Origin/consistency of chipload recommendations

This is one of those, it seems like I was right, but I’m probably not, moments. Your question has really got me looking into this, and it seems like I am completely wrong. I’ve asked some much more seasoned machinists than me, and they say I can use the bull nose for the entire operation. I’m definitely going to try it out the next punch I have to make. It also appears that bull nose tools are recommended for longer tool life. man, It just seemed that a sharp corner tool would cut better than the radiused corner. It looks like I am wrong on this one. You know what they say about assumptions…
Sorry for the false information. :pleading_face:

4 Likes

It’s nice when the math/theory matches reality. Thanks for looking into it and reporting your findings. :slightly_smiling_face:

3 Likes

After revisiting this topic again (I was scared because there were something like 40+ unread comments and at that point, it feels overwhelming to start catching up again), I found this comment of yours the most interesting. It seems counter-intuitive that chipload doesn’t scale linearly but it does match up with what I recently commented on another thread how most of the heat goes into the substrate, not the chips or the endmill. If the only difference is the residence time, then the slower speed must just create a situation where the heat buildup reaches a critical point and fails to produce good results in machining.

There is a heat/time factor that is neglected in chipload that matters in plastics more than in wood, foam, or metal.

What I think we are finding out in this thread is that machining is much more complicated the more assumptions you remove. Nothing seems to line up precisely and things don’t scale ideally. Kinda feels like science, doesn’t it???

4 Likes

The more discussion we have around this topic, the more I feel it’s indeed “only” a matter of how much hot material one can remove from the stock per unit of time (so MRR basically), and then there are two hards limits to do this, a min chipload below which rubbing happens, and a max chipload that one can take before it’s too much force to put on the endmill/machine.

Some may prefer to minimize forces by taking very thin cuts very quickly (i.e. use a peeler frantically), others may just decide to chop larger chunks of material at a slower pace (i.e. wield an axe) and then live with the higher induced forces by compromising on DOC/WOC, either way if you are not doing it fast enough heat accumulates and bad things happen.

Ok, that was admittedly a poor attempt at over-simplifying things :slight_smile:
I guess the real way forward is experimenting and reporting, and I still plan to do a temperature measurement campaign soon (but life gets in the way…)

7 Likes

You don’t really need to worry too much about heat accumulating in anything except the operator with hand tools. The goal with power tools should be to minimize heat unless it facilitates cutting as in classically defined (?) HSM. So, make “dust not chips”! :wink:

Its also amazing the differences in machining our desktop routers have compared to large mills. When your load sweet spots are within a few pounds, everything seems to matter.

Anyone that’s run square to 0.060rad back to back on a shapeoko should be able to tell the difference all things being same. If not, probably not pushing hard enough anyway.

5 Likes

Yup - how about milling forces on the order of 450 lbf as shown in Kistler’s video.

This topic was automatically closed 30 days after the last reply. New replies are no longer allowed.

Recent data suggests that, at least when milling Aluminum, increasing chiploads increases material K-factor (decrease unit horsepower) over certain ranges. That’s consistent with published results for 1" diameter endmills with 10s of kW spindles on machines capable of 100s of lbs average feed forces.

@Julien, It’s interesting that the finishing (WOC = 2% of endmill diameter) speeds and feeds shown below apparently don’t expect feed rate compensation for chip thinning!

1 Like

Indeed. It would be interesting to know why / whether this is done on purpose. Looking at the recommended value for a 1/4" endmill in aluminium at WOC=2%, if we were to take chip thinning into account, we would be down to around 0.0004’’ chip thickness, which is below my comfort zone, but who knows, with a SHARP endmill and very rigid machine…

This is all really good information.

However it’s been almost 4 years since this topic started.

Is there an updated/consolidated chip load / feeds&speeds calculation sheet for the more newer Shapeokos with the rigid hybrid table?

2 Likes

I guess we would need experimental data from folks who have a SO5 or HDM to see how much more aggressive how can be on these machines, but I think the answer would mostly boil down to “you can cut deeper depth per pass”: the physics of cutting has not changed, endmills geometry has not changed, and newer Shapeokos are still used with either a trim router or a spindle, so all the math around computing chipload and chip thickness still applies as is. BUT, and it makes a major difference, a more rigid machine can cope with stronger lateral forces, so it can basically cut deeper. On older Shapeokos, the name of the game was to do relatively shallow cuts with large stepover and high-ish feedrates. On newer Shapeokos, I suspect there is a different optimal balance between depth of cut and width of cut.
And since optimal depth of cut value was probably the least scientific parameter in this equation, experimentation is key (again)

When the Pro came out I seem to remember it was mentioned that one could double the depth per pass.

