(Mill) Chip Thinning Question

[Ftoggle]

I could sit here and run chip-thinning predictions all day long... but only because I have (a really full schedule) elsewhere and what I'm actually saying is “it takes me all day and then some, most days,to get back to the same old question”.


So here's my question, because I know there are so many of you that deal with this all day long, professionally...


If I know my [milling] machine actually prefers around 150% ADOC and 25%RDOC, roughing... and let's just 'say' 12.5% RDOC at same feed

1. lessens tool and table axial loading,
2. reduces harmonic tendencies,
3. 'hints' it will improve final surface finish, but also
4. increases the onset of tool rubbing...

why doesn't a 6% RDOC, finishing, actually 'demand' a substantially higher feed rate? (or does it?)


You know what I'm saying --- and I could actually toss in the real numbers, instead of calling arbitrary/50% reductions of RDOC... but I'm sort of 'putting the question out there, as a basic abstraction'. Can anyone site meaningful examples from their experience or share their better thoughts on this?

Similar Threads:

• Problem- Thinning leather with mill?
• Sprutcam 8 - No Chip Thinning Compensation?
• Thinning acrylic solvent?
• Chip thinning strategies, trochoidal toolpaths, high-speed machining using Mach 3?

[SCzEngrgGroup]

First, you have to distinguish between roughing (where the goal is maximum MRR), and finishing (where the goal is a good surface finish). Those are two completely different situations, which require different trade-offs. Chip thinning does not exist at 50% radial engagement, and is a small factor at 25%, and starting to become really significant at 12.5%. Those are all roughing engagements. For a variety of reasons, a smaller engagement, and the higher feedrate it enables, will often allow increased MRR, while putting less stress on the machine and the tool, which increases tool life, which reduces cost. As an example, using a 1/2" HSS 2-flute in 6061, I can slot at something like 15 IPM at 2500 RPM with 1/4" DOC, giving about 1.8 MRR. The same tool at 0.05" engagement, will run 110 IPM at 6000 RPM with 1/2" DOC, giving about 2.75 MRR. At 0.025" engagement it will run 150 IPM at 6000 RPM with almost 1" DOC, giving about 3.7 MRR.

Rubbing is only an issue if you're going WAY too slow for the engagement, or you have a WAY too narrow engagement for the RPM, either of which results in a very low chipload. For finishing, you WANT a narrow engagement, but with enough engagement to avoid rubbing. This usually means a chipload on the order of 0.001",except for very small tools. You don't much care about MRR when finishing, you want whatever speed gives you the best surface finish. That will generally be at a feedrate well below what that narrow engagement would allow for roughing.

If you don't already have it, get a copy of HSMAdvisor (https://hsmadvisor.com/), and learn to use it. It will be the best money you ever spent for your machine.

Regards,
Ray L.

[Ftoggle]

Thanks for the input, Ray. I just had the chance to finish reading your post. And I appreciate your thoroughness in response to such an arbitrary or non-specific question.


I threw your numbers to the spreadsheet, one I'd previously concocted about this/my concern, and your settings 'seem to be' suggesting something else I was also originally thinking...


because, after TEA compensates your 2^nd and 3^rd examples for chip thinning (while roughing), they both come back at about 1.1% of TD as actual chip thickness; around ½ that, in the case of your 1^st example given (the one where it's running at full slot).


Don't mind me if I find that slightly confirming, at least in the case of the ½ inch EM you referenced in your remarks. The only reason I brought that point up is I tend to get very random predictions, from tool suppliers, on the rec'd chipload for a lot of small EMs; mostly because the size I'm [leaning to] hasn't even had it's ipt especially categorized. It looks almost like Vegas to me, most of the time, or like there's a size vs. geometry grinding problem going on(?)...


but then of course I slap myself in the head, reminded of how tool-size deflection drives the ipt degradation (and recommendation) on the EM downsizing.
acknowledged:“get a copy of HSMAdvisor” and comma (silent “stop struggling”)


Your last example also/kinda reminds me why I can get away with an ultra-deep but ultra-shallow width of cut on a high speed finishers square (to lift the witness marks); but mostly, your finishing reference (.001 ipt) reminds me of how I used to 'finish well' at [1/an odd prime] of the original roughing feed. 7 seems almost like overkill... but 3's just too coarse for my liking.


