Peel Mill with Seven Flute 3/32 dia. endmill in 17-4

[[email protected]]

Hi guys I don't typically use endmills with more than 5 flutes. I am cutting some 17-4 and needed a 3/32 endmill for some small features. I found some 7 flute harvey 3/32's in our shop and figured i could peel mill at full depth of .28". Does anyone have an idea of what kind of step over i could do at that depth or how to figure that out? I don't want to load the cutter up with chips and since it looks more like a burr tool than a cutter im kind of concerned. 

[crazy^millman]

1% to no more than 3% step over. Chip load .0005 to .001 max per tooth. 220 SFM if coated correctly if not then might slow it down to 110 SFM.

You know Harvey has speeds and feeds on their website? Speeds and Feeds

[[email protected]]

So please let me know if I am understanding Harvey's Info correctly. It looks like I can use an SFM of 350 to 400 depending on hardness(not sure?). .00065" chip load per tooth. and my Radial stepover must be less than 10% of Diameter(.0093 or less) when cutting at an Axial Depth of 50%(.046) to 3 times(.281) the Diameter. 

So their speed and feed suggestions seem really high on the RPM to me but I don't know....350 SFM x 3.82 = 1337 divided by .09375 = 14261.3 ! wow am i missing something?

Anyway I am going to try 5500 RPM @ 25 FEED (IPM) at a .009" stepover. Also when I click Mastercam's RCTF button it makes the feed even faster. Which I understand it means Radial Chip Thinning Factor but I am afraid to use it's suggested feed since the chip load in Mastercam will show it exceed the .00065 recommended by Harvey. 

I appreciate the help, I have a hard time with dynamic paths figuring out how hard i can push things especially with such a small 7 fluted endmill.

MATERIAL: STEEL, CORROSION-RESISTANT, BAR, UNS S17400
(17-4PH), IAW AMS5643, SOLUTION HEAT TREATED,
PRECIPITATION HARDENABLE
ALTERNATE MATERIAL: STEEL, CORROSION RESISTANT,
PLATE, UNS S17400 (17-4PH), IAW AMS5604, SOLUTION
HEAT TREATED, PRECIPITATION HARDENABLE

[gcode]

One thing to keep in mind is the TIR of your tool

a Ø1 endmiil running out .002" is .2% of the tool diameter and 10 to 20% of feed per tooth

a Ø.093 endmill running out .002 is 2.15% of tool diameter and 2 to 300% of feed per tooth 

this will almost certainly fail 

[crazy^millman]

No the RPM is correct and I was going off of memory for speeds and feed. This is a small tool so the smaller the tool the faster the rpm needs to be to maintain the correct Surface Footage per Minute. Not sure if you have been around CNC Lathes, but if you have every cut large diameter parts and faced them you will understand real quick max RPM for a CNC Lathe and when it becomes important. Here the tool is smaller so the rpm to maintain the correct SFM must them go higher. I have run .01 endmills at 100k with a speeder in aluminum parts with no issue. Like Gcode said runout if the killer so don't take for granted it is running true. I have seen brand new out of the box shrink fit holders with .004 run out. You know what you know when you know it and can prove it.

[Colin Gilchrist]

For dynamic paths, I usually stick with these default values to start:

Aluminum > 15% - 40% (30% is base)

Steel > 5% - 25% (15% is base)

Stainless > 3% - 15% (7% is base)

Titanium > 1% - 8% (3% is base)

HSRA > 2.5% - 10% (4% is base)

The "stiffer" the tool, the more you can trend towards the "higher" percentages. The longer the flutes, and the longer the "stickout" (and shoulder length below the shank), the less stiff the tool is. The damping ratio changes as the length(s) get longer.

I would guess that the Harvey Numbers for Chip Load, already include the RCTF. Keep in mind that "with more flutes, comes less room in the 'chip gullet' to pack a chip". This is part of what necessitates the "low radial immersion" of these paths. We are trying to "limit the contact length and time" of the flute hitting the material and shearing off a chip. The chip can't be bigger than the "space" in that chip gullet, otherwise we'll start "chip packing" and snap off the tool. This is also why we need air or coolant to "blast or carry away" the chips during the cut.

