CNC Tooling
 

My team is ordering its firct cnc mill, a haas TM-2P, and I'm not quite sure what tooling to get. So far this is my list with the different questions I have. I'm thinking of buying a large part of this from Lake Shore Carbide and Maritool:

1/8" - 3/4" End Mills

• Do I need both roughers and finishers? How are the combined roughing and finishing end mills from Lakeshore?
• Which is better: Lakeshore variable flute end mills for aluminum or Maritool aluminum high helix end mills?
• For the maritool high helix finishers, which is the best coating?
• Should I get corner radius end mills in addition to square end mills?
• Should I get reduced shank end mill or regular length? Both?

4-40, 6-32, 8-32, 10-32 Specialty Aluminum Taps from Maritool

• Is spiral flute or spiral point better?

Reamers

• Do I need to get reamers for each of our common bearing sizes, or is the TM-2P precise enough with a regular end mill?

Drill/Mills

• Is it better to giet idividual tools for counterskining, chamfering, and spot drilling?

Ball End Mills

• Lakeshore variable flute ball end mills for aluminum vs Maritool 3 flute high helix end mill for aluminum?

Face Mills

• Which seller is best?
• Should I get multiple types(i.e. 45 degree and shoulder)
• What diameter should I get?

Drills from maritool

• Should I get screw machine length in addition to regular?
• Is carbide worth it?
• Should I get the 3 flute drills from maritool?

Re: CNC Tooling
 

Cory McBride. He's your guy for this.

Re: CNC Tooling
 

I'm hoping he'll respond to this thread. hint hint :)

Re: CNC Tooling
 

Endmills: Where I worked we used 3 flute carbide endmills from MA Ford. Probably the 116 series. I'm sure they aren't cheap, but they lasted a *long* time when run properly. We often used different tools for roughing and finishing, but they weren't roughing tools. They were just more worn down from so much cutting we didn't trust them for finishing. For my team, I've suggested they buy the 3 flute Aluminum specific endmills from maritool. We've made great use of roughing bits on the team, but somehow we usually got away with not using them at work.

Taps: Roll taps were the best. We didn't always use them, and I'm not sure why sometimes we used other taps, but we had various types of every size. The roll taps left stronger threads and they never jammed up and broke because of chips like the spiral flute taps do (because they don't make chips).

Reamers: You're never going to get a better hole than if you ream it. Always ream precision holes if you can. Even on a brand new VF3, we reamed high tolerance holes.

We chamfered, countersunk, and did spot drilling with 1 tool. We actually had 3 different tools, but they were just different sizes (1/4", 3/8", 1/2")

Shell mills: I mostly used 90 degree with rectangular inserts, but I've heard very good things about 45 degree with octagonal inserts. Mostly used a 3" tool, but the machines also had 2" tools.

Drills: If you can, I'd suggest you just get the 115 piece set, and individually buy a bunch of extra #43, #36, #29, #21, and #7 drills. That would cover you for #4-40, #6-32, #8-32, #10-32, and 1/4-20. The other drills don't get used all that much, so if your budget is restrictive a smaller set wouldn't really cause many problems.

Everything above is what we most commonly used, but our tool crib was full of specialty tools of every type, finish, and size (except the one you needed).

I'm sure Cory is going to show up with plenty more advice, and probably more applicable to FRC usage.

FWIW, my years on the team we used HSS Niagara cutter bits. We also struggled with speeds, feeds, and most importantly, a huge lack of decent coolant. We broke an insane number of cutting tools. The few carbide bits we had tended to shatter and the HSS bits would get hot, chips wouldn't clear out, they would weld on to the tool, and then it would snap off. We broke expensive tools (donations) too. So I'd just recommend taking it a little slow at the very beginning before you start throwing $30 endmills in there.

Re: CNC Tooling
 

Cory helped me get set up with some suggestions from Lakeshore and Maritool. It's quality stuff. PM me your e-mail address and I can send you a list of what we ordered. I'd recommend more ER collet holders than endmill holders. More versatile.

Re: CNC Tooling
 

I will try to post more later, but I'm in the middle of a ton of projects/work right now.

My best recommendation is don't splurge. Buy the things you know you will use all the time and add the rest later (unless you have the money now and have to spend it all right now).

We purchased a ton of tooling when we got our machine in 07 and to this day about 40-50% of that initial purchase has gone untouched because we didn't know exactly what we'd be doing and what we should buy.

We got a bunch of ball end mills and roughing end mills in regular and extended lengths as well as 2 and 4 flute end mills in regular/extended. We have pretty much any size you'd need and any type, but they aren't good for what we do every day. We've pretty much turned over all our tooling so that nothing we use on a regular basis is comparable to any of the tooling we initially purchased.

I like Lakeshore for end mills. Never really have purchased from Maritool, since their end mills have been more geared towards ferrous machining until recently. Don't bother with the roughing/finishing combo. Your machine doesn't have enough power to take full advantage of either. We have 2 flute and 3 flute in 1/8" increments from 1/4" to 3/4", with the vast majority being 1/4" and 1/2". 2 flute for anything under 1/4". If you treat them nicely they will last forever-I've been using one 3 flute 3/4" end mill for 3 years and a 3 flute extended length 1/2" end mill for almost as long. Pretty much the only reason you'll ever need to replace an aluminum specific EM is because you either did something stupid and broke it, or you couldn't evacuate chips fast enough to keep it from loading up and snapping. They really don't wear out.

The only coatings worth looking at are Zirconium Nitride, Molybdenum Disulfide (Destiny Tools' "Stealth" coating. Really awesome for aluminum), Titanium Diboride, and Titanium Carbonitride (ok, but not great). Avoid Titanium Nitride, Titanium Aluminum Nitride, or Aluminum Titanium Nitride like the plague for non-ferrous applications. These will cause aluminum to gall on the tool.

If you are just learning I would probably recommend against purchasing the aluminum specific tools up front. It's hard to justify spending 50 bucks on a 1/2" endmill that you are guaranteed to break in short order when you could spend half as much for a tool that will get the job done a bit slower. Once you have some experience operating the machine and aren't making as many mistakes they're a worthy investment.

I also like latheinserts.com. We bought a lot of aluminum specific inserted tooling (and some Destiny end mills) for our lathe and CNC mill from them. The owner is very friendly and helpful with recommending tooling for a given application. His prices are also extremely good and he will never try to sell you something you don't need.

Re: CNC Tooling
 

Thanks everybody. You've helped me to narrow down what to buy by a lot. This is the updated list of tooling to buy with comments and remaining questions:

End Mills(from Lakeshore, current ones are uncoated carbide, once we learn to use the machine we will be getting the specialty aluminum ones):

1/4" - 3/4" 2 Flute End Mills Regular Length
1/4" - 3/4" 3 Flute End Mills Regular Length
1/8" 2 Flute End Mill Stub Length(I feel like the majority of work done with a 1/8" end mill is on plate that had a maximum thickness of 1/4". Should I get both this one and the an 1/8" 2 flute regular length?)
1/4" 2 Flute Ball Nose End Mill(for any strange shapes we might have to make)

• Should I get any extended length end mills?
• Should I get any corner radius end mills?

