helical spiral into a hole

[maker9876]

10mm flat end mill

3D adaptive clearing

helical ramp

With helix set to 9.5mm maximum and 1mm minimum, the toolpath will spiral into a 15mm hole, but not a 14mm hole.

How exactly are the boundaries of the possible calculated?

[LibertyMachine]

Screenshot or share file? 

To share: File > Export > Save to local folder. Return to thread and attach .f3d file

[HughesTooling]

It works for me so do you have stock to leave or the minimum cutting radius set too big.

Mark

[maker9876]

In the attached file the Adaptive toolpath spirals satisfactorily down into the very bottom of the hole because I increased the diameter to 15mm.

It wouldn't spiral into the hole when it was 14mm? (just modify the drawing in the CAD)

[HughesTooling · Accepted solution]

Setting the tolerance on the Passes tab to 0.01mm makes it work.

Mark

[HughesTooling]

Setting the geometry tab like this works with the tolerance set to 0.1 so it looks like the rest machining is affecting it as well.

before.png

Mark

[maker9876]

So it does. Thank you!

This tolerance feature seems to be a fix all in many situations but I don't understand what it's doing, nor why it should have problems with a perfect circle?

Whilst we're at it the "additional offset" feature in the Machining Boundaries tab of the 3d Contour Toolpath is also a bit of a mystery. And I worry it might somehow affect the dimensions of the part.

[maker9876]

Having just milled the part notice there's a problem with the contour toolpath as well. It's broken into fragments.

Have tried playing with tolerances.

Earlier this file was working perfectly with different dimensions for a different bearing (it's a mount) and produced a number of parts.

[HughesTooling]

---

@maker9876 wrote:
So it does. Thank you!

Whilst we're at it the "additional offset" feature in the Machining Boundaries tab of the 3d Contour Toolpath is also a bit of a mystery. And I worry it might somehow affect the dimensions of the part.

---

The boundary setting will not affect the size of the part it only restricts what the tool can machine. For pockets you'd normally use inside or centre and for bosses outside with maybe an extra offset so the cutter has room between the outside of the part and the boundary. Take a look at the attached file, I've setup some ops using the three different offset and a ball nosed cutter.

Tool outside.

before.png

Mark

[HughesTooling]

Which toolpath\op is the problem, the 3d contour? If I was making i'd use a 2d op like circular or bore.

Just took a look at the 3d contour and setting the additional offset to 0.01 is the problem. You have tool inside then an offset in of 0.01 so in the floating point math fuzz the op is only seeing parts of the surface. You would be fine using tool center with a end mill and the job you're machining.

before.png

Mark

[maker9876]

Yes!

I was just in the process of noticing that in all your example toolpaths Additional Offset was set to 0.

The only reason I had a number in there at all is because F360 seems to be pre-populating it of late. Setting it to 0 seems to work just fine. I'll set it to 0 in the future.

Out of curiosity tried larger values (eg 1mm) but the results didn't seem to make much sense.

[HughesTooling]

Because you have it set to tool inside you'd need to set it to -1 to make the boundary bigger, setting it to +1 will mean only the 14mm hole will be seen by the op.

Mark