Controlling/varying the stepover of multiple radial cuts when using single form thread mills in F360?

[t.g.mandel]

I will be experimenting for the first time cutting threads in aluminum with a small single form thread mill and 2.2Kw high speed spindle.

In preparation, I have modelled my own tool and have modified the feed rates and pitch diameter offsets using some great resources offered by NYC CNC. I also noticed manufactures recommending multiple radial passes, but varying the tool engagement for each pass given the triangular shape of the cutter (i.e., 1st pass 50%/2nd pass 30%/3rd pass 20%).

I want to use multiple varying radial passes, but in F360 I only see the option to choose multiple roughing passes at the same stepover, and the option for a final spring pass. 

Is there a way for me to program multiple passes but with decreasing stepovers?

I understand that too many shallow passes can decrease tool life, but I want to balance that with the force limits of my small tool and spindle.

Any suggestions and insights are appreciated.

Tom

[seth.madore]

No, variable depths of cut are not possible in Fusion at this time (or have they ever been). This is something we've discussed solving, but it's just an idea at this point.

That said; aluminum? You aren't going to have any tool wear unless you manage to weld the material to the tool. Aluminum and carbide are good friends, provided there's some lubrication to keep the heat down

[t.g.mandel]

Thank you for the confirmation.

I have a 'somewhat' related question that will highlight my current inexperience with F360 CAM, and is something I have always been unsure about.

For my M6 thread I programmed my thread mill with a 1 mm thread pitch (TP) and a pitch diameter offset (PDO) of 1.1557 mm. Am I correct in that the thread depth will be PDO/2 or 1.1557/2 = 0.5779 mm. And if my pilot hole is 5 mm in diameter, then the total thread cut width would be 5 mm + 1.1557 = 6.1557 mm?

What therefore are the differing results if I choose to have:

1) no multiple passes/stepovers?

2)  1 stepover @ 0.5mm? (total=0.5mm)

3)  4 stepovers @ 0.5mm? (total=2mm)

4)  4 stepovers @ 0.05mm? (total=0.15mm)

Does F360 give an error if the stepovers surpass what the TP/PDO values call for?

If the total stepovers I program are too small, does the last pass make up the difference called for by the TP/PDO values?

Hopefully my examples and questions make sense.

Tom

[seth.madore]

The Pitch Diameter Offset is the difference between Major and Minor, no other math is factored in, as Fusion automatically divides by 2 for you.

Major: 6

minor: 5

PDO: 1mm

Your stepovers are calculated back from your (background calculated) Pitch diameter offset. It will only give you as many passes are possible before the toolpath collapses in on itself. There will be a warning if you've defined more passes than are possible, but the toolpath will still run with as many passes as it can fit

[t.g.mandel]

Thank you again for the clarification. I used the NYC CNC 'thread mill calculator' spreadsheet to determine a modified PDO. Just to further clarify then, if for example I purposely choose one stepover that is less than half the radial depth of cut required, then F360 will use the remaining depth of cut for the final pass? I ask because would this not be a way of getting/forcing at least two different radial cuts/stepovers (the first larger, the last smaller) - which is the goal and the main problem I was trying to solve.

[a.laasW8M6T]

FYI, you can easily do M6 in one pass, no need for multiple cuts or spring passes, especially in aluminium.

I machine M6 in hardened 440C Stainless in one pass

[seth.madore]

---

@a.laasW8M6T wrote:

FYI, you can easily do M6 in one pass, no need for multiple cuts or spring passes, especially in aluminium.

I machine M6 in hardened 440C Stainless in one pass

---

With a desktop mill? 😉

But yeah, I do same in stainless, with sometimes a spring pass

[a.laasW8M6T]

oops missed that part, maybe not haha, still given a nice slow feed rate it should be fine.

[randypetrongelli]

Would be really nice if they could implement this, specifically for dovetail cutters, which the stepover should be decreased for each successive pass, as the engagement increases...

[seth.madore]

I'm not aware of any near term plans to implement variable stepovers, sorry to say.

[randypetrongelli]

Thanks Seth 😞
Usually it doesn't matter too much, but I'm cutting some pretty hard Rc40-43
I suppose I can each pass it's own op 😞

[jonathanBUCVS]

I just ran into this myself with chamfer / dovetail style tools. I worked around it, so just adding another voice to the "would be nice" count.