HSM in the real world Is it more than tool life? calculators that comp for thinning

Trying to analyze a few things. I am trying to first find a decent and free-ish calculator that properly assess chip thinning and or HSM techniques.

Further, I realize the very first thing to realize is better tool life BUT, I also want to know about cutting times, MRR, HP requirements, etc.

I have heard plenty say they have saved soooo much time with reprogramming but I also might call into question the prelim program and how good it was. Where was all this time gained?

I realize we get to increase feed to comp for chip thinning but are we now getting better in^3/HP? Does it take more or less thrust? Can we also increase the SFM?

What I have to question is a slower machine that can't move at 3000ipm, taking 500 nibble passes and having to walk all the way back to start each time. Does it still work out?

I really like the calc done by kennametal but does not have functions for chip thinning.

huleo,

Not free-ish (don't know you limits on that), but would suggest a look at HSMAdvisor...it seems to cover most, if not all of your concerns, plus plenty of extra reference material.

We just invested in lifetime licenses and have been pleased with the results so far. There is a 30day free trial. If you search here on the forum you should find plenty of remarks about the software.

Advanced CNC Speed And Feed Calculator - HSMAdvisor

HTH
Fred

huleo said:

Trying to analyze a few things. I am trying to first find a decent and free-ish calculator that properly assess chip thinning and or HSM techniques.

Further, I realize the very first thing to realize is better tool life BUT, I also want to know about cutting times, MRR, HP requirements, etc.

I have heard plenty say they have saved soooo much time with reprogramming but I also might call into question the prelim program and how good it was. Where was all this time gained?

I realize we get to increase feed to comp for chip thinning but are we now getting better in^3/HP? Does it take more or less thrust? Can we also increase the SFM?

What I have to question is a slower machine that can't move at 3000ipm, taking 500 nibble passes and having to walk all the way back to start each time. Does it still work out?

I really like the calc done by kennametal but does not have functions for chip thinning.

Click to expand...

It won't allow you to increase the MRR the machine is capable of; horsepower is still horsepower. It will often let you drastically increase SFM, and allow you to apply that horsepower in scenarios that weren't possible with traditional cutting strategies.

HSMAdvisor (standalone paid app) or FSWizard (free online web app) are both good places to get started.

I second and third HSMAdvisor and FSWizard.

I use hsmadvisor too totally worth it i actually pay the program with the time gain on the first job i run with it.

Its not always about horsepower its about how you use them if you got a big slow ass cat50 you better take a big cutter and remove more material.

But in my case my sloppy 7.5 hp toolroom milling taking smaller step over and increasing the feed save me alot of time and tool. You dont need lightning fast machine mine is 400ipm max travel speed but you actually never reach this. With my 8k rpm i rarely go over 200ipm. I got a video on youtube using hsm in ss. Machine is not worth 200k but can still remove material fast.

I personally think that HSM is making smaller machine shine more than the bigger boy. But its the futur in both case. Thats my 2 cents

Volumill has a free calculator. They just want to know who you are and its yours.
Download the MillingAdvisor Desktop Version | VoluMill?

rlockwood said:

It won't allow you to increase the MRR the machine is capable of; horsepower is still horsepower. It will often let you drastically increase SFM, and allow you to apply that horsepower in scenarios that weren't possible with traditional cutting strategies.

HSMAdvisor (standalone paid app) or FSWizard (free online web app) are both good places to get started.

Click to expand...

That is actually a very good description! I am going to steal it for future use.

I just want to add that i lately tend to use low TEA (tool engagement angle) milling for micro-machining.
I get a lot of parts with really tight inside corner radius(stupid stuff like 0.5mm corners 0.3" deep) and using Mastercam's Dynamic milling on those is a great time and tool life saver.

Still a 1/2" 4 flute HP endmill beats a 1" 3 flute R390 indexed cutter 3 to 1. All depends on the geometry, of course.
Generally If you are able to take >1.5x dia (>2x dia preferred) DOC, HSM machining is the winner.

zero_divide said:

Generally If you are able to take >1.5x dia (>2x dia preferred) DOC, HSM machining is the winner.