Again, 'rather confirming'; but yes, I accept you were being both generous and generalizing in that specific remark. Of course, thanks for 'all' your inputs; not your fault if I sound as though I might be, somehow, continually digressing.


Regards

[SCzEngrgGroup]

Keep in mind, the specific tool is a major factor in what you can get away with, but it is FAR from the only factor. There are major factors (machine rigidity, spindle power, coolant, tool stick-out, fixture rigidity, etc.), and tons of minor factors. Calculators, like HSMAdvisor, give you guidance, but cannot give absolute, bullet-proof numbers every time, for every situation. You still need to validate the numbers, and learn how to "read" the cut, to know what's wrong, and how to improve the result. Take the time to understand HSMAdvisor, and make sure it's limits are set properly for your machine, and it will quickly become invaluable.

As for the wide variance on manufacturers recommendations, some give numbers that will ALWAYS work, which means they're very conservative. Some give numbers that will only work on a very large, heavy, rigid machine with LOTS of horsepower, and a high-volume, high-pressure coolant system. You simply cannot compare numbers between manufacturers. Find tools you think will work, buy a few, and test them. Take the time to optimize each for your machine, and the kind of work you do. Find ones you like, and stick with them. Even two EMs that appear identical, can behave VERY differently.

Also, FWIW, most people seem to believe expensive carbide tools are ALWAYS better, but it simply isn't so. I do 90% of my work with HSS tools. I'll use carbide for smaller tools (under 1/4"), as carbide is stiffer, which really helps on small tools. But for roughing 6061 on machines in this class, a 1/2" 3- or 3-flute is hard to beat, and carbide has little to offer over HSS, other than higher cost. These machines don't have the RPMs, power, rigidity, speed, or coolant to get much benefit out of carbide. And using HSM, a $12 HSS 1/2" 2-flute lasts a loooooong time, and give a beautiful finish, so why spend $30-50 for carbide that doesn't work any better (and often worse, as carbide is so easy to chip/damage)?

Regards,
Ray L.

[Steve303]

Ray, can you recommend a source for the HSS endmills you use.

Steve

[SCzEngrgGroup]

Ray, can you recommend a source for the HSS endmills you use.

Steve

I've had good luck with the HSS 1/2" 3-flutes from discount-tools.com, made by Quinco, though you sometimes have to buy quite a few to get a reasonable shipping cost, as that brand is drop-shipped from the manufacturer. I usually buy 10-20 at a time, which lasts me a year or two. Discount Tools is very nice to deal with. I used to buy Putnam, AccuPro and ATrax 2-flutes from Enco, before they got absorbed into MSC. Never, never EVER buy anything Interstate brand!

Regards,
Ray L.

[Steve303]

I've had good luck with the HSS 1/2" 3-flutes from discount-tools.com, made by Quinco, though you sometimes have to buy quite a few to get a reasonable shipping cost, as that brand is drop-shipped from the manufacturer. I usually buy 10-20 at a time, which lasts me a year or two. Discount Tools is very nice to deal with. I used to buy Putnam, AccuPro and ATrax 2-flutes from Enco, before they got absorbed into MSC. Never, never EVER buy anything Interstate brand!

Regards,
Ray L.

Thanks Ray, my apologies to the OP for hijacking his thread. Do you use HSS ball endmills for aluminum as well?

[SCzEngrgGroup]

Thanks Ray, my apologies to the OP for hijacking his thread. Do you use HSS ball endmills for aluminum as well?

I would if I ever had a need to, but so far I haven't...

Regards,
Ray L.

[Ftoggle]

Ok -- so here's the second installment in my usual 'series' of questions... and of course it comes to you in the form of a screenshot,

from a spreadsheet I had open on a second monitor.

