[cobrakai]

Hey everyone,
I'm working on a couple projects that require starting with a large 2" thick piece of 6061 aluminum billet and milling most of it away, with ~1.5" deep pockets and several .13" radius internal corners. That means a 1/4" end mill is needed in a few spots.

It also means I need to stop using my chipped end mill and buy a couple tools that will make this go smoother. I've done a ton of research and it has all led me to purchasing a couple 3/8" High-Helix end mills -- both roughing and a finishing type. First, to remove the bulk of the metal while leaving about .010" and then going back and finishing it off.

I'm over using HSS tooling because it just isn't as sharp and not nearly as rigid as carbide. Also, solid carbide tooling can be had for decent prices now. Also, it seems like 3 flute end mills work best all-around due to the ability to slot, profile, pocket, rough, finish, etc.



So, here's the concern. I found plenty of 38 degree and 45 degree tooling as mentioned above (MariTool High Helix for Aluminum). But I have been advised against using this in the Tormach with TTS due to possible pull-out issues. I had it pull out once during an aggressive cut before and that was with standard tooling, although I have since degreased all mating surfaces. Tormach has recommended indexable center cutting end mills, but they don't go small enough for what I'm doing.

What would you recommend for me? Thanks in advance for the input.

[WOTDesigns]

I run data Flute ARFs primarily in Aluminum but if you have a lot to remove I recommend 1/2" 3 Flute corn cob rougher. They remove material in a hurry and keep HP low compared to standard geometry. I've never had any issues with pullout related to tool geometry.

My personal opinion (I run my tormach and X3 both with TTS 60+ hrs a week) is that pullout is primarily poor maintenance. Period. I generally only get pullout if I do something REAL dumb like accidentally switch the order on roughing and finishing and send a 1/2" em 0.5" deep, full slot, 35 ipm... That causes pull out and then a broken end mill.

A collet can't just live in the machine and slide forever without maintenance. I pull the collet and drawbar every month or so and clean, re grease and re install. I also check he belt, motor mounting bolts, clean chips that got up there, etc. Almost every time someone asks about pull out after a disaster they then ask follow up questions that make it very obvious they completely and utterly ignored or didn't read the white paper on TTS.

Follow the white paper advice and you will break a 3/8 em LONG before you will see any pull out.

Brian
WOT Designs

[cobrakai]

Thanks Brian.

Is the reason for suggesting a 1/2" simply for faster material removal? Since most of my geometry is designed around a 3/8" internal radius I was hoping to find the best universal combination.

Also, do you have a power drawbar? I am questioning the draw strength of the Belleville washers as compared to manually torqueing the drawbar. But I did follow the directions by greasing the drawbar sliding surfaces, degreasing the TTS holder and inside of the R8 collet, and tightening the drawbar as specified. I'm just afraid to have it pull out again and ruin my work!

Where do you get your data flute tools? They look nice.

[WOTDesigns]

I do use the PDB. Yes 1/2 was just for material removal. Really the corn cob rougher are CHEAP so grabbing one of each doesn't hurt the bank. I order those from McMaster most of the time.

The data Flute I pick up locally from R L Stephens in Fullerton CA. I believe KBC will order them for you and just about any other local supplier should have them or order them.

Brian
WOT Designs

[cobrakai]

I found this selection guide helpful. By comparing their recommendations to the geometry, it's useful to see why they recommend each type.



Oh and thanks for the second reply. Looks like they are recommending the corn cob roughers only for ferrous metals, while their aluminum specific roughers actually have an odd interrupted edge. (ALDH-C)
Attachment 208386

Then they suggest these 5 flute finishing mills for taking off that last little bit.


But your ARF recommendation is great for all purposes. I'm definitely going to check these guys out. There are quite a few on eBay.

[WOTDesigns]

Yep. You can download their entire catalogs (very nice with great info) and price list. I have both on my phone. Handy when programing. Their feed rates tend to be a little outside the realm of the Tormach but gives a good idea of a ending goal... NOT starting point.

Brian
WOT Designs

[Steve Seebold]

I do use the PDB. Yes 1/2 was just for material removal. Really the corn cob rougher are CHEAP so grabbing one of each doesn't hurt the bank. I order those from McMaster most of the time.