Click to expand...

This is what I'm slowly convincing the other guys at work about. Next I have to get them to buy their own damn license of HSMAdvisor!

huleo said:

Where was all this time gained? Can we also increase the SFM?

Click to expand...

There are 2 things I think are important to the time gain... Surface Speed. You are only in the cut for a short amount of time per revolution...
That allows the tool to cool, but more importantly I think, it doesn't allow the chip to build too much heat... You can really get stupid on the
surface speed. Think up towards and over 1000sfm in mild steel, 8-10k rpms on a half inch endmill in steel, I've ran 800plus SFM on
4340 at a 39C and the cutter last for hours...

Take that same high SFM and try running a slot where the tool is in the cut 50% of the time... The chip has 5 times longer to build up heat, you
will get a red hot molten pile of goo and a broken endmill. You have to back the SFM down to a point that you aren't melting the chip.

The other thing, touched on already... It allows you to take a smaller, lower dollar tool and pull down big HP #s with it. A half inch endmill with
A narrow and deep engagement, high SFM can pull a 15 to 20 plus HP cut in a mild or alloy steel... Using a conventional approach of shallow and wide, you'll bust or
melt your endmill before you approach that kind of metal removal.

What I have to question is a slower machine that can't move at 3000ipm, taking 500 nibble passes and having to walk all the way back to start each time. Does it still work out?

Click to expand...

The HSM technique of deep and narrow works awesome on rigid big fast machines, but where it really shines is on low HP floppy machines... I've got a 1978 Wells Index out here
with a Bandit control, 2HP, and I've got her tweeked to be able to rapid at 100ipm... HSM techniques on that thing are the way to go, of course you need to back figure for
HP limits, but the tools last and it'll move material as fast as 2HP will move it. I figure 1.4 cubic inches a minute in alloy steels, and about 1.7 in mild, it'll pull 2, but after a while
the spindle starts to bog.

OK, starting to make sense. I still need to run some numbers to consider thrust loads but obviously if this technique does in fact reduce thrust loads for a given HP range, that would be a big deal. I run some of the paths but never really sat and ran all the numbers. I usually just calculated about .001 fpt for chip thinning and 20% boost in SFM. Can probably push further.

Better tool life, faster machining time, less cutting forces meaning less HP required and less shock on the tool and more accurate parts from less tool deflection - HSM is basically an important advancement to CNC machining. If not for the cost of the CAM, most people should be HSMing. But there are so many types of HSMing depending on the software vendor. Its not all about radial chip thinning with helical and trochoidal toolpaths. Some will rough out most of the stock with plunge milling first and then goto helical toolpaths radial chip thinning strategies. So loads are different in those cases with plunge milling a primarily axial thrust action on the spindle and tool.

Bob is correct. Small radial cuts can really increase the sfm. Here's a video of me using a 3/4" endmill in 4340 HTSR. I was running about 900 SFM with a .0075 per tooth feed. Endmill was still in good shape after 2 of those parts.
https://www.youtube.com/watch?v=vy7A4tqredU

I was with you right up until "less hp required". That is the part that does not make sense. You are basically trading off thrust and increasing torsion to the tool. Chip thinning can be calculated, I am still unsure if there are hard figures for SFM, probably more of an estimate and trade in tool life. Ultimately though, HP is HP, Which is "the measure of work being done"....

Now, being a calculating guy, I realize and was hoping for some better explanation similar to band sawing off material. It takes less time and power to chop off 200lbs of material than it does making chips out of 200lbs of material. But, we are still making chips.

I guess the other factors to look at is the extra rapid and Z down time. As well, some older machines (we have some), can only handle so much feed and do not have look ahead but I guess you gotta get smart with the programming and not try to use HSM at 200ipm in tight corners.....

