I need to calculate horse power requirements for operations and am looking for material “K” factor/power constants charts, including for plastics- particularly HDPE. Can you point me in the right direction?
My (limited) knowledge is that K factor is related to metal bending.
I have cut a ton of HDPE in my day, and anything over 2hp is going to be great for you.
If you’re looking at our machines the 4hp would be an excellent choice.
In this case, “K” is a constant used to calculate the horse power requirements for removing a given volume of material at a given rate; it enables a machinist to determine the power requirements for a desired cutting rate- or, if horse power is fixed, what removal rates can be projected.
So, is a 4 horsepower spindle “an excellent choice”? Without knowing the acceptable material removal rate, there is no way of making that determination. Is the expense of an 8.5 hp spindle worthwhile? It may mean the difference between a .3 x tool diameter depth of cut and 1 x at the same feed rate. What does it take to drive a tool of any given size through what material at what rate?
The material’s “K factor” or “unit power constant” is essential to that determination, is combined with Material Removal Rate and estimated spindle Efficiency.
Here’s one primer: Back to the Charts for Productive Milling | Modern Machine Shop and another- A New Milling 101: Milling Forces and Formulas | Modern Machine Shop
In my experience Material Removal Rate is much more of a science in milling than in routing. In routing it’s a little more “seat of the pants” (at least in my experience)
To give you a little more background at how I arrived at the “4hp is excellent for HDPE”
I used to run about 4 4x8 sheets of that stuff per week, producing thousands of parts. I sourced some bits that were good for HDPE (single flute upspirals).
I did a chipload calc that got me “in the ballbark” for a good feed and speed setting to cut HDPE.
It worked fine, from there on each job I would push the cutter harder and faster until the cut quality started to fall off. Then I’d back it off a little and run with those settings. Had I stuck with the “factory” feeds and speeds I would have left a lot of speed on the table.
On my old machine I had a 3 HP router (An S30). I could push that spindle so hard I’d overcome my vacuum holding and in some cases start racking my machine (I had a non Avid CNC machine at this point)
If I had a 4hp back then I’d have had more headroom for other work like slab fattening and such, but for strictly HDPE 3hp was great.
This is all to say I think it’s good to apply some science to these decisions, but science/theory can’t replace experience. Sometimes data only tells half the story.
I appreciate all that feed back, Eric. I wonder what diameter tooling were you pushing? I aim to drive 3/4". I have access to an AVID Pro with an S30C 3 HP spindle- but am considering forsaking that spindle for either the 4 or 8.5 HP manual Hitecos offered by AVID, something like the 5 HP Hiteco with ATC, or the RM70C (7 hp ATC).
At this juncture, I’m not approaching the question from the “this is the tool I have, what can I achieve with it, creep up to max cutting efficiency” direction.
When employing long tooling (up to 7", or 9.33 x diameter) into HDPE , it may be that much of a spindle’s power capacity will go untapped. In pockets, chip evacuation may preclude deep cuts. But much of the roughing of relief carving might benefit from more power, rushing where able, creeping where necessary. I’ve seen HDPE milled to over an inch depth of cut at high speed- but with a 30 HP spindle!
Oooh I remember this conversation, now it makes a lot more sense…
I was doing 1/2" thick sheets of HDPE using typically 1/4" tooling.
I was cutting with short bits and with the spindle very close to the material surface… So pretty ideal conditions for a router designed to work well with sheet goods.
To use tooling that long there are a lot of other factors at play here… You have huge depths of cuts, super long tooling, etc.
There’s just not a lot of documentation out there for setups like this. I suspect that if you did a chipload calc for a massive 7" long bit it would recommend crazy feeds and speeds that cannot be achieved by anything other than a huge industrial machine.
I think this is very much a case of “you just gotta try it”. Sounds like you can to given that you have access to a machine with a decent setup.
If it were me, I’d see if I could source some big blocks of wood, like pine or fir. Cut them down (or glue them up) to the size stock that you’d be using for HDPE.
Mill those out and see what works. It’s cheap material so you could a lot of testing. This would help you dial in your workholding, toolpahts, etc.
Once you’ve done that you have taken a lot of variables off of the table.
You would be potentially left with just chipload/feeds and speeds to content with. You could take what you learned from cutting Fir and apply that to HDPE.
Here is a great application that calculates tool deflection and horsepower requirements for different material, bits and Feeds&Speeds. Not sure how you can take advantage of increased HP with those kind of long bits but you can pose a lot of what if scenarios and get the answer with this app .
After failing to find a plastics material power constants reference (actually, I found other folks looking for and failing to find the same thing), I came to the same conclusion: pose a bunch of hypotheticals to GWizzard. Thanks for the suggestion.
What is the cutting tool you’re looking at using? And do you have any details you can share about what you are cutting… shape, size, model, anything like that?
I’ll be press forming and annealing 80 lb blocks of post-industrial and post-consumer HDPE; the billets will measure ~14"x21"x7.5". The general plan is to face opposing sides, bringing the thickness down to 7"; some blocks will be relief carved from one side, while others will receive through holes for mounting on a vertical indexing fixture at the end of the table. The 7" stick out carbide tooling will be machined on consignment, designed for plastic, and used as sparingly as possible, with operations typically contrived to employ the shortest off-the-shelf tooling practical.
The machined blocks will interlock, constituents of monumental sculptures.
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.
Going to get this out of the way first. I don’t really like “K” factor for a lot of reasons. Most of them related to the effects of tool geometry in the real world of a cut. It can help with figuring out starting values in certain applications materials. But there are often other limitations that your going to run into first.