I've seen it happen where poor coolant flow is the reason that tools are snapping, not the actual cutting parameters. I had an issue where day shift was pumping out parts, and everything was running smooth as silk. Night shift starts to have some scrap pop up. One part here, one part there, etc. This goes on for a couple weeks. We start looking at speeds/feeds, stepovers, and all parameters. This goes on for almost two months. Finally, I decide I want to see what is going on myself. So I decide one day that I'm going to monitor the process. So I camp out by the machine for basically all of first shift. I'm watching the Operator, and he is on his game. He tends the machine, and is constantly adjusting his coolant lines to compensate for the different tool lengths, and also adjusts the tip angles of the coolant lines to direct the coolant where it is needed. I stay late in my office programming, eat dinner, and just kind of keep a watch over the process over the guy on 2nd shift. He "runs the machine", and by that I mean he loads a part, and pushes the button. He never adjusts a single thing. A couple of hours into his shift, I hear the "ping", and the change in sound of the machine going from "cutting metal to cutting air". So I walk up and confront the guy. I dig through the pile of chips and find the endmill which just snapped off. Sure enough, the flutes are packed with chips, because the coolant wasn't carrying away the swarf. This led to the endmill "re-cutting chips, and packing the swarf into the chip gullets".

[Colin Gilchrist]

I'd recommend the following:

11,000 RPM

.0005 per tooth x 7 teeth = 0.0035 per revolution (conservative)

0.0035 x 11,000 rpm = 38.5

I'd run 11,000 RPM, and 40 IPM.

I'd use a Step-over of 0.005, if you are going full flute length (100% or 200% step-down) (about a 5% radial stepover value).

If you're running a 0.009" stepover, I'd keep the Step-Down at 50% (about a 0.05 deep step, per pass).

But my preference is always to use the "as much of the flute" as is practical. The exception to this is "pocketing". Because of the need to flush chips, I like to stick with 50%-100% of the diameter, for my stepdown.

[[email protected]]

1 hour ago, crazy^millman said:

No the RPM is correct and I was going off of memory for speeds and feed. This is a small tool so the smaller the tool the faster the rpm needs to be to maintain the correct Surface Footage per Minute. Not sure if you have been around CNC Lathes, but if you have every cut large diameter parts and faced them you will understand real quick max RPM for a CNC Lathe and when it becomes important. Here the tool is smaller so the rpm to maintain the correct SFM must them go higher. I have run .01 endmills at 100k with a speeder in aluminum parts with no issue. Like Gcode said runout if the killer so don't take for granted it is running true. I have seen brand new out of the box shrink fit holders with .004 run out. You know what you know when you know it and can prove it.

Thanks for the input, when I used to setup for myself I indicated almost everything. I still get in debates with the guys on the floor whether or not indicating reamers is necessary...anyway I do understand the relation of Surface Feed to the Diameter of the cutter it just always make me feel uneasy when it tells me to spin it 4000 higher than my machine capabilities. I never would have thought to get a speeder to actually achieve 100k rpm(in .01 endmill scenarios), I just always turned everything else down to match the max rpm of my machine. Which I have never worked with anything faster than 15k spindles. Yes the small chip gullets getting packed and every other factor you guys mentioned is exactly why I brought this up here. Thank you all for your help. I will try to post back with results

[crazy^millman]

36 minutes ago, [email protected] said:

Thanks for the input, when I used to setup for myself I indicated almost everything. I still get in debates with the guys on the floor whether or not indicating reamers is necessary...anyway I do understand the relation of Surface Feed to the Diameter of the cutter it just always make me feel uneasy when it tells me to spin it 4000 higher than my machine capabilities. I never would have thought to get a speeder to actually achieve 100k rpm(in .01 endmill scenarios), I just always turned everything else down to match the max rpm of my machine. Which I have never worked with anything more than 15k spindles. 

When you need the speed these guys offer one of the best units. Need to run filtered air at at least 5 micron filtration. 

Big Kaiser 100k-120k Air Speeders

Air Regulators with filtration

[JB7280]

On 12/23/2021 at 10:46 AM, Colin Gilchrist said:

 

I would guess that the Harvey Numbers for Chip Load, already include the RCTF. Keep in mind that "with more flutes, comes less room in the 'chip gullet' to pack a chip". This is part of what necessitates the "low radial immersion" of these paths. We are trying to "limit the contact length and time" of the flute hitting the material and shearing off a chip. The chip can't be bigger than the "space" in that chip gullet, otherwise we'll start "chip packing" and snap off the tool. This is also why we need air or coolant to "blast or carry away" the chips during the cut.

 

Colin, I've been trying to learn more about where/when/how to push a tool to get better cycle time, or more tool life.  Is there a good way to tell if you're having a problem with chip packing, BEFORE tool failure? 

 

Do you know where I can learn more, regarding how to determine which parameters to push, things to look for, etc?

