance, you can use chamfer mill or ball end mill.

You can also use threading cycle to create texture on part face but that would have to be done by manual program, Fusion has some restriction in terms of what can be done with certain tools.

Attached is raw demonstration of what you can do in polar mode regarding "facing only half of the part", which is also not true because you are facing entire surface by means of rotating C axis instead of tool working on negative side of X axis.

Given same parameters, your cutting cycle time would be the same on both, mill and lathe.

[safiredesignengineers]

hi Vic

thank you for your reply, the bar face will not be a flat face it will be a detailed 3d feature face like a coin face for example and it needs to be done an a lathe but rather than moving the y axis and x axis to spiral as per your sample which is effectively milling the complete surface what i would like to do is use the c axis to rotate the material precisely in combination with the x axis and the z axis, note the z will simply be going in and out as the x travels from the outside into the centre to machine the feature.

in this way there should be less machining than on a mill  as the x travel is only from the o/d to the centre as opposed to the hole circular surface.

is this possible?

i hope this makes sense....

[Anonymous]

In regards to only doing half the face on lathe vs full face on mill,.............. which half do you want to do on sample part below, half with rectangle, half with circles or half of each ?🙄

My point is, there is no such thing as only doing half the face on lathe to save cycle time, you are cutting full face on mill and lathe, only difference is in how mill-turn handles it compared to vertical or horizontal mill.

3D tool paths, XCZ motions managed by polar coordinate, just rotating C axis to keep tool on positive side of X axis.

In 2D tool paths you have choice of doing XC or ZC, tool is positioned in place, depth in Z or X axis and other two axis are driven to produce contour or pocket, in sample below tool is first positioned in X axis then Z and C axis are driven along selected contour.

In sample shown in my last post, Z axis is first positioned to depth then X and C axis are driven along selected sketch.

[safiredesignengineers]

Hi Vic

this is not about saving time or which way is better etc.., what i wanted to know is whether fusion can program a lathe in this way as i want to try something on a new lathe that has just arrived.
based on your samples (thank you for sorting  them) i am assuming it will but can fusion simulate this the way the lathe is going to actually do it, currently in your sample the milling tool moves around the bar but the bar will be spinning and the milling tool hardly moving..

A

[Anonymous]

Well I was threading on your original post and ... "only doing half the face on lathe.....", that's where we need to sort things out.

Whatever configuration you have on model, Fusion will show same simulation for mill and lathe, tool running around feature and cutting, in reality mill table is the one moving around while tool only moves up and down.

When you run same program on lathe, instead of tool crossing into negative side of X axis, C axis rotates so that tool always works on positive side of X axis, this is managed by polar mode and it's usually deceiving factor for people but is actually very simple in nature.

If you cut a slot across face of round bar and start the cut from top, tool will come to center line and stop moving until spindle turns 180 degrees, at that moment tool will travel from center line back to top of the bar or its original starting point in X axis.

As a result, there will be small tool mark where direction switched because continuous feed  was interrupted for a brief moment while C axis rotated 180 degrees. 

Same thing happens to any and all features below X axis center line on more complex tool paths and spindle will go back and forth to adjust as required, you don't see that in Fusion simulation of lathe milling, it's managed my polar mode in machine's control.

[safiredesignengineers]

thanks Vic

your input has been great and has made me think more about the new lathe and it's processes etc..  i have a lot to take in and learn now i have live tooling, y axis etc..  but i am sure fusion will be a great asset in programming it.

A

[Anonymous]

I have access to Mastercam but 90% of what I did in past 12 months is done in Fusion, I can model complex parts and program all features in one package, yes it has flaws but what in this world does not?

It's a tool, add it to your "tool box" and combine its advantages with your other options.

Forum is learning tool as well because more eyes see more options, dive in and see where it gets you.

[Anonymous]

I have to correct one of my statements above, in post showing flat and textured face screenshots, I stated that you cannot do XCZ moves inside polar mode.

That's wrong and I don't know what I was thinking at the time, in my follow up post there is a model with rectangle and circle extruded in opposite direction, clearly 3D work, so it posts as 3D work inside polar mode.

I have done enough work to know better, but there are times ........, sorry for any confusion in that regard, the rest of it stands.

Until few months ago, shop had Haas ST30SSY and Haas allows rapid moves within polar mode, while Yama lathe with C axis and Fanuc control requires me to program high feed rate moves, perhaps that got in a way.

While I am on subject, you have to know your machine's capability, then adopt post to it and program work knowing what approach is within that machines range and ability.

For instance Hyundai Wia with Y axis does not recognize "G53 Y0" as homing Y axis, I have to use "G28V0" instead or nothing moves until Y axis home green light is on.

So my turning operations start like this:

N1(FACE1)
G00G28V0.
G53X0.
G53Z-10.
G54
G99G18M40

[safiredesignengineers]

Hi Vic

thank you for your valuable feedback, i am currently trying to get a good working post-processor for a siemens sinumerik 828D on a Doosan lynx 2100lsy mill-turn lathe with sub spindle  for fusion 360.

Once i have this i can then sort out this 3d tracing problem..

A

[seth.madore]

I'm not aware of a Siemens based Doosan post. There is a Siemens Mill/Turn post available here, but it will require substantial modification for your needs.

[safiredesignengineers]

hi seth

thank you for your reply, how do i get it modified?

regards A

[seth.madore]

The generic posts are open for editing by anyone that feels comfortable taking that on. If that's not you, we do have the Post Forum where you can ask for help, or you can reach out to one of our resellers and inquire about a custom post created, tailored to your specific needs. A list is available here