The data Flute I pick up locally from R L Stephens in Fullerton CA. I believe KBC will order them for you and just about any other local supplier should have them or order them.

Brian
WOT Designs

Hey Brian, give me a call tomorrow and I'll clue you in on an endlill that works as good as the Data Flute for a lot less money. And I'll tell you where to get them. Trust me here, I've used them both.

714-420-2453.

[WOTDesigns]

Will do Steve. It's actually good timing since I'm starting a 3200pc production run tomorrow. I switched from 1/4 bar to 1/4 plate plate sawed to size and want to try 4 sheets thick instead of 3... Data Flute goes from 3/4 to 1.25 on the 1/4" ARF20250 so I'm happy to try a few 1" long.

Brian
WOT Designs

[Steve Seebold]

I found this selection guide helpful. By comparing their recommendations to the geometry, it's useful to see why they recommend each type.



Oh and thanks for the second reply. Looks like they are recommending the corn cob roughers only for ferrous metals, while their aluminum specific roughers actually have an odd interrupted edge. (ALDH-C)
Attachment 208386

Then they suggest these 5 flute finishing mills for taking off that last little bit.


But your ARF recommendation is great for all purposes. I'm definitely going to check these guys out. There are quite a few on eBay.

It doesn't matter who you ask. Any tool salesman will tell you the tools he sells are absolutely the best on the market for your application. When they tell you that, ask for a sample.

I did that once. I filled out a questionaire in a magazine and sent it in. It asked what kind of material I worked with and at that time I was doing a lot of work with 17-4 stainless. They sent me an end mill and recommended a feed and speed. I thought they were crazy, but I thought "hey, it's your end mill". I did it the way they said to do it and it turned out to be the best end mill I EVER found for cutting 17-4 stainless. That end mill was a DuraMill Whispercut. I ran it full width, 2,600 RPM and 36 IPM.

[WOTDesigns]

DATA FLUTE also has a new TRIPLE THREAT I'm waiting for an excuse to order. Steve is right and sifting through their BS gets challenging. One thing to remember is that NONE of them are making suggestions for Tormach rigidity or HP. The corn cob cutters (I use hss) seem to need no hp at all.

Brian
WOT Designs

[cobrakai]

Wait I'm confused. Are you saying I should trust their recommendations because they are the manufacturer and know what they're talking about, or there's a lot of marketing BS because they're trying to sell tools?

Now FYI, maybe I'm overcomplicating this for myself. Brian's talking about running 3200 pieces of something, while I on the other hand are dealing with maybe 20 or 30 of something. As such I'm only using a few tools and they will last quite a while before wearing out. Unless of course I snap them off

[Steve Seebold]

DATA FLUTE also has a new TRIPLE THREAT I'm waiting for an excuse to order. Steve is right and sifting through their BS gets challenging. One thing to remember is that NONE of them are making suggestions for Tormach rigidity or HP. The corn cob cutters (I use hss) seem to need no hp at all.

Brian
WOT Designs

Brian, if you have a part that has a lot of material coming out of a pocket, don't try to cut it all the the sides of your end mill. Make a hole pattern, drill the first hole then plunge ruff it. You'll move a LOT more material that way. You can make a hole pattern with a step over that's about a 40% of your cutter diameter and then all your ruffing pressure is in the Z axis. Straight down. You need to run flood coolant though. Spray mist won't work.

[Steve Seebold]

Wait I'm confused. Are you saying I should trust their recommendations because they are the manufacturer and know what they're talking about, or there's a lot of marketing BS because they're trying to sell tools?

Now FYI, maybe I'm over complicating this for myself. Brian's talking about running 3200 pieces of something, while I on the other hand are dealing with maybe 20 or 30 of something. As such I'm only using a few tools and they will last quite a while before wearing out. Unless of course I snap them off

If you use carbide and you use it the right way, you'll probably get tired of looking at it before you break it. I make a lot of parts. Most of what I do is one to ten piece orders with an occasional 50 piece job, but I have been running the same 1/4 inch 3 flute end mill for over one year.

[Steve Seebold]

Hey Brian, I forgot something. AFTER 9:00 AM. Remember, my shop is called "MID DAY MACHINING" That means I don't start till the middle of the day.