[crazy^millman]

1 hour ago, JB7280 said:

Colin, I've been trying to learn more about where/when/how to push a tool to get better cycle time, or more tool life.  Is there a good way to tell if you're having a problem with chip packing, BEFORE tool failure? 

 

Do you know where I can learn more, regarding how to determine which parameters to push, things to look for, etc?

Do you have Thru coolant Holders? Do you have High Pressure Coolant on the machines? If the answer to both of these questions is no then you are not able to push anything the same way as with it to really know.

We had a project a few years ago where 30 minutes into a cut in Titanium using the recommend speeds and feed the tools were snapping off. Now there were 2 factors working against us here. #1 was the forgings were 20% larger in areas than we originally told they would be. Corrected the programming to take care of that issue, but was still not getting the best tool life. The customer had a Tool voucher from a Vendor and begged us to use their holders. I called out the holders in a hurry trying to help going against my better judgement since the holders didn't have through the spindle coolant ability. We were still not getting the tool life I wanted or expected. Issue #2 was no Coolant through the Tool so we had the Hydraulic collets EDM drilled. The tool life was around 30-45 minutes. After it was 2-4 hours and were we able to push the tools even harder than before. The difference was the High Pressure Coolant was getting into the cutting area to evacuate the chips.

Have a customer right now decided to put High Pressure Coolant on some 23 year old machines. Were gun drilling parts at about 2 hours with standard Coolant pressure and normal gun drill in 17-4 PH. With a new Triple Margin Drill and High Pressure Coolant have got the drilling down to less than 20 minutes. The really benefit from the newer technologies the machines must be up to the task no in just processing the code stand points, but even the ability to evacuate the chips from the cutting point. Coolant is not the only means there are droplet type systems using air that are as effective. Also Cryogenics is picking up steam after 15 years in the development of it.

Colin touched on the discussion, but one I see many companies not fully grasp and understand its importance in today's manufacturing process and proper development of utilizing these toolpath strategies with the tooling now available.

[JB7280]

54 minutes ago, crazy^millman said:

Do you have Thru coolant Holders? Do you have High Pressure Coolant on the machines? If the answer to both of these questions is no then you are not able to push anything the same way as with it to really know.

We had a project a few years ago where 30 minutes into a cut in Titanium using the recommend speeds and feed the tools were snapping off. Now there were 2 factors working against us here. #1 was the forgings were 20% larger in areas than we originally told they would be. Corrected the programming to take care of that issue, but was still not getting the best tool life. The customer had a Tool voucher from a Vendor and begged us to use their holders. I called out the holders in a hurry trying to help going against my better judgement since the holders didn't have through the spindle coolant ability. We were still not getting the tool life I wanted or expected. Issue #2 was no Coolant through the Tool so we had the Hydraulic collets EDM drilled. The tool life was around 30-45 minutes. After it was 2-4 hours and were we able to push the tools even harder than before. The difference was the High Pressure Coolant was getting into the cutting area to evacuate the chips.

Have a customer right now decided to put High Pressure Coolant on some 23 year old machines. Were gun drilling parts at about 2 hours with standard Coolant pressure and normal gun drill in 17-4 PH. With a new Triple Margin Drill and High Pressure Coolant have got the drilling down to less than 20 minutes. The really benefit from the newer technologies the machines must be up to the task no in just processing the code stand points, but even the ability to evacuate the chips from the cutting point. Coolant is not the only means there are droplet type systems using air that are as effective. Also Cryogenics is picking up steam after 15 years in the development of it.

Colin touched on the discussion, but one I see many companies not fully grasp and understand its importance in today's manufacturing process and proper development of utilizing these toolpath strategies with the tooling now available.

Ron, the machine I work on most often, does have high pressure, through spindle coolant (1200psi) and most of my tool run in Lyndex SK collets, and I almost always run HP coolant through the collet.  Except of course when the cutting tool is equipped with coolant holes, then I'll use a sealed collet, or other appropriate method.  

[crazy^millman]

25 minutes ago, JB7280 said:

Ron, the machine I work on most often, does have high pressure, through spindle coolant (1200psi) and most of my tool run in Lyndex SK collets, and I almost always run HP coolant through the collet.  Except of course when the cutting tool is equipped with coolant holes, then I'll use a sealed collet, or other appropriate method.  

Awesome what I like to hear. Don't be afraid to push things then.

If you're working in Aluminum might look at these tools. Sorry I think they only come in Metric sizes.

SGS S-Carb APR 4FL

45014

[JB7280]

1 hour ago, crazy^millman said:

Awesome what I like to hear. Don't be afraid to push things then.

If you're working in Aluminum might look at these tools. Sorry I think they only come in Metric sizes.