Reamers(Solid Carbide from Maritool):

.874" Reamer
.875" Reamer
1.124" Reamer(anybody have a supplier for these. I've checked multiple online places and have not found a place that sells them yet)
1.125" Reamer

Face Mills:

• Which seller is best?
• Should I get multiple types(i.e. 45 degree and shoulder)
• What diameter should I get?

Drills(All regular drills are high speed steel from Maritool. If we need tap drill sizes or longer clearance sizes we will throw them in a drill chuck):

#9 Screw Machine Length Drill(10-32 Close Fit)
#21 Screw Machine Length Drill(10-32 Tap)
#18 Screw Machine Length Drill(8-32 Close Fit)
#27 Screw Machine Length Drill(6-32 Close Fit)
#32 Screw Machine Length Drill(4-40 Close Fit)
#9 Jobber Length Drill(10-32 Close Fit)
1/2" 82 Degree Countersink Drill from Maritool

• Is high speed steel sufficient for FRC?
• I figured that the tolerances on a cnc would be sufficient for close fit. Should I get free fit sizes instead?
• Should we keep the tapping drill sizes ready in our tool crib too?
• I decided against the mill/drill(combo tool for spotting, chamfering, and countersinking). Is this a bad decision?
• Has anyone used the maritool aluminum specific 3 flute drills?

Taps(thread forming taps, from Maritool):

4-40, 6-32, 8-32, 10-32 Taps

• any other confirmations on thread forming being better than spiral flute?
• spiral flute?
• recommendations on specialty aluminum taps from Maritool?

Re: CNC Tooling
 

Do you have a budget? It's hard to give recommendations in a vacuum.

I would recommend against buying anything over 1/2" in carbide until you are familiar with the machine. You'll just be throwing away money and $86 is not a small mistake. I'd probably start with 1/8" 3/16" 1/4" and 1/2". You could throw 3/8" in if you like, but it's not super necessary. There's really never any reason to have end mills above 1/4" in increments of less than 1/8 though, and usually 1/4 is a better interval.

Depending on what tool holders you get (not a good idea to use in a collet chuck, as the flutes on the second end will get clamped against the collet), Lakeshore's double end mills are a good investment and can save you about 33% on sizes 1/2" and under.

Extended length isn't necessary at the start. You'll figure out what you need it for and then you can buy it as needed (probably only will need 1/4" and 1/2").

Corner radius is always preferred if you don't need a square shoulder. The number one reason end mills go bad is the corners of the flutes chip and then the cutting edge gets destroyed. Corner radii help prevent this.

Carbide reamers are a waste of money for FRC purposes (Maritool doesn't even sell anything above .500 in carbide). Stick with HSS.

We don't bother reaming anything we CNC unless we want a precise slip fit. Press fit bores are just as easily achieved via circular interpolation. It's generally a good idea to have a healthy stock of reamers though.

This is pretty much the best face mill you can buy for aluminum (we have one). The problem is the inserts are extremely pricey, only give you 2 cutting edges, and cannot be used to cut anything but aluminum or plastic. That kit is a fantastic deal as you would pay $700 for the inserts and body normally.

I'd probably recommend this guy as it's dirt cheap, has a unbeatable warranty (destroy it, even while being an idiot, and the replacement is free), uses cheap inserts that can be indexed 4 times, and can take inserts for ferrous and non-ferrous materials (he only sells ferrous inserts but I'm certain he could find you non-ferrous ones). Your machine can't take a decent cut with anything over 2". 45 vs 90 only matters if you intend to cut to a shoulder with the face mill. 45 cuts better.

Maritool sells nothing but high quality stuff, but you want bright finish drills and the only standard drill bits he sells are black oxide. Aluminum has an affinity for black oxide and will stick to it. The parabolic drills are unnecessary. They won't work well in anything but aluminum and a standard 118* or 135* drill works just fine in Al. No need for anything but HSS either.

There's nothing wrong with the 82* countersink, but you'll need either a spot drill or a mill/drill to spot drill holes and chamfer any features that are not holes. Close vs free doesn't have much to do with the accuracy of the machine as compared to what it is you're assembling and how much slop you can afford (or how much you need to actually be able to put it together). We use free because #7 becomes a dual purpose drill.

Form taps are great but they're a fantastic way to get yourself in trouble if you don't fully understand how they work and the relationship between percent of thread profile, class of thread, and H-limits. Essentially you have to drill a larger hole than a cut tap uses, but that hole is not always the same size depending on what the H limit of the tap you buy is.It can also become problematic when you have a part that for one reason or another you can't or don't want to tap on the machine and you drill it for a form tap and then someone else hand taps them with a cut tap without realizing the difference. They're also only good for ductile materials (aluminum, low carbon steels, some stainless)

More important than the cutting tools you get, you need to get workholding and toolholding. These are a significant investment relative to the cost of cutting tools.

Re: CNC Tooling
 

This is one of the best threads/posts I've seen on Chief in a long time.

Re: CNC Tooling
 

Agreed saving this one!

Re: CNC Tooling
 

Don't forget about workholding and toolholders are Cory mentioned. Those are the big expenses up front. Bare minimum you want a step block kit and 1 or 2 good vises. Kurt is the standard, but we have two Glacern 615's (http://www.glacern.com/gpv_615) that have been great. About half the cost of the comparable Kurt (3600V), it gives you the ability to clamp the vise on it's side for tall parts. Jaw bolt pattern is the same as the Kurt's, so you can use any of the industry standard step jaws, v-jaws, soft jaws, etc.

Are you set for CAM software? That's the other big consideration for most teams. We use EdgeCAM since we use it in our PLTW classes, but MasterCAM is probably the most widely used package.

I don't see much use for any end mills over 1/2" - it puts a big load on the pull stud, and the TM machines don't have a ton of torque/HP to start with. Power output drops off at high spindle speeds you'll be using for aluminum. There are motor curve charts out there if you do a little googling. Peak torque for the TM-2 is at 1200RPM as per the Haas site. For frame rails, gearbox plates, and the like, there's really not a lot of need for a huge end mill.

Form taps are good for small threads (#4 & #6), but for bigger sizes I've never seen a big advantage. Spiral point taps (shoot the chips ahead of the tap) for through holes, spiral flute taps pull the chips up and out the flutes of the tap (for blind holes). Buy a bunch of the appropriate wire gauge pilot drills (#36,29,21,7) in short or stub length. We buy the "Heat-Resistant Cobalt Steel Short-Length Drill Bits" from McMaster (28765A57), Cobalt is unnecessary, but McMaster only has TiN and Black Oxide in short length HSS, and those are both bad for aluminum.

Get a mill/drill with a 90 degree tip. McMaster stocks those as well. They can do triple duty (drilling, spotting, and chamfering).

Re: CNC Tooling
 

Also give your local MSC and Sandvik Coromant reps a call. Over the years I have had reps arrange for a good amount of tooling; as some shops have tooling that they can not use for production that would work great for learning.