[WOTDesigns]

Their data is assuming massive machines with practically unlimited HP. You will not run a 1/2" (any manufacturer) deeper than 1/4" anywhere near their recommendations happily for very long . You have to modify their recommendations to work. DF doesn't even give slotting data on most tools, but their heavy peripheral at 1/2" deep will stall the spindle on my 1100 where a HAAS would provide great results (just as an example).

The 3200 part run I've run well over 15,000 parts for that assembly this year but they are run with a few drill bits and a 1/4" end mill in the first set up, 1/8 em second set up, one gets three more set ups. I learn all 1/8 x 1" em break about the same but some tend to leave a better finish. Small tools I don't trust to wear out on production so I throw the ARF20250 in a drawer after each run (usually roughing 2000 parts).

Last week I was running job shop work: 10 each of 4 different parts with the largest one being 1.5"x4"x8" with 70% of the material removed. Quantity doesn't really matter. Good tooling works well on 10 parts or 2000 parts just the same. I only use DF because it's locally available and I have a credit line with the company I buy them from which is handy since I only have to pay for my tooling every couple months. Every manufacturer has tools worth buying I'm sure. MELRIN and Lake Shore have great stuff too. I don't have their catalogs neatly stored on my phone and my supplier has to order their stuff. Useless to me. If I need a tool I need it now. I'm not ordering a tool because if it breaks and was so special I had to order it, now I can't work for three days till I can order and receive another one. Meah. Like buying local, but I have easy access so it's easier for me than someone in other locations I'm sure.

Brian
WOT Designs

[Steve Seebold]

If you were like me, you'd buy more than one tool that works good. I am 35 miles away from a tool supplier, so when I buy small tools, I buy at lease 4 pieces.

When I buy 3/4 end mills I'll buy one. 1/2 I'll buy 2. 3/8 or 5/16. I'll buy 4. 1/4 inch and smaller I'll buy 6.

I've even done a job where I had to use a .010 (ten thousandths) end mill. I got all the way through that job and only used 3 end mills.

The absolute best way to ensure you're going to break a tool when you're 35 miles away from your supplier is to buy just one.

[FuriousGeorge]

I really like the variable flute endmills from Lakeshore carbide for finishing (2 FLUTE ENDMILL FOR ALUMINUM) and the Tormach 17mm center-cutting modular insert EM for roughing (Center Cut End Mill - 17mm).

A good rule of thumb is to always use the BIGGEST diameter and SHORTEST length end mill you can use. Rigidity varies with length to the 3rd power and diameter to the 4th power. A 0.75" long End Mill is 8x more rigid than a 1.5" long EM and a 1/2" diameter EM is 16x more rigid than a 1/4."

for roughing on a Tormach IGNORE CALCULATIONS FOR SPEED!!!!!! Run it between 2500 and 3500 RPM and calculate your feed from there. The Tormach's torque is at a max right around 2500 and this is the most important factor for roughing with a hobby level machine. With the 17mm centercutting Endmill I run at 3500 RPM, 50 ips, .1" DOC and 60% stepover. The tool can easily take more than this, but it starts to affect your finish.

[cobrakai]

Good point about buying multiple tools. I have broken two 1/8" bits so far and chipped the teeth on a 3/8" bit. They are fragile if you don't feed it just right.

Picking the best RPM and feed rate is easy I think. Correct me if I'm wrong. The RPM should be selected based on chatter/vibration, motor torque, and cooling ability. The feed is directly calculated based on desired chip load (.001 for finishing, .005 for roughing) and number of flutes. So far I've been doing around 2500RPM with my 3/8" cutter but I think I could go a lot faster, like 4000, or 5000.

Where it gets confusing to me is the depth of cut and width of cut. There are so many variables here. A shallower depth of cut puts less load on the cutter but has fewer flutes engaged and has potential for more chatter. The width of cut affects the impact angle of the flutes with the material as it goes along, but if you have a cutter capable of slot milling, why not do almost 100% width of cut?

I realize these questions are going slightly off topic. I guess it's hard to get clear answers with this because there are an infinite number of ways to cut metal with millions of types of tools.