3 Likes

@Vince.Fab’s ProvenCut has done some of that with the machines that he has access too - including a “1500 W” Shapeoko HDM. Unfortunately, even though he likely has a pre-lock down version of the VFD and hence access to actual cutting power and torque, he apparently uses NYCCNC’s K Factors (shown in one of tabs of the SFPF Calculator) for his power estimates. Maybe if he had more subscribers (<$50/year) he would continue this worthwhile endeavor!
Others could too especially if they had access the data readily available from the VFD! :frowning:

1 Like

Usual preface, I’m with PreciseBits so while I try to only post general information take everything I say with the understanding that I have a bias.

I did the best I could to at least skim through this before responding so hopefully I’m not re-hashing much, if I do I apologize. With the limited time I had it took me a couple days to even do that. So I’m also not going to be quoting a lot in this.

To me the short answer to the increased rigidity is pick your increase. Like for like, the forces are basically cubic material removed per flute. So let’s say that we have two machines that are identical other than rigidity and one can handle twice the load. Either feed twice as fast or cut twice as deep.

It’s technically more complicated and there’s typically less added force increasing the depth if the tool has a helix. The forces also increase in different directions and by different amounts with tool geometry like helix changes too.

In theory twice as fast will increase the tool life more as you are making half the flute impacts to cut the same distance and decreasing the heat build up on the tool. On the flip side the increase in the cutting depth will give you part of that increase (half the passes) and changes the flute engagements depending on the helix (could be good or bad).

More in general to chiploads…

A lot of this is simplified, some of it is based on “best available” combined with “real world” data. I still find new information in studies and articles that makes no sense, or overturns previously held ideas in ways that do make sense. I’m also always looking for more data, so if you have any I’m open to, and interested in it. Most of this is pretty standard though.

Basically I think you were on the right path with the find a minimum chipload for a chart and work up from there. The issue is that what that minimum is gets complicated. Especially when close to deflection or power limits.

Basic Minimum
The simplified minimum for a tool (in these ranges) will depend on the edge radius of the cutter, and the material. Won’t go too far into this as you already have. The edge radius is a function of the tool grind, geometry and carbide grade used. Assuming that we can cut a chipload more than that radius the material strength and cohesion will determine the minimum by if the chip can support itself (softer, more flexible materials need a bigger chip).

Runout
Then you have runout that in multi-flute tools can add and subtract from chipload. Simplified example, a 2 flute cutter taking a 0.002" chipload with 0.001" runout will in the worst case cut 0.003" on one flute and 0.001" on the other. If runout is more than the chipload then you will cut twice your chipload on a single flute after plunge. Again simplified version, helix, exact flute/collet position, number of flutes, and type of runout changes this.

Acceleration margin
You also need a bit of margin for acceleration to compensate for direction changes (depends some on controller/CAM). Otherwise you will be under the minimum chipload potentially getting a bad cut or snapping tools.

Heat
Then as has been pointed out you have heat. While most of the good studies on it are in metal, the soft material ones seem to mostly follow the same rules. The primary source of heat being from the compression/deforming of the material in what becomes the chip. There’s also some from the contact points of the material and tool. This is effected by tool geometry as depending on the geometry you can have more or less tool surface making contact with the material per chip.

High chipload limit
On the high side of chipload you’re going until failure of the material/tool, or cut quality.

Material variations and effects are vast and more than your current chart can account for in my opinion. e.g. metal grades, wood grain, multi material composites, etc.

Tool wise you have geometry, carbide grades, and tool wear are going to change everything from tool deflection, to cutting forces, to direction of forces, etc.

Cut quality is a lot by itself and changes with material but some examples would be. Machine/tool deflection and hold down. The deflection ones are pretty easy, too much and chatter, or tool goes snap. If the material can move, the finish is going to be worse. More so if it’s a significant amount to the chipload. There’s also surface speeds and chiploads that will cut better in some materials entirely separate from the minimums.

These all affect each other, potentially more critically if we are talking about deflection or power limited machining.