Re: CNC Tooling
 

For workholding we are thinking of getting 2 Kurt 3600V vises. Because the table on the TM-2P is so big I'm not sure if it would be beneficial to get 3 vises. I've heard good things about glacern too so we are still deciding between the twoo. Workholding seems like it is a very good area to invest in.

For CAM I've heard good things about mastercam from the CD community but our haas rep recommended gibbscam. I'm still not quite sure which one to get.

I found these drill bits on mcmaster: http://www.mcmaster.com/high-speed s...gth drill bits. They say good for steel, cast iron, and plastic and they are 118*, but I assume they will be fine.

Are 90* spotting driil okay? I've heard that your spotting angle should be bigger than your drill bit angle.

For toolholding I want to get at least 4 1/4" EM holders and 4 1/2" EM holders. I'm still not sure if I want to get 1/8", 3/16", and 3/8" EM holders. I want 14-16 ER16 tool holders, 1 drill chuck, and 1-2 face mill arbors.

Re: CNC Tooling
 

Having used both gibbs and MasterCAM, I would definitely prefer MasterCAM, personally found it easier to use and it's industry standard. Also for my quick and basic stuff [most of it] I use HSMXpress it's a CAM plugin that integrates into SW [inventor soon to come, Autodesk just brought them] and for 2.5D milling operations is completely FREE.

For tooling such as drill bits, you should just really start with some cheap/basic bits and work your way up. Find what you like and would use the most often then buy good ones of those. For drill bits HSS bright finish bits will work fine and you probably wouldn't really notice a difference between 118 and 135 degree points, again get some and try them and see what you like. Everyone prefers a little different tooling.

For when we had access/used a HAAS machine, it was a mini mill with the 10 tool ATC. It was loaded with an edgefinder, facemill, drill/countersink [used a spot], and then the rest were all CAT40 ER20 holders. A full set of collects going from 1/32 all the way up to 1/2 was used for an endmills and drill bits, we kept the common sized endmills/drill bits in the machine [1/4, 1/2, drills for taps, etc] and then used the left over tool changer spots to load up uncommon drill bits/endmills for whatever part we were working on. For the common sizes we had extra collets for so we could run more the one size tool at a time. With this setup we really didn't have to change out tools to often. However the machine was not ours and often was switched out between jobs.

Also do you guys have an mentor/teacher that is onsite that can help you guys get setup with the HAAS? The HAAS control software isn't terribly hard to learn but having an expert with you is a great asset.

Re: CNC Tooling
 

We sat through live demos of about 5 different CAM programs and settled on OneCNC XR5 for many reasons. We haven't used it extensively yet, but it has a great feature set, pricing, and support. You can PM me about it. I haven't used MasterCAM since version X, which was rather buggy and somewhat painful to use. I've heard it's gotten much better. I tried GibbsCAM years ago and hated it, and I've heard similar stories from others.

Re: CNC Tooling
 

4 each of 1/4" and 1/2" end mill holders is a lot. We only have 2 of each. You don't want to use a solid holder for 1/8" end mills. Any runout will destroy the tool in short order. Use a collet.

14-16 is a lot. It's taken us 5 years to accumulate that many and our machine can hold more tools. I don't know that I'd start out with so many. I'd also add a few ER-32's. You're going to want them to hold any drills/end mills over 1/2", or even 3/8" for rigidity purposes.

I don't really see a need for 2 face mills-just get one that takes standard inserts that are available for ferrous and non-ferrous materials. I'd rather have 2 drill chucks.

The drills you found are fine. 90* spot drills are fine.

The more vises you get the better. 3 vises means you're 50% more productive if you're making multiple parts. I would buy 4 of the Glacern 3600V clones over 2 3600V's.

Again, all of this comes back to your budget. This is all a "price is no object" list without one. If it's tight, lots of things I've suggested can be cut back to the bare minimum to get up and running.

Re: CNC Tooling
 

I thought I'd revive this excellent thread from the dead. Getting ready to purchase some new tooling, and I see there are usually several options for the amount of corner radiusing. For example, Maritool offers .008, .015, .030, .060, and .090 radius options for a 1/2" endmill. Never having purchased one I'm not sure why to choose one over the other. I'm assuming that the biggest radius will lengthen tool life the most, and since we are mostly doing thru-cuts on everything the radius will never have an impact on the cut geometry. Anyone care to elaborate on this?

Re: CNC Tooling
 

You have it right. Larger radius will reduce the chances of edge chipping and increase tool life.

Re: CNC Tooling
 

Would you mind sharing some fixturing techniques Cory? Are team is trying to figure out the best way to mill gearbox side plates.

Re: CNC Tooling
 

Although I'm not Cory, we usually put a good size tooling plate (just 6061 plate, about .75" thick or so) in a vise and face mill it to level it out. Then we run a program to drill and tap that fixture plate with our hole locations for our gearbox plate. Then we clamp 1/4" plate to that with little C clamps, then we drill the 1/4" plate only barely through, using the same XY part zero offset. Then we remove the clamps, bolt down the plate, and do all the pocketing and cut the outside profile.

Re: CNC Tooling
 

We do what Dave said, with modifications. If the plate is small enough to be clamped in a vise (less than 17" for our vises), we'll clamp the plate in the vise, drill and tap all the holes in it, then load up a fixture plate and drill and tap through a subset of the holes drilled in the actual part in the first operation.

Another alternative that works well for smaller (roughly the size of our drive gearboxes) is to do everything in one operation, in a vise, and leave tabs connecting the part to the stock when contouring the outside. After you're done you can cut the tabs and sand them flush with the outer contour. If you're careful and you follow the sanding with scotchbrite you can blend the contours very well.

Re: CNC Tooling
 

A more quick and dirty solution is, I have just taken 1/4 6061 and clamped it to the table of the machine with a hunk of 3/4 ply wood in between. Then drill my though holes, and wood screw the alum plate to the chuck of wood. Then do all the inside/outside cuts, pop the screws and you have your part.

Re: CNC Tooling
 

We run more or less the same setup, but we use acrylic as backing and double-sided tape instead of retaining tabs or screws on the part.

Just tape the part to roughly the same size scrap acrylic (we use 9mm), and strap clamp the part onto the table. We generally run a 1/4" 3 flute high helix end mill with 0.1" deep passes. With that you don't have to worry about chip evacuation in the slot, and it leaves a thin final pass (0.025" in 1/8" and 0.05" in 1/4"). Then just take the whole plate out of the mill, hit it with the heat gun until the tape releases, and then assign freshmen to a character building deburring/scotchbriting.

Mitee-bite sells a similar product that leaves less residue, but you have to heat the part to apply and release the compound. Double sided tape seems to be cheaper and faster when you have students to help. It's McMaster number 50245A21.

Otherwise just check out Mitee-Bite or Carr-Lane and poke around, they have lots of interesting stuff for fixturing. We tend to just do a lot of simple parts in the vice, the double sided tape method, and rarely a part using soft jaws. Two vices are helpful for long parts to minimize vibration/chatter, just indicate them in and clamp your part.

Re: CNC Tooling
 

I'm fairly accomplished with manual mills and lathes, but I am almost done building a 27" x 50" CNC router, and I'd like some advice on tooling and cooling. The driver here is a Hitachi 2.5 HP variable-speed router, with a range of about 8000 to 24000 RPM and 1/4 and 1/2" collets.