It doesn't consume "less" horsepower. It lets you maximize an endmill's full cutting potential. So that 1/2" endmill that's about to break in half during a 3-4hp slotting cut, can be used in an HSM strategy, but instead can be loaded to 15hp...

The real gains come from...
1 - Calculating for the corrected chip thickness. This yields higher feedrates vs. conventional milling strategys.
2 - Because each tooth spends less time in the cut, (which equates to more time generating heat,) the tool runs cooler in a low-radial width of cut, verses a full-width slotting cut, for example. So now, since the tool is running so much cooler, you can CRANK UP the surface speed and still be within safe cutting temperatures.
3 - Since we've cranked up the surface speed 2-3 times, we have to increase the feedrate to keep that same chip thickness. This is where feedrates get crazy impressive.

Here's just one example... (On a badass machine, no less...)

huleo said:

Trying to analyze a few things. I am trying to first find a decent and free-ish calculator that properly assess chip thinning and or HSM techniques.

Further, I realize the very first thing to realize is better tool life BUT, I also want to know about cutting times, MRR, HP requirements, etc.

I have heard plenty say they have saved soooo much time with reprogramming but I also might call into question the prelim program and how good it was. Where was all this time gained?

I realize we get to increase feed to comp for chip thinning but are we now getting better in^3/HP? Does it take more or less thrust? Can we also increase the SFM?

What I have to question is a slower machine that can't move at 3000ipm, taking 500 nibble passes and having to walk all the way back to start each time. Does it still work out?

I really like the calc done by kennametal but does not have functions for chip thinning.

Click to expand...

.
1) i just plug formula into excel and it calculates for chip thinning in a millisecond. learn to use excel for math formulas. usually takes about 1 minute to enter a math formula
.
2) yes side milling you can increase sfpm often as much as 200% compared to slot end milling
.
3) yes some cutters are more energy efficent that is cut more cubic inches of metal with less hp. often you can go from 0.8 cubic inches per hp to 1.6 cubic inches per hp in 1018 steel by changing cutter type and changing from slot end milling to side milling at high depth
.
4) you can also use chip thinning with a facemill where inserts are at low angle to face. often called high feed facemills but the are limited to low depth of cut
.
5) most things depend on part shape. many people are not working with simple cube parts.

huleo said:

I was with you right up until "less hp required". That is the part that does not make sense. You are basically trading off thrust and increasing torsion to the tool. Chip thinning can be calculated, I am still unsure if there are hard figures for SFM, probably more of an estimate and trade in tool life. Ultimately though, HP is HP, Which is "the measure of work being done"....

Now, being a calculating guy, I realize and was hoping for some better explanation similar to band sawing off material. It takes less time and power to chop off 200lbs of material than it does making chips out of 200lbs of material. But, we are still making chips.

I guess the other factors to look at is the extra rapid and Z down time. As well, some older machines (we have some), can only handle so much feed and do not have look ahead but I guess you gotta get smart with the programming and not try to use HSM at 200ipm in tight corners.....

Click to expand...

It does require less HP in general. But first, lets recognize its hard to compare apples to apples and not apples to oranges. There are so many variables for each case: HSM and non-HSM. With non-HSM you can use a full face width cut or partial. You can play with the depth of cut. With HSM you can use the entire length of flutes, you can also use more or less of that. The amount of radial engagement into the material can be changed also. All of that stuff affects the forces exerted on the tool. So how can one come to an apples to apples comparison with so many variables?

Its hard to calculate machining parameters because there are so many variables which need to be listed. Most of this can actually be observed though via how much power is drawn to the spindle during the machinig process.

HP is a measure of work done. RPM & torque. So basically it comes down to reaction forces back onto the tool due to cutting forces as most spindles operate on constant RPM mode.

In non-HSM with a full face width of cut but lower depth of cut, you have a certain force profile on the tool. You can model this as a distributed load acting tangentially in the radial direction with higher forces on the outer radius of the tool and zero radial forces at the center of the tool, and forming a 'triangle' like distributed force profile.

