Helix machining for circular holes

[bill]

was just about to mill this part. This make it easier to plan for clamp-down of this part!

Bill, some of the vertical moves seem to be rapid moves and some seem to be normal. Can you find a reason for that?

None of the feed rates had been set; that might be why, but I have not investigated deeper; lots of furniture moving still/changes in path!

[roivai]

Found a weakness with the sorting algorithm. Luckily I had a quick E-Stop finger.

When cutting a hole where there are two different diameters at different heights at the same XY location, like one in the picture, the sorting probably picks the order rather randomly? At least in my case, it started plunging for the deeper one first..

2017-05-16-212635_3840x1200_scrot.png (49.95 KiB) Viewed 2239 times

Ideas how to modify the sorting algorithm?

[mmxe]

I did get this working and it produces very nice paths! I sent you a pm about specific implementation issues.

When clearing a circular hole, it does a helical descent, then rapids out, moves over the step width and repeats with progressively larger helices.

I'm curious if users would also like to see the alternative strategy where it spirals down a step, then spirals out to the full width, rapids back and repeats.

Is there ever an advantage of one over the other?

My guess:
End-mills generally is not made to plunge and might wear out quicker with the helical decent, so I would guess that for certain tool material combinations, the alternative strategy could be preferable.

So speed vs tool-preservation I guess.

Ugh, I just wrote an hour long response to this and the forum software made it disappear.
I'm a machinist and a mechanical engineer. I want to help make this path code awesome.

End-mills are specifically made to plunge, unless you buy the non-pluging type.

Helical descents are awesome. There's no need to rapid out of the first hole you've made. End mills are slightly mis-named. They are made to cut using the flutes too!

In fact, the most modern machining techniques attempt to use the flutes as much as possible. It's found to be much better for tool life, faster at material removal, better at avoiding tool vibration (which kills tool life and surface finish).

So we often make a pocket by starting with a helical ramp down to the depth we want to cut, which is often 1/4-3/4". Then we start making adaptive clearing passes. The goal of adaptive clearing is to avoid cutting corners as much as possible because corners force you to slow down the feed rates because the cutter engagement is going from around 10-20% to 70-100%. This is bad for speed, bad for tool life because it often induces vibrations, and bad for surface finish. If you've listened to a cutter entering a corner at high speed, if sounds like a huge bird chirp. It's not good.
Using a larger depth of cut also spreads the cutting forces along a larger portion of the tool, which makes tool wear slower and more even than if you only take for example a bunch of 1/16-3/16 inch passes. This kind of shallow step concentrates all tool wear onto the very end of the tool and a very short portion of the flutes.

Modern techniques for outer profiles often involve approaching the stock from the side with full flute cutter engagement and then cutting at a reasonable step over for that depth, then stepping up from the lowest Z level to a higher Z level. It's more efficient at material removal.

Also, rest machining is a must. The path planning software needs to know what material is left after the previous operation to intelligently plan the next operation.

Cutter compensation is essential to making accurate circular interpolation for bores and shafts.

+1 for keeping terminology consistent with the machinists world. They've been around longer than computers. Use their language for a tool build for their work.

this was all more eloquently detailed out in my first attempt.

[chrisb]

Hi mmxe, good to have you here around.
I am not a machinist and have taught machining mostly by myself. From time to time I see a friend who works in that area professionaly, whom I can ask.
So it was most interesting to read about the usage of the tools, because I often wondered why people use only the lowest end of their mills. Whenever possible - e.g. for contouring - I move the tool even deeper than necessary because the tip gets worn soon enough.

I have one further question: When using a reasonable amount of the flute, what step over precentage do you use, do you decrease it compared to milling with the tip only?

[cox]

End-mills are specifically made to plunge, unless you buy the non-pluging type.

Thanks for not letting this fine forum be degraded forever by my wild speculations

I do not know what type my end-mills are, as most come with little or no specifications from cheep online shops, any way to tell if they are the plunging type or not?

[chrisb]

Plunging types must have at least one cutting edge going to the middle. I don't know if that precondition is sufficient but I guess so. The non plunging type have their cutting edges as crown around the center. I have them only with bigger diameters.

A guess of mine is, that the plunging angle is defined by the triangle between the inner end of the cutting edges and the center. (I will try to make some photos.)

[chrisb]

Here is a photo showing a non plunging end mill:

20170525_083103.jpg (29.29 KiB) Viewed 2150 times

Plunging straight down is not possible due to the material left in the center. The dotted angle is (so my assumption) the maximum plunging angle. With this mill the tip of the triangle does't go to the center, because of the additional hole in the middle.

[herbk]

Hi Chris,
something like that we learned, but it was a "few" jears in the past and i don't remember exactly...

And like cox wrote: for the most of my used tools i don't have any specifications. If you not know which angle the tool needs, we got the rule of thumb: "3x tool diameter horizontal move per mm step down and you are on the save side".

[m0n5t3r]

Found a weakness with the sorting algorithm. Luckily I had a quick E-Stop finger.

When cutting a hole where there are two different diameters at different heights at the same XY location, like one in the picture, the sorting probably picks the order rather randomly? At least in my case, it started plunging for the deeper one first..

it would do the same without sorting

You can work around it in two ways:

• set absolute start height at zero (assuming zero is the top of your stock); this will help in other situations as well (say, you have a chamfered hole: the actual helix surface will start where the chamfer ends, I got bitten by this recently while messing around - I was wondering why the thing was plunging straight for 2mm before starting the helix)
• do two helix operations, one for the top holes followed by one for the bottom ones

As for fixing, I guess the start depth could be added to the distance that is used for sorting, I'll try it tonight.

[m0n5t3r]

Heh, looks like whoever moved the code to PathUtils missed my last fix, I was wondering why it was drilling the first hole twice again...

Pull request at https://github.com/FreeCAD/FreeCAD/pull/778