I see many choices of straight bits for cutting aluminum. Any suggestions on what to look for / at, brands that seem to work well, etc.?

In my manual milling and turning world, coolant use is rare. Just don't need it for most materials. But in the CNC router world, I fear that coolant is almost always used. Anyone have time to help me drink from that firehose? Not just coolants themselves, but ways of applying it, collecting, filtering out the chaff, etc. I don't even know what I don't know yet...

Re: CNC Tooling
 

I'll leave others to comment on tooling, but I will say we run a mister nonstop during cutting. It greatly increases cutting speed and reduces failures. This doesn't create a lot of liquid per hour, so we don't have any method of collecting or reuse for it.

Re: CNC Tooling
 

We have a mister that looks just like this one on are diy CNC http://www.cnccookbook.com/CCMillCoolantMister.htm
I'm not sure where we bought it but it connects to a 20 psi air line and another hose goes into a coolant bottle. It uses a venturi to suck up the liquid. Since it uses compressed air it also helps blow chips out.

Re: CNC Tooling
 

On our router at ~20,000 RPM, we've had a lot of trouble cutting aluminum with a standard 1/4" 3 flute carbide variable helix endmill we use with great results at 6,000 RPM with coolant on the mill. On the router, it just wants to load up and melt/weld chips. I'm thinking a 2-flute would give better chip evacuation.

Currently, our coolant system on the router is a student and a spray bottle of WD40.

Re: CNC Tooling
 

David,

Like Adam we also use a mister non stop. Your issue is using the WD-40 squirt bottle. Its a waste of time, we did that for a few weeks until we got tired of endmills gumming up and wasting our money.

What we also do is a run 2 airlines + the mister. So two airlines are blowing away the chips so your not recutting chips. The mister keeps the endmill from gumming up.

http://littlemachineshop.com/product...y=212208195 9

This is the one we have, bought it off of ebay for ~$40 bucks.

-RC

Re: CNC Tooling
 

We use a mister too. I'm not sure of the model. It does help a significant amount, we've been able to cut faster after starting using it (I think we started out at like 2 in/min with a 1/4" cutter in 1/4" alu before, now we set it to 6 ipm fairly regularly). In my experience, mist coolant helps most with cutters in the 1/4" to 1/2" range, where heating tends to slow down your cutting speed. With very small cutters (1/8" or smaller) I've seen them break more because of their small diameter than whether or not coolant was used.

Like others have said, collection or recycling isn't really an issue as the mister doesn't put out much fluid. However, it's very important to clean up properly after using the coolant. A lot of our steel tool holders have noticeable rusting in small spots from the mist, and after some pooled under our vise, it left a mark on the machine's table. I recommend wiping down the machine well every day, and taking up any fixtures on the table every week or so. On the other hand, it's a good idea to do this anyways.

8000 is extremely fast for tools in the 1/4" or 1/2" range, in my experience. With coolant, I believe we typically set 1/4" two flute cutters at 2000 rpm or so in 1/4" aluminium at a feed rate of about 5 ipm. Our mill only goes to 3600 rpm, and we only really use it that high for very small tooling.

Re: CNC Tooling
 

A 1/4" diameter carbide end mill under ideal conditions wants to be run between 12,000 and 36,000 RPM (750-2000 SFM).

At 2000 RPM you're at 125 SFM which is fine for HSS but doesn't take advantage of carbide's benefits.

Re: CNC Tooling
 

Don,

Look at the Onsrud catalog - the 63-600 product line is probably what you want to pick up. McMaster sells them if you search for "Router Bits for Aluminum" - "Grooving and Slotting". They're 1 flute solid carbide. The biggest issues with routers are going to be chip evacuation and and getting lubrication on the tool.

The 1-flute tools are nice because they give plenty of space to evacuate chips, and you don't have to run them at a high feed rate to maintain a proper chip load on the cutter to prevent it from rubbing. Depending on the construction (ball screws? rack and pinion?), your machine will probably be happier at lower feed rates and acceleration rates.

You'll definitely need something to get evacuate chips and provide a little lubrication on the tool. Otherwise you'll be re-cutting chips and getting a built up edge on the cutting tool - leading it to load up with aluminum and come to an untimely end. We're picking up a micro-drop coolant system (Trico Md-1200), which is like a mister, but instead of a constant stream of mist, it shoots small droplets of lubricant along with an air blast. They're more expensive than mist systems, but seem to clear chips better and don't make as big of a mess. Regular misting systems tend to linger in the air, and breathing that stuff isn't the greatest. At the very least look into a Fogbuster system to minimize that, or good ventilation.

Re: CNC Tooling
 

Second the Onsrud single flute cutters. They have been life-changers for our CNC Router. We run our spindle at 18,00 RPM with these same 63-XXX series Onsrud cutters, and they are incredible. Chip clearing performance was key in getting nice finishes on our cuts - and the feed rates we can run with these cutters are pretty aggressive too.

Our CNC Router came with a Unist Mister as an option, and we consider it a must when cutting aluminum. Mr. Stehlik here at 610 has been a big fan of the mist coolant approach and Unist misters in general, and has outfitted our metal chop saw, mill and lathe all with similar Unist misters. I don't think we've used a bottle of coolant all year long, clean-up has been easier, less machine corrosion, and the cut qualities have probably been better overall.

Here's a link to our Canadian supplier for the Onsrud cutters:
http://www.cncroutershop.com/ca/inde...us-metals.html

A not very useful picture and description of our router's mister setup from the manufacturer:
http://www.axyz.com/us/secondary-options/
...but if you read between the lines, it setup not as a continuous mister, but as in the post above it periodically dispenses droplets of coolant through a pulse generator.

A link to Unist's line-up of misters:
http://unist.com/solutions/machining-cutting.html

Re: CNC Tooling
 

We got a box of roughly 100 1/8" bits for our 4' by 4' cnc router to cut sheet aluminum. Our sponsor gave us the box several years ago, and we've only broken a few and we've cut a TON of sheet metal. The bits are similar to 3317A21 from mcmaster, but they are a little different, and the writing on the box is in Chinese. The trick is to get the feed rate correct, and have an air line always pointing at the bit.

Re: CNC Tooling
 

Thanks for all that info, especially the mister and lack of need for fluid collection - it seems that's the way to go.

6 IPM? gee, that's really quite slow. I expect to be cutting several tens of inches per minute. Maybe my mileage will vary...

The minimum speed I can get is 8000 RPM.
OK on Omsrud, I have heard this from others as well.

It is a Rack & Pinion machine, with an integrated dust (chip) collection system and safety shield (using a 2-1/2" vacuum hose), which I hope will deal with both the mist vapors and chips. And dust, when I cut anything not metal.

Any comments on which cooling fluid you use? There are so many choices...

Re: CNC Tooling
 

Have you checked out the math for calculating speeds and feeds? 2000RPM and 6IPM is way too slow, that's only 0.001 in/tooth. Way too low for a 1/4" end mill.

