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! 
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
Thank you John. This puts into perspective some things I am aware of but don’t always take into consideration, As I look at my drawer full of broken bits.
I know what this thread is saying BUT it is hard to put into practice as a hobbyist. I think that is why CC has set up the values they have. Many are looking for the “Rule of thumb” that they can work from.
Thanks again
Glad it was useful. If I can help further let me know. Hopefully as less of text wall, but I wouldn’t bet on that.
Yeah, I agree and it was one of the reasons I put that “last note” part in. But this thread seemed to be trying to get deeper into it and the reasons behind it. Additionally, if you are getting to the edge of deflection or power you might not have a choice. I also think that even a partial understanding of pieces here (not just what I posted) can have value as it can let you make incremental improvements to your process and troubleshooting over time.
4 Likes
This topic was automatically closed after 5 days. New replies are no longer allowed.