[SCzEngrgGroup]

Picking the best RPM and feed rate is easy I think. Correct me if I'm wrong. The RPM should be selected based on chatter/vibration, motor torque, and cooling ability. The feed is directly calculated based on desired chip load (.001 for finishing, .005 for roughing) and number of flutes. So far I've been doing around 2500RPM with my 3/8" cutter but I think I could go a lot faster, like 4000, or 5000.

Where it gets confusing to me is the depth of cut and width of cut. There are so many variables here. A shallower depth of cut puts less load on the cutter but has fewer flutes engaged and has potential for more chatter. The width of cut affects the impact angle of the flutes with the material as it goes along, but if you have a cutter capable of slot milling, why not do almost 100% width of cut?

A greatly simplified description. Calculating *usable* feeds and speeds is easy. Calculating optimal feeds and speeds is quite complex. And non-optimal results can greatly increase production time, reduce finish quality, and greatly reduce tool life. The correct values cannot be calculated with knowing at least the following critical parameters, though there are MANY others that can also significantly change the outcome:

Tool material, diameter, number of flutes, flute length, flute geometry, shank diameter, stickout, and several others
Work material
Coolant
Cut width and depth, which enables chip thinning calcualtions, which can enable drastically increased feedrates
Manufacturers recommended SFPM for that tool in that material
Manufacturers recommended chipload for that tool in that material
Machine rigidity
Spindle RPM, torque, and power capabilities

The toolpath being cut can dramatically affect the optimal parameters, with "HSM" toolpaths enabling MUCH higher feedrates, owing to the more constant tool loading.

All of the above will give you a reasonable starting point, which can be further optimized by listening to the machine, and examining test cuts. In many cases, the "cure" for a problem will be counter-intuitive. For example, if chips are welding to the tool, many users will increase RPM, and/or decrease feedrate, which is exactly the WRONG thing to do. Chip welding results form heat buildup in the tool, which is the result of too high RPM, or too low feedrate, and a resultant light chipload. A heavier chipload will carry the heat away from the tool. Under proper conditions, the tool will remain cool, and the chips will be very hot. The same is true for chatter. Often, the cure is to feed faster, not slower.

Look at some of the good feed/speed tools like FSWizard, HSMAdvisor, or GWizard, and you'll see just how much performance potential you're probably leaving on the table using the very simple calculations outlined in your post. Most people are quite surprised at how much more throughput they can get than they thought, and gain significantly increased tool life, and better surface finish, at the same time!

Regards,
Ray L.

[tbaker2500]

Cobrakai,
Couple of points. First off, using a 1/2" bit is HIGHLY recommended for the part you described, because of tool rigidity. I recently did a job where I had to do 2" deep pocketing, and so I needed a 2" LOC carbide 1/2" em. I could cut at maybe 50% of the speed I normally cut with my 1"LOC 1/2" em. The bit does bend, vibrate, causing chatter, poor finish, poor tool life. Your 1/4" em going down 2" is going to have a very tough time. Expect to break several before you get the cut figured out.

WOC vs. DOC. This was the hardest thing for me to grasp when I started. Here is my experience on a 1100. Doing full slotting more than .25" DOC is a no-go. Ultimately, it's very hard for the chips to make it out of the tool before the next chip tries to pack on top of it, unless you are cutting real slow. Cutting with a narrow WOC, you can certainly go much deeper, because the chip can fly away sideways. (Flood cooling often obscures these effects with the chips. Since I've started running dry, I've been able to see how the chip evacuation really affects the cuts.) But, most non-HSM cam programs don't have a function to cut at one speed for your first slot (If you are pocketing, your first cut WILL be a slot), and then a higher speed for subsequent cuts at higher speed and less WOC. Therefore, you have to set your feeds and speeds for the slotting cut if you don't want to break your EM. CAM programs like Sprutcam and HSMWorks use trochoidal milling and similar techniques to not cut a slot, but circle into a cut to keep the WOC constant.

Pullout- set it up right, and don't fret. The only time I've had pullout is on improperly tightened setup, or, most importantly, a heavily chattering cut. If your cut is squealing or chattering so bad to pull out the holder, so many other things are going wrong. Chatter can pull the part form the vise (yes, happened to me on a well tightened vise holding the part in step jaws), ruin the part dimensions, ruin the finish, and break your bit quicker. So focus on making a good cut (Use Gwizard as a starting point, and visit his page on chatter), and tune your setup to not resonate.