Spindle Speed is roughly the surface speed (in feet/min) * 4 divided by cutter diameter. Carbide in aluminum numbers can exceed 1000 SFPM, so you can run up to at least 16,000 RPM with a 1/4" cutter. You can run slower with no ill effects here, might want to check out where the peak torque or efficiency is on your router.

Feed rate is the chip load * #teeth * spindle speed. Here's the link to the Onsrud specs. They don't provide a SFPM rating which is odd, they just list 16,000 RPM.

http://www.onsrud.com/files/pdf/2012...20Aluminum.pdf

They list 0.003-0.006 in/tooth for 1/4", you don't want to have this drop too low or the cutter will just be rubbing as opposed to taking a clean chip. Plugging those in gives you 16,000 RPM and between 48 inches/min and 96 inches/min as your feed. If your machine is unhappy accelerating that fast - just drop the spindle down to 8,000 RPM and feed between 24 in/min and 48 in/min.

I like the calculators at this site - they have one for HP/Torque requirements also that will let you get a feel for how heavy your cuts are.

http://www.custompartnet.com/calcula...speed-and-feed

G-Wizard is another nice (pay) piece of software that gives some good suggestions and does fancier stuff like calculating tool deflection on smaller cutters.

http://www.cnccookbook.com/CCGWizard.html

We use KoolMist 77 as flood for our mill (McM 11365K61), but it obviously works as mist as well. It's probably not the ideal coolant for aluminum, but it's one of the safer ones to work with. The MSDS sheet is pretty tame, it doesn't go rancid in the tank, water soluble, no skin reactions, biodegradable, etc.

I would just take the dust-shoe off when you're cutting aluminum, it'll get in the way of the coolant system and you won't be able to see the cut. Bump up the pressure in the mister so that it clears chips from the slot, or mount up an air blast. A lot of milling in steel and hard alloys is now done without coolant, just a heavy air blast to clear chips and prevent recutting. Aluminum needs the lubrication though.

Re: CNC Tooling
 

Yes, 6 IMP. We do throw a good chip though, nice little curls. It is quite slow, mostly because we have a mill mentor who is, shall we say, conservative, with his machine's speed. He is right to go slow, though, the chips look good and we have had problems with breaking tools in the past (and crashing into clamps, but that's another story).

I'm sure with those router speeds, you'll be able to go faster. We're running a very different type of mill (a HAAS toolroom mill), so take my cutting speed experience with a grain of salt.

Perhaps we do cut too slow, but since the chip looks good and our part tends to vibrate excessively if we push it much faster, I'm inclined to stick with what we have now.

Re: CNC Tooling
 

A HAAS TM should be able to go faster.......... we were cutting up to 30IPM on ours in Alum with no problem.

What kind of spindle speeds are you spinning at?

Re: CNC Tooling
 

Are you using carbide or HSS? With HSS I could see 6 IPM being reasonable, but you should be running at about 0.003 IPT or more with a good carbide end mill, which would be a baseline of double what you're currently running. With a cutter that small and a top speed of 3600 RPM I would never run slower than max speed. We were forced to run our machine no faster than 2500 RPM recently and were slotting 1/4" plate at 23 IPM with a 3 flute end mill. You have a less rigid machine, but 1/4" Al plate isn't very taxing and I would expect similar performance.

As Scott mentioned, with a chip load of 0.0015 IPT you're coming closer to smearing material off as opposed to shearing, which will dull your tool and cause premature breakage. This will be a bigger problem if you're conventional instead of climb milling as chip formation begins with zero thickness and increased rubbing.

If you find that you're breaking tools it's almost certainly a chip evacuation problem. We can slot 1/4" plate with a 3 flute aluminum specific end mill indefinitely as long as the chips are cleared out of the path of the tool. As soon as you start re-cutting chips you run the risk of dulling/snapping the tool or welding the chips to the flutes.

Re: CNC Tooling
 

Like I said, somewhere in the 2000-3000 rpm range.

Re: CNC Tooling
 

Just for perspective, whenever I CNC using a 1/4 HSS EM I run the spindle at 2500 rpm and cut at 10 IPM. For me HSS doesn't chatter till you get up around 20IPM, if you're chattering at 6 IPM you might want to look into your fixtureing and make sure you've got a nice sharp endmill.

Re: CNC Tooling
 

Most of our cutters are HSS, but I believe we have a few carbide tools. We tend to really only push up to that 3600 limit when using 3/16" end mills or smaller and small diameter number drills.

This whole discussion of our cutting rate leaves me rather wondering if our mill has been incorrectly displaying units for cutting or something... I was always told that the units for the feed rate readout were in inches per minute. Like I said, we usually cut with that in the 2-6 range. I think we've pushed it up to 10 or 12 in the past, but that introduced some very serious vibration, and I believe even some tool deflection. Cory, maybe you're right, maybe this is all caused by a less rigid table, and our low cutting feed rate is just a product of vibrations occurring when we get near "normal" cutting speeds.

We have experienced some dulling and tool wear. Perhaps this is due to the lower cutting speeds we use wearing instead of cutting. When we increase spindle speed and cutting speed, though, we tend to start melting chips onto the tool. I always attributed this to poor cooling (even with the mist coolant) rather than chip evacuation or low cutting speed. We always (well, except for a few special cases) climb mill.

Granted, when I'm talking about tools breaking, I'm talking about a couple of 3/16" or smaller endmills breaking when they took too deep a cut at too high a feedrate.

Re: CNC Tooling
 

Feed on a mill is displayed in inches per minute, but it doesn't mean much without knowing the chip load which is in inches per tooth. Chip load is independent of number of flutes, which makes it easier to talk about as a comparison.

Re: CNC Tooling
 

Most work I do with a 3 flute carbide 1/4" endmill with flood coolant is at 6000 RPM and around 40-50 IPM depending on stepover and depth of cut, and I bet I could feed a good deal faster than that. I slow it down to about 20 IPM for a 2-flute ball endmill.

On our router, I'm running about 18,000 RPM on a 1/4" 3-flute carbide, and cut around 12 IPM (and much lighter cuts too) but that's due to a lack of coolant of any sort, poor chip evacuation, and chip recutting which is causing a heating issue.

A machinist I work with is running a 1/4" 3-flute tool at 12,000 RPM and 350 IPM (with flood coolant of course) with a 1/4" DOC and high-speed machining toolpaths with probably 25% stepover.

Re: CNC Tooling
 

I uploaded a machining calculator called ME consultant to the CD media section. It's a great simple freeware tool to find out basic speeds and feeds.

Enjoy

Re: CNC Tooling
 

Thanks for that coolant info Scott. "Rancid in the tank" is a real eye-opener for me. Oh, and the dust shield is clear plastic, so seeing the cut isn't a problem.

DampRobot, 6 IPM is 1" in 10 seconds, or 0.1" per second. Just seems slow to me, but....

1. You're getting good results. Something must be right, eh?
2. What kind of depth of cut we talkin here? 0.1" or 1/2"? That matters...

Anyway, I keep looking at #1 above and concluding it's OK.