Summery
To me this means circling back around to the best that can be done is to supply a minimum chipload or range. Preferably one where:

  • The material is being cut. Ideally with margin for acceleration.
  • Not melting/burning. Ideally with margin again.
  • Compatible with or without typical runout
  • Inside the deflection/power capacity of the machine/tool to run twice that chipload (for worst case runout with 2 flutes).

From my perspective this means that it will have to be limited to specific tooling as a change in geometry like rake or helix can significantly change the force, force direction, and tool deflection.

The pass depth and stepover also have to be spec’ed per tool to limit the forces from the cut. Though I’m not a fan of minimums that have chip thinning as it can lead to issues with plunges at a minimum.

I’d use pass depth as the place to establish the minimums with the margins above for different machines. Once you get to a high enough difference in deflection or power limits though the option for higher chipload may end up with better results (tool life and cut quality).

Again, I think you need broader categories or limits. 6061 is not going to require even close to the minimums of a 1000 series or a lead loaded aluminum. Balsa is going to need an entirely different chipload to Maple, and Rosewood wouldn’t be close to either. Extruded acrylic vs cast would be another good example.

Some of the other things I saw that I wanted to address.

Surface speed
RPM/surface speed gets weird. A simple explanation is that it’s how fast you are rubbing the tool and material against each other at the contact point. The higher it is the more heat at the contact points but it’s usually less than the chip forming. As the material, geometry, and edge radius changes it can have more impact to the point that you are destroying the tool or the material. With modern carbide grades where the edges can be finer, stronger, and tougher there’s a lot more room for higher surface speeds than the old days.

Related to this I find the test with HDPE interesting as the contact time with the edges is the same for both the 25K and 10K with the same chipload. I’ll consider it some more but it gets fuzzy as I wouldn’t consider a 0.002” chipload to be enough in that material without at least a modestly aggressive cutter geometry.

There is an increase in shear forces as surface speed increases, though that would be hard to test easily. Closest I can come up with at the moment would be to use a larger cutter with a smaller stepover at the lower RPM. With the right settings you could simulate close to chipload and surface speed at a lower RPM. Cutter geometry might be an additional variable though.

There are examples in non-hardening metals where they use tooling to increase the heat through surface speed to “soften” it and take more aggressive cuts. It’s dependent on the tooling and metal though (usually tooling with land and softer metals). I’ve seen some articles that it works even in hardening materials if the next flute is fast enough but with more tool wear. I have not seen that work in practice. My guess is that it’s a very narrow range with very specific geometries and machines.

Tip styles
Tip style changes depend on the geometry if they change the chipload. As an example it’s very common to see low, zero, or negative rake in a ball-nose (It’s a lot harder and costs more to keep rake in a ball). If it’s low enough relative to the rest of the tool you will have to bias to the ball’s rake.

V-tips tools are a mess as there’s a bunch of variation. A couple easy things are spade style usually only have one cutting flute. So you need to calc for 1 flute and a lower chipload if 0 helix as it has the highest forces. Anything with an “infinitely” sharp tip is not going to have that tip for very long (infinitely small is infinitely weak). That’s on top of having zero surface speed at the bottom. The chiploads are hard to generalize as part of it depends on the flute volume and tip size (exceed that and you choke the tip breaking the tool).

Last note
If you’re reading this and find it overwhelming and think that you’re never going to be able to cut anything, don’t. For the most part if you are using decent tools, of a decent size, in soft material, the margins are so big that you don’t need to worry too much. Can you get better tool life and cut quality with the above properly used, different geometries, or better runout? Yes, but it’s better to be cutting, producing, and learning than to get paralyzed by the “optimal” or “perfect”. If you are looking at smaller tooling, hard or finicky materials, then you might need to learn some of this or it might at least help to understand why things change the way they do.

Hopefully this is actually useful, not already covered, and not just depressing. Let me know if there’s something I can expand or help with.

10 Likes

Why is this topic, which has been open for 4 years, closing in 20 Hours?

I’m bad luck?

More seriously I think it just got reopened for Jay but I don’t see the usual notice for it. When I first saw it it said it had a few days left before it closed.

All threads should have a timer on them. When we see a thread pop back up without one, we turn it on.

2 Likes

John,

Thank you so much this fountain of knowledge, this adds so much to everything we’ve been discussing here. Much appreciated.

I can reopen the thread at anytime if needed.

4 Likes