[someday maybe I'll forgive myself for thinking my age(?) warrants luxuries like multi-tasking... but that's a bit unlikely]

Have a look; all opinions are appreciated, all diversions are certainly given their due also.

[Ftoggle]

My apologies for the apparent clunky-ness... the spreadsheet was actually for myself, not for publication... and it gets a little [late and long] around here... that is to say, 'before' I can actually convince myself I'm 'allowed' to let go and go to bed. Be glad you have your own homes to go to, right?


I also wrote the [remarks] in a style that weren't possible for me to misinterpret whenever referring back to them... because I'm essentially [the one] who has to hold it all together... and I don't really have a legit [peer] at the moment to bounce the random 'what-ifs' off of. I'm sure you know how that is – a lot of people seem to have a propensity for only seeking out the receiving end, they don't necessarily wanna 'get it'. But don't confuse that for being negative, I just 'get that'... and I seem to have a chuckling propensity for telling people “but don't worry – it only 'seems' like it's tedious... but because it is”.


This particular ots version (yes, it's OpenOffice) was concocted 'only' to address some concerns I had in reference to these [relatively-expensive] and [omg suh-low] sub-4mm end mills. I'm actually, now, good at [strategizing and 'confining'] tool paths, within the CAM aspects of the software I've been using – at least for these rather small features; without any wasted motion; without any impending crashes or tool overload. But, of course, I'm always looking for a new edge, and seriously, who isn't.


As I indicated to you previously, I don't do this full time, and I'm always willing to admit I might have inadvertently 'overlooked' something. For me, that is actually a very healthy, almost zen, approach to the situation... because it's going to happen, right? Better now than later.


But the basis of it is actually quite simple – I find it much easier to interpret the effects on chip thickness from [the perspective of this simple formula]:

2x √(RDOC– RDOC²)

That's probably familiar to some of you, but of course I've reduced it; primarily because I found it too clunky in it's original Helix form. All you really have to remember when 'using it' is that RDOC must be input as the decimal equivalent of TD percentage. In other words, if RDOC equals 25% of tool_diameter, the correct entry equals 0.25 – then it just flows. Simple geometry, right? The net sum is the decimal proportion of '1' in regards to a 50% RDOC chip thickness.


In a couple of minutes, I'll probably be [running off again]... to catchup on whatever I've left undone, elsewhere, again... so, whatever I might leave [unfinished] here, all I can hope is [the communication continues to flow smoothly], and that you'll overlook any mental absences I simply haven't yet had time to address.


I will include 'one' additional statement, however – hopefully to clarify. In this sheet, the RDOC/ADOC 'ratio' updates according to a fixed-slice cross-sectional area (based on the tool data 'preliminary' specifications). This calculation 'precedes' any/my adjustments to F&S, because it was intended to 'baseline' an MRR (identical to the suppliers preliminary R/A specifications). In other words, if I inject a smaller RDOC, the sheet outputs an ADOC that holds that preliminary CS area. Enough of that.


Also, I understand – even to me, this all sounds a bit wordy; especially considering I was only trying to leverage [a deeper cut], [by spreading the tool load toward the stiffer root of the shank], [but also to speed all things up].


But I just don't know a better way to get the 'point' of the picture I'm painting across, without attempting to spell it out.


I was kinda hoping the gist of my question was properly addressed in the remarks conclusive of the JPEG paragraph 5 – but I realize we all [think] differently, at the sum level... or expect conclusions to arrive on a bit different truck, so to speak. [uhhhh... yeh]


In the end, the calculations produce a way for me to create direct comparison – between the tool suppliers 'ultimate' projections for tool MRR (as load, if the rpm were available) and the actual load and speed my machine may be capable of. That is to say, so I don't 'violate' the tool limitations, even prior to loading it up. WooHoo– yay me, right?


So if you can actually [agree or disagree] with my estimations, given the 25 days or so I'm 'obviously' comfortable with in getting back to this... (yes, it's been that long; no, I don't have a shame button),


no mistake, I am grateful. Even without 'paraphrasing' any of your prior investments to me, I have certainly witnessed the immediate value of them; I don't expect that will change.


Thanks again. And Regards.