Re: CNC Tooling
 

I remember vaguely that the tool moved about one tool diameter every two seconds (for a 1/4" tool) when we were cutting quickly. That gives a feed rate of 7.5 IPM, which squares fairly well with the 6-10 value I remember. I recall it seeming quite fast, but I guess it's all relative.

We have got results we're pleased with. We don't have to deal with anything as intensive as flood cooling, and we don't feel like milling something takes too long (setup and tool zeroing still dominates the time spent on the mill). With a 1/4" tool, we usually wouldn't cut anything thicker than 1/4" alu plate at that speed. Stuff on the 1/2" or larger scale we would use a larger cutter (1/2" or something) and probably even do in multiple passes, depending on the geometry and the tool. With 3/16" tools or smaller in 1/4" or even possibly 1/8" material, we'd take multiple passes too, just to be safe.

Since others have shared their advice about cutting faster (in the 20-60 IPM range), I'll definitely make a point of trying it. Cutting faster is always good, as is better tool life, etc. Since we do make good chips and cut quickly enough for our tastes at our current speeds, if we don't have success with the higher speeds, we'd be happy going back to what we're more familiar with.

Thanks to everyone for their experience and suggestions. I'll post again in this thread when I get a chance to experiment with the speeds on our mill.

Re: CNC Tooling
 

Roy,
I just down loaded ME. This looks to be a great tool and I plan to show it at work. Thanks
I have been watching this thread and there are a few things I would like to add.
• When using double face tape, make sure everything is clean before applying the tape. Test to make sure that the coolant will not attack the tape.
• If a mister is left unused for a while it should cleaned before use. They can build up a mold and the next time it is used it will become air born.
• When it comes to cutting aluminum, stay away from any coatings that are gray to black. They are TiAlN (Titanium Aluminum Nitride), AlTiN (Aluminum Titanium Nitride), and TiAlSiN (Titanium Aluminum Silicon Nitride). Aluminum will stick and nasty thing will happen.
Another CAD/CAM package to check out is BobCad. They have sales every so often. We purchased 2 seats of mill and lathe for $1,500.

Re: CNC Tooling
 

I evaluated BobCAD/CAM (along with half a dozen others) and I can't say I'd recommend it based on my 2 hour demo of it. The UI and workflow seems primitive and complex compared to some other software packages. Also, once contact is initiated, be prepared to deal with their relentless sales force. You're basically on their contact list for life at that point, and you'll hear from them at least twice a month.

Re: CNC Tooling
 

It really is a great tool to have on your desktop. Simple and effective.

Re: CNC Tooling
 

We used HSMXpress last year for all our milling and worked for everything that we needed it for (pocketing, countersinks, bosses, contours, etc.). You provide your email address in exchange for their free version (HSMXpress, HSMWorks is their paid version). I think they emailed me once if I was interested in HSMWorks and haven't contacted me since. It's a pretty easy to use package with really good Solidworks integration. They were purchased by Autodesk a bit ago so they're working on an Inventor version.

One of the good parts of having a plug in program into your CAD program is when you do rev's they'll automatically rebuild into your CAM program so that all you need to do is re-post it for your G-code.


The 1/4" EM was definitely our workhorse last year and when we were newbs at it, we'd have it cut with the tip of the EM (broke a couple EM's). I later on predrilled a lot of the paths with a 1/4" drill then entered maybe 1" into the material using the top of the EM closer to the tool holder. It's all about balancing heat, your tools, your fixturing, and your machine. You'd be surprised how much you can push your tools with the HP/revs you have.

Re: CNC Tooling
 

OK, so I finally downloaded ME Consultant, and I'm not sure that I'm understanding what I am seeing. The Help file doesn't open for me.

Referring to the image, can someone confirm for me that with the parameters shown (1/4" 4-flute HSS endmill cutting 6061 to a depth of about 1/8"), I should cut at about 72 IPM?

What do "Spindle %" and "Feed %" mean? I don't understand the percentage.

==============
On the topic of cooling, I went to Harbor Fright and bought an airbrush gun for $10. I ran the brush at about 20 PSI and it sprayed a nice fine mist of water (my test fluid), which I could vary from barely a mist to almost super-soaker level. The air action should blow away the chips from the cut, and the coolant will, um, cool it. I'm going to buy a gallon of Koolmist 77 from McMaster and see what it'll do with a scrap block of aluminum.

Re: CNC Tooling
 

Those are reasonable numbers. I don't know what the % means, but I'm guessing you modified the spindle speed and left the chip load as they recommended it? It probably means that 10,000 RPM is 197% of the default speed it would recommend.

Re: CNC Tooling
 

Hi Don,

The manual is a standard windows help file. Try opening in another computer or I can print it out for you and send a pdf.

Snipped from the help manual


Spindle Efficiency is the percentage of the power produced by the machine spindle motor that's actually available to a cutting tool. For machines in good condition, this figure is normally in the 80% - 90% range.

When Feed % (feed override) is changed, feed outputs, machining times, material removal rate, and power requirements are recalculated.

The maximum value allowed for Feed % is 300.0

When the override is below 100.0, the Feed Reset button is blue. When exactly 100.0, the button is white. When above 100.0, the button is red.

Re: CNC Tooling
 

Yup, I normally see around 300-400 SFPM as the suggested range for HSS end mills in 6061. In their database they're using 334 SFPM as the 100% (recommended) speed, and you're at roughly double that if you're running 10k RPM.

It's easy enough to look up the recommended numbers from your end mill manufacturer - here's Niagara http://www.niagaracutter.com/techinfo/index.html

As previously mentioned, I wouldn't suggest trying to slot with a 4-flute cutter in aluminum, especially with just mist. Any problems with chip evacuation (caused worse by increased heat - higher SFPM range) and the cutter is going to load up with aluminum and snap.

Carbide and fewer flutes (1 flute onsrud) solves those issues. At the very least you should reduce the depth of cut a bit so that the chips are smaller and can get out of the slot easier. Probably still have to babysit it and blow chips out of the slot manually.

Re: CNC Tooling
 

Agreed. Doing just a little online research yielded This Page, which (although quite long) helped me understand the issues I am facing. Boy oh boy, this is different from my ancient manual machines! But now I feel prepared to start experimenting in aluminum. With some 'used' end mills, so when they break I won't feel so badly.

Re: CNC Tooling
 

BobCAD is extremely aggressive about sales.
A bit too aggressive at times.

I find there interface a bit old fashioned in visual style but I have found that depending on your perspective of the CAD/CAM/CNC workflow BobCAD can be great product. I own a few versions with and without dongles.

There is unfortunately a learning curve.
I had the same trouble the first time I used it.
Once I got the hang of it things went smoother.
I could never have made due with a 2 hour demo either.

Does this not depend on the speed of the spindle?

Usually you have to spin the TiAlN end mills at higher speeds to make the coating operate as intended (18k to 22k RPM).
You would not want to use a TiAlN end mill too slowly or it will be worse than an HSS end mill.

Then there's the other issue, the higher the spindle speed the higher the IPM you need to move or risk rubbing. Not a problem for good machines but a problem for light weight gantry mills.