SGS S-Carb APR 4FL

45014

In aluminum, I used a lot of the helical tools with the small chipbreakers.  I always thought the more "serrated", older style roughers like you linked, weren't as well suited for HSM toolpaths.  Is that not the case?

[crazy^millman]

53 minutes ago, JB7280 said:

In aluminum, I used a lot of the helical tools with the small chipbreakers.  I always thought the more "serrated", older style roughers like you linked, weren't as well suited for HSM toolpaths.  Is that not the case?

These tools have through the spindle coolant directly in the flutes and if want to keep long stringy chips under control for roughing then you are already using serrated edges. It might look like old a school rougher, but trust me the 4th flute in Aluminum with the TSP is a game changer. Want to bury this tool in a full slotting application give it a shot. Want to start thinking about 60% step over at 100% DOC using HST toolpaths this will be tool I will give it a try with. We all think only 3 flute for clearing out chips, but these tools with the polished gullet areas are impressive to watch cut. The TSP ability right at the cutting edges is the real difference. With TSP holders we get it above the tool, but with these it is in 2 places right at the cutting edges and at the tip.

[JB7280]

5 minutes ago, crazy^millman said:

v

 

5 minutes ago, crazy^millman said:

These tools have through the spindle coolant directly in the flutes and if want to keep long stringy chips under control for roughing then you are already using serrated edges. The look like old a school rougher, but trust me the 4th flute in Aluminum with the TSP is a game changer. Want to bury this tool in a full slotting application give it a shot. Want to start thinking about 60% step over at 100% DOC using HST toolpaths this will be tool I will give it a try with. We all think only 3 flute for clearing out chips, but these tools with the polished gullet areas are impressive to watch cut. The TSP ability right at the cutting edges is the real difference. With TSP holders we get it above the tool, but with these it is in 2 places right at the cutting edges and at the tip.

Interesting.  I will check them out next time I have a need.  I've been using some Garr VX-7 tools in titanium, invar, and heat treated stainless.  The coating they have on those tools is pretty amazing.  Blew every other tool I tried out of the water as far as tool life goes.

[[email protected]]

On 12/23/2021 at 8:59 AM, Colin Gilchrist said:

I'd recommend the following:

11,000 RPM

.0005 per tooth x 7 teeth = 0.0035 per revolution (conservative)

0.0035 x 11,000 rpm = 38.5

I'd run 11,000 RPM, and 40 IPM.

I'd use a Step-over of 0.005, if you are going full flute length (100% or 200% step-down) (about a 5% radial stepover value).

If you're running a 0.009" stepover, I'd keep the Step-Down at 50% (about a 0.05 deep step, per pass).

But my preference is always to use the "as much of the flute" as is practical. The exception to this is "pocketing". Because of the need to flush chips, I like to stick with 50%-100% of the diameter, for my stepdown.

So I went with 11,000 rpm @ 38.0" ipm and .280" ap(depth of cut) Min toolpath radius of .005" It worked GREAT! Thanks for the support to give me the confidence to try something out of my comfort zone.

[David Colin]

Speaking about small tooling and lubricant, anyone already tried this one? I should try it soon in Titanium. In demo video they use 2 flutes endmill but my seller told me he experienced that 3 flutes works the same (chipload) regarding slotting capabilities. 

 

[Aaron Eberhard]

27 minutes ago, David Colin said:

Speaking about small tooling and lubricant, anyone already tried this one? I should try it soon in Titanium. In demo video they use 2 flutes endmill but my seller told me he experienced that 3 flutes works the same (chipload) regarding slotting capabilities.

That looks really cool.  Let us know how it works out if you try it!

[JB7280]

1 hour ago, David Colin said:

Speaking about small tooling and lubricant, anyone already tried this one? I should try it soon in Titanium. In demo video they use 2 flutes endmill but my seller told me he experienced that 3 flutes works the same (chipload) regarding slotting capabilities. 

 

Mikron has some similar endmills without the fancy sleeve on the end.  The coolant pattern is great, and they work REALLY well.   Interesting seeing DIXI.  We have a huge 800mm DIXI HMC.

[jean]

On 1/4/2022 at 2:08 PM, David Colin said:

Speaking about small tooling and lubricant, anyone already tried this one? I should try it soon in Titanium. In demo video they use 2 flutes endmill but my seller told me he experienced that 3 flutes works the same (chipload) regarding slotting capabilities. 

 

That's Impressive.  

[So not a Guru]

On 1/6/2022 at 7:22 AM, jean said:

That's Impressive.  

Looks great in the video, let us know how it does IRL.