With HSM and low radial engagement chip thinning cuts but using more length of flutes, you generate another force profile. You can model this as a 'line' force because the distributed loads only act on a small portion of the radius, and this force is also tangential but only exists at the radius of the tool.

So you calculate to see which one yields less forces, and that is the one that uses less HP. Heres the thing, depends on how you program the cut. You can't make apples to apples comparison. But we do know this though, most normal machining parameters for non-HSM are say less than 10% radius depth of cut and less than 70% radial engagement. For HSM, you can tailor this in the programming so that the HP of the motor can make the cut. You can lower or increase the chip thickness and chip load on the tool as necessary.

Finally I want to address internal corner features. With conventional non-HSM milling, you will have low cutting forces and then suddenly dramatically go higher at the corners. THis is sometimes what causes tool failures too. With HSM, you can fight the corners by recessing it while keeping the chip load constant and manageable. In this example, HP required on the corners are definitely less with HSM strategies than conventional non-HSM.

MRR is dependent on sharpness of the tool. A blunt tool will easily require 2X or greater hp for the same cut. That's aside from the added vibrational issues. HSM utilizes the entire flute, so the wear is spread evenly, and with the right parameters, the flutes stay sharp longer because the cutting edge isn't reaching the same temperatures as when you were burying the cutter at 2/3 to full slot stepover. So HSM definitely gives you higher MRR per hp indirectly by keeping the cutter sharper. It's less noticeable on a brand new cutter, but certainly noticeable as it gets used.

By not burying the cutter, chip evacuation is improved. This means you can use 5 and 6 flute cutters where you previously would have had to get by with 4. You can use the extra flutes to your benefit by increasing feed rate, seeing in improvement in tool life (wear is spread over larger # of flutes), or a combination of both. A 5/6 flute cutter is also more rigid than an equivalent sized 4-flute due to larger cross sectional area, so you can get by with slightly increased length to diameter ratios.

If you're willing to take a slight hit in productivity, you get process reliability that is pretty much unachievable with other methods. Tool life can increase exponentially as you back off the radial DOC. We regularly have cutters lasting 400+ minutes (time in the cut) cutting steels and iron at full axial DOC (1.25 to 1.625"). This is what keeps our machines running at night. The cutters never actually break and the flutes rarely chip, which make them excellent candidates for resharpening.

Jashley73 said:

It doesn't consume "less" horsepower. It lets you maximize an endmill's full cutting potential. So that 1/2" endmill that's about to break in half during a 3-4hp slotting cut, can be used in an HSM strategy, but instead can be loaded to 15hp...

The real gains come from...
1 - Calculating for the corrected chip thickness. This yields higher feedrates vs. conventional milling strategys.
2 - Because each tooth spends less time in the cut, (which equates to more time generating heat,) the tool runs cooler in a low-radial width of cut, verses a full-width slotting cut, for example. So now, since the tool is running so much cooler, you can CRANK UP the surface speed and still be within safe cutting temperatures.
3 - Since we've cranked up the surface speed 2-3 times, we have to increase the feedrate to keep that same chip thickness. This is where feedrates get crazy impressive.

Here's just one example... (On a badass machine, no less...)

Click to expand...

There are too many variables so apples to apples comparison can't be done as a whole for all possible scenarios. This isn't a mathematical proof with absolute universal truth to it. But HSM does consume less HP in some situations definitively and that is fighting internal corners with helical cuts to recess it back before doing a final profile op. With conventional non-HSM tool paths, those corners will have higher cutting forces because the end mill cuts in more directions right at the corner. This means higher HP required at that point and more power drawn. With HSM toolpaths that will thin out and recess the corners with helical cuts, you keep HP constant or low, and even as you do a finishing profile op on that corner, there is also less material and thus less HP used.

Jashley73 said:

Here's just one example... (On a badass machine, no less...)

Click to expand...

Just watched the video. That is pretty badass.

K, not to be an ass but over a minute to make the entrance hole???? Um, drill it??? Machine probably has TSC too. That is a 20 sec op.....