Generally and not in reply to anyone:
I linked this in a topic in the motor section but I will link it here as well:
http://blog.cnccookbook.com/2012/03/...tting-success/
Props to scottandme for posting a reference to G-Wizard as well (last page).

The issue I have with this topic is that I suspect that the different teams have different CNC machines.
A servo driven bridge or turret mill will have different requirements than a stepper driven gantry mill.
The bridge or turret has greater rigidity.
Depending on the spindle operating range it will impact the IPM.

It is hard to pick out what machine is what.
Some of the machines might be using steppers and therefore must target lower IPM feeds.
Some of the machines might have less cooling.
Some of the machines might have higher speed spindles with no ability to go slower.
The key elements that make this work depend on the knowing the machine sore spots.

For example:
I assume the mill in question is a turret type like a Bridgeport?

At this link...
http://www.daycounter.com/Calculator...lculator.phtml

Plug in 0.25", 300SFM, 3 flutes.
You get: about 4,500 RPM, 27.5 IPM
Makes sense that this works.

Plug in 0.25", 1,310SFM, 3 flutes
You get: about 20kRPM, about 120 IPM
This is probably not going to work.
I would be a bit suspicious of a carbide end mill rated at 1,310SFM uncoated.
Even more suspicious if your router can sustain the feed rate to keep it from rubbing.

At a spindle speed of 20kRPM I think you should consider a TiAlN end mill for the router with 2 flutes and 1/8" diameter.
That would get you:
655SFM, 20kRPM spindle speed, 80IPM feed.
If your gantry mill is outfitted with either really powerful steppers or servos it will work.

Try this:
http://www.wttool.com/index/page/cat...lls+%28USA%29/

Otherwise if you can't get the power from the steppers on your gantry:
Use a single flute as others have suggested and you'll divide that feed rate in half.
At that point if it's not enough edit your depth of cut and tool path to accommodate.

Re: CNC Tooling
 

Anything with Al in the coating will not work to cut aluminum. Mainly for chromoly steels, stainless, titanium, nickel alloys, etc. They need high temperatures to "activate", which requires high SFPM numbers. From what I understand it actually creates a thin film of aluminum oxide when it hits that activation temperature. That's purely dependent on the size of the cutter and the material - but 18 to 22k is pretty extreme for a VMC - that's a specialized machine. Most are in the 8k to 12k range give or take. Generally with those cutters they don't use coolant (same with many carbide/ceramic insert cutters), just a heavy air blast to clear chips. The coolant can cause the insert to fracture from thermal shock.

For aluminum you either want uncoated, ZrN, or TiB2. TiCN can work well, but avoid TiN. Most major brands make geometry specifically for cutting aluminum (higher helix, polished flutes, etc, etc).

Re: CNC Tooling
 

So you are basing this on the VMC (Vertical Milling Center) not being able to obtain those high spindle speeds in general?

What if they are using a standard shop router(19kRPM - 25kRPM) or a RotoZip (15k-30kRPM) for a spindle on a homemade gantry?

Course the price they pay is not just for the coating it's also that they will need a high feed rate.
A high feed rate most smaller steppers would have difficulty achieving.

I agree with you if you slow down the spindle and operate more in the range of 8k-12k TiAlN is the wrong coating to use.

Without knowing what sort of machines each team is trying to use it gets a bit more involved.

Re: CNC Tooling
 

We use BobCAD/CAM at work. It was a program we picked up in the spring to potentially use for robotics and potentially replace our current software since the yearly license fees were getting crazy for two seats. We have a few licenses with the goal that one will be on a machine at the school so the students can design parts and make the g-code to cut out a lot of the time that was spent manufacturing parts by the small staff available to work on parts for us.

We hear from those guys once a week every Monday (going to be awaiting their call tomorrow morning!) and while yes it is annoying they give us great deals on new software as well as amazing discounts on software we purchase additional seats of so its annoying but really nice. Their training staff is also great! Met a few of them at Eastec this year and they were very friendly and informative!

As for the program itself it took me a while to get the software down since it was my first experience with a creating tool paths but I went through their DVD instruction videos and from there on a little practice makes perfect. If their is one thing I wish they did better it would be their pan/zoom/rotation. Oh well.

On the brighter side it has been very easy to use on various machines in our shop that run on differing controllers which has been a good plus!

For FRC purposes I would see if you can talk to company to get the software for free.

Re: CNC Tooling
 

1300 SFM is perfectly reasonable for uncoated carbide. Most vendors will recommend 700-2000 SFM for a carbide end mill with aluminum specific geometry.

TiAlN, AlTiN, and TiN are always bad for aluminum. They have an affinity for aluminum which leads to galling, causing your end mill to load up and break.

While you are correct that TiAlN and AlTiN are designed to perform best at elevated temperature, you could never even get them to that elevated temperature in aluminum as you would have to run without coolant and you would be guaranteed to melt your chips and pack the flutes long before getting up to temp, completely disregarding the fact that these coatings are not advisable in aluminum due to their physical properties.

Re: CNC Tooling
 

There are plenty of different coatings available if you look through a major supplier catalog. All different geometries and designs for different materials, as well as several different coatings. For aluminum - regardless of machine, TiAlN is a bad choice. The aluminum will have an affinity for the Al in the coating and will gum up. For aluminum geometry you generally want a high helix angle to help chip evacuation, a large gullet to allow plenty of space for the chips to eject, and a sharp cutting edge. Coatings that work well in aluminum are ZrN, TiB2, and TiCN. Uncoated works perfectly fine as well. Generally they make the surface harder and smoother to prevent the chips from welding to the surface of the tool. With aluminum coolant is normally used to help eject chips, add some lubricity, and keep chips from welding to the surface of the tool.

For a router in particular - the best option is using a carbide single flute tool. Carbide can run high SFPM numbers in aluminum, so that way if your router is 8-10K minimum speed you won't be burning up the tool. Single flute does two things well. Firstly, it gives a ton of room for the chips to evacuate so that they don't pack up in the gullets of the end mill and cause the tool to load up with aluminum, stop cutting, and snap. The second is derived directly from the speed and feed formulae. Say each tooth needs to be taking 0.002" per revolution so that it doesn't start "rubbing" as opposed to cutting. If you have one flute, that means you're only moving 0.002" per revolution of the tool. If you have a 4 flute tool, each tooth needs to take a 0.002" bite, so you have to move 0.008" per revolution of the tool to maintain proper chip load. On a router that can be the difference between a manageable feed rate, and something that the machine cannot achieve.

For example - you have a router that can vary from 10K to 20K RPM and you're using a 1/4" end mill to slot.

I would use a single flute uncoated carbide end mill. Depending on the specific tool, SPFM in 6061 can be anywhere from 800 to 2000 SFPM. You can run slower, but running fast will wear the tool prematurely. A 1/4" tool running 800 SFPM is 12,200 RPM. Perfect, right in the range for our router spindle. Now finding the feed rate is just (spindle speed * # of flutes * chip load). Say we're being conservative and taking 0.002"/tooth. That means our feed rate is only 24 inches/min. Any machine on the planet can do that without worrying about acceleration in curves, angle changes, etc. If we want to go faster, we can bump up to 20k on the spindle (~1300 SPFM, likely fine for carbide), and the feed rate jumps up to 40 inches/minute. Perfectly achievable numbers, the tool isn't going to burn up or rub, and we have a ton of room for chips to jump out (only one flute!).