For the below I’m going to use Millalyzer (Link), and reference Harvey (Link for 3:1, (Link below for 10:1) and Onsrud (Link below) for chipload/SFM examples. To be clear Millalyzer doesn’t account for even close to everything and I’m just using Harvey and Onsrud’s numbers as they are fairly well know. I’m not endorsing the products or numbers.
A lot of this is going to be limited by the tool diameter and aspect ratio you are looking at. Going by what you posted (assuming that I got it correct) you want a 3/4" tool that is going to reach 7". Using the above we’re going to use the following:
Pass depth: 0.75"
Those are the converging specs from those sheets. We now need a tool to operate on this. So we’ll do 3 a generic geometry tool, a middle of the road soft material tool, and a more aggressive soft media tool. Common specs to all of them will be 9" blank, 7" flute length, 7.5" stickout, and no corner radius. What I’m changing is the flute rake, and helix.
All that was to get to here. (Had to combine these. New user limit)
If we look at this data we have the power required for those 3 tools slotting with the same chipload, of ~4kW, 3.5kW, and 2.9kW. So in the extreme case of actually being able to push your tool that’s about what you are looking at.
However, if we now look at the tool deflection we have between ~0.016"-0.023" depending on the tool. That’s not really usable so even if we have a perfectly stiff machine and the spindle power to use the tool we will have to lower the chipload, pass depth, or stepover to keep the tool from extreme chatter or breaking. You can see this in the other Harvey sheet with the 10x aspect ratio where they have lowered the chipload and pass depth to 0.0067" chipload and 0.5625" pass. Not going to go back through all of them but that puts the soft media version of the previous chart to only using ~1.1kW and reduces tool deflection down to 0.0064" (SS below. New user limit).
There are other considerations as well like machine deflection, runout, carbide grade, etc. Those will all also have an effect on the cut and how much you can use available spindle power. Not going to get into that here though.
Short version, you can’t use more than the 4hp spindle due to the tooling limitation before anything else. At least not for the preposed tool and material.
Hope that’s useful. Let me know if there’s something I can help with or expand on.
John, that was super kind of you- and useful. I reckoned the only place I’d manage to utilize significant spindle power was with shorter tooling. Just now my brain is out of spec, without a meaningful question to be found… so the most I can offer now in response is my thanks.
Here’s an idea:
Have you thought about only cutting half the depth and then flipping the part and indexing it?
Let’s say you had a tool that could cut 3.5" deep, you could face down the top, cut some features in to that face, then flip it and do the other side. That way you don’t need a 7" long tool.
I bet you could find some 3.5" reach tools off the shelf.
That might also help you avoid other issues that might come along with a tool that long like: Not being able to raise the Z enough to move in and out of the workpiece.
Flipping and indexing are great strategies, and feature prominently in my planned workflow. That said, some faces or inclusions (pockets) with draft angles can’t be addressed by flipping. My faced stock will measure ~7"x14"x21"; I plan to build a vertical indexing mount below the table to confront the 7" faces, but anticipate inclusions that may only be reached with a long tool.
No problem. If you come up with something let me know.
This could be a valid strategy depending on the tolerance needed. You are going to have the deflection offset if you don’t keep the same conventional and climb side on the flipped cuts though.
With the above, keep in mind that the deflection numbers I posted even if 100% correct for the tool you’re using are for a single tool rotation. The issue with this is that the total deflection will increase from that over time as the next rotation will have to make a cut into the deflection. Millalyzer tries to predict this but it caps out somewhere around 10% of the tool diameter. All of the examples from above exceeded the range after 4 or 5 rotations. So your total offset would be over 0.15" (again assuming the tool matched the example tool I made up).
I was kind of in a hurry to make my last post before leaving here for the day so there’s a few other things I’m going to add.
As I showed in the tool comparisons it’s possible to get less deflection with more aggressive tooling. There’s also a few other ways that you could get it down with the tooling choices.
- The first and easiest would be to look for "reach" or "necked" tooling. This is where the tool has a reduced shank after the cutting length. This leaves more mass in the tool and therefore deflects less. Here's what that looks like with the same settings except a 1" length of cut and a 0.675" neck after that up to 7".
It’s about twice as rigid so half the deflection.
There are also things like tapered cores that will increase the rigidity of the fluted section. This will almost never be listed by a manufacturer though.
The carbide grade used will also effect it. The Millalyzer examples I used above are using a Kennametal 8% cobalt I believe. However, there’s a lot of different grades inside grades and they all have different properties.
If you could find them a “chip breaker” flute would help some too. If you search for that make sure that you are not looking at a composite cutter as chip breaker is also a term for a grinding style tool originally designed for the PCB industry for FR4 .
I’ll stop there unless there’s something someone wants more info on. Let me know if there’s something I can help with.
!!! This would have been completely counter-intuitive to me, reckoning that more shaft would always equate to more rigidity!
I think there was some confusion somewhere. In the first tool examples I used they are fluted 7" on a 9" blank. In the reach version they are fluted 1" then have 6" of neck ground down to 0.675% on a 9" blank.
There are tools that are as an example 1" fluted section on a 9" blank with no neck. However, they are intended to cut no more than the fluted section and the rest of the shank used to reach into an existing pocket. They shouldn’t be used for cutting deeper or even to the edge of the existing pocket.
The reason for the above is that it’s impossible to grind a flute into the shank without slightly reducing the diameter. At least not with a real cutting flute. At a minimum you have to grind off part of the back of the flute (relief / margin) in order to keep the back of the flute from rubbing past the edge as it rotates. This means that the edge of the flute even on a brand new tool is smaller than the shank. So if you plunge past the flute even in multi-pass cutting you are rubbing the shank into the material and potentially greatly increasing the heat of the tool and material. In plastics this will often lead to melting. This is also why you typically see a worse tolerance given for tools the same diameter as the shank.