If you like 1/8" end mills, then you can run 24 IPM at 12,200 RPM (0.002"/tooth and only 400 SFPM), or 40 IPM at 20k RPM (0.002"/tooth and 650 SPFM).

Using a two flute cutter doubles those feed rates while keeping the spindle speed the same. Three flute triples, and so on. But now you have increasingly little room for the chips to evacuate, especially with a smaller 1/8" end mill. Your previously reasonable 25-40 IPM feed is now up to 100-160 IPM on a 4 flute tool, and you'll need to be taking a shallower cut if you run out of HP in your spindle.

As for the first part - TiAlN is perfect if the situation is correct. Here's Niagara's chart: http://www.niagaracutter.com/techinf...d_solcarb.html

Say we're cutting 300-series stainless (over 32 rockwell C). We would probably want to be using an air blast to clear chips, and let the coating do the work. We need to coating to heat up to work properly, so here we don't want to be under the recommended SFPM numbers.

So say a 3/8" 4 flute end mill - chart reads 100-150 SFPM and 0.001"/tooth. TiAlN coating adds 60-100% increase in SFPM. So we're somewhere between 160 and 300 SPFM. Let's use the high end - that gives us all of 3,000 RPM and 12 inches/minute. That's why most big VMC's don't really need insane spindle speeds unless they're running aluminum, copper, brass, etc. Even with the coatings, most jobs in steel, stainless, titanium, etc aren't going to going that fast. After that you'll have to start reading about HSM and radial chip thinning, etc, but that's way beyond the scope of this.

Re: CNC Tooling
 

Well I am confused then.

Cause I not 7 days ago used a TiAlN 1/8" end mill, 2 flute on aluminum.
With coolant and it was hardly a new end mill for that purpose.
I am not the only one either.

So I guess the question I have is at what operating temperature is this coating appropriate?
Since the question here appears to come down to whether or not it can reach that temperature.


Answering my own concern:
I have a long commute so I decided to call around to Duramill and Niagara.
Spoke with the technical folks not sales.

The reason the coating operating temperature is not specified is apparently because they consider the TiAlN coating inert.
It shouldn't want to bind chemically to aluminum any more than Titanium (no affinity according to Niagra).
The coating provides hardness and durability till the yield temperature well over 1,000 degrees Celsius.
This differs from aluminum titanium nitride which is high in aluminum and therefore is an active coating.

The issue they clarified is that aluminum will of course melt well into the safe operating temperatures of these bits.
So you don't have to hit a certain temperature to make them work.
However just because the bit will withstand these temperatures does not mean the aluminum you are working won't melt and wet the bit.
Obviously once the aluminum melts and wets the bit welding will soon follow.

The reason my machines are not experiencing that issue is because I do not cut aluminum without coolant.
Therefore I am cooling everything.
I do not consider the cooling to be really heavy duty so the bit does get hot.
However the aluminum being worked is basically a heatsink and the coolant cools that.
The gantry mills I have used TiAlN with are pretty rigid. I have seen much worse.
Also I am aware that aluminum tends to melt so I take measures to keep moving.

This is why there is no minimum desirable operating temperature specified.
This is also why it works for me.
I told both companies that I've used these with aluminum and no huge red alarms went off.


However I still agree a slower spindle is desirable for this purpose.
It would eliminate the need for the tool that could be a bit more expensive.
Additionally it would reduce the risk that a slow cut would weld.

Re: CNC Tooling
 

Michael, my team has a Techno LC 4896 (I'm 90% sure this is the model). Last year, all of our metal work was cut on this machine, running it sometimes for around 12 hours straight. The stuff that you need, in my mind is:

• 1/8" End Mill Bit that can cut metal
• 1/4" End Mill Bit that can cut metal
• Vacuum table to hold material down flat
• Sacrifice Board
• Metal Screws and such to attach the material to the sacrifice board
• Coolant (we used mist coolant, not sure the brand or anything else. I can get back to you on that. I see that your Haas TM-2P is made for flood coolant)
• CAM software, we used Mastercam last year with success. Our new Computer Integrated Manufacturing teacher has switched us over to EdgeCAM, we'll see how that goes
• Someone with experience. If you get wood-cutting bits (1/8" and 1/4" are fine), which I would recommend getting for training, have someone use the machine all first semester as much as possible to learn it and learn some of the shortcuts and such on the machine

That last one is big, even though it doesn't sound like it. The more people you get to use it during the offseason and the more hours that you have people working it during the offseason, the more parts you will feel comfortable with being cut on it. Also, the more people you have on it, the more efficient your team can be in cutting on it, since one person could run the machine, and the others that can CAM will be making the tool paths.

If anyone has any more questions feel free to ask. I haven't read through the entire thread as of right now, but I'll try to get to it.

Re: CNC Tooling
 

What did you do for your vacuum set up? Our team made our vacuum from a board with a ring cut around it for a o ring like thing, then we used 2 shop vacs to pull the material down. We've had some success using it with plywood, but we just can't get aluminum to stay still.

Re: CNC Tooling
 

Our cnc's vacuum table came with it from TechnoCNC. However, your set up sounds like it should work. Ours has recently had problems holding materials down, but this is where the screws come in. The screws hold the aluminum to the sacrifice board and the sacrifice board gets sucked down holding the aluminum with it. When that doesn't work, like it sometimes doesn't, we have had two options, which work best in combination. One, you can cover the extra spots on the sacrifice board where the material isn't with papers in plastic sleeves. This makes it so that the table isn't trying to suck down air, lowering the pressure. Instead, it is all sucking down the material, holding the pressure. The second option, which is a lot more fun, is to sit on the material. This pushes the material down to the table and the table holds it down afterwards. The other thing we do is turn all of the valves off on ours when we turn it on, and one by one turn the valves to open the vacuum at different spots on the table where our material is. I have also heard that using tape around the sacrifice board and material will help, but I haven't tried it yet.

Re: CNC Tooling
 

I'm surprised that they said that - I've heard plenty of people having issues when they tried to run TiAlN in Aluminum and had issues with build up edge forming, surface smearing ruining the finish etc. Could have been your cut parameters being moderate enough that it wasn't noticable, or the cut was generating minimal heat (quite likely with a small 1/8" end mill). I guess best case you're paying a decent amount of $$ over uncoated without an appreciable benefit compared to other coatings.

Either way - the proof is in the products that they sell. Duramill and Niagara don't put that coating on their aluminum-specific end mills. They both sell either uncoated or TiCN coating on those tools. They're both a bit behind the curve on aluminum coatings it seems, since ZrN and TiB2 are being used in many other mfg's high end aluminum products. We've used the Niagara aluminum specific end mills with TiCN since McMaster sells them and it's convenient (AN3xx series). They work well, but I can't speak to if they're appreciable better than uncoated - we don't push our machines that hard and they're not being run 24/7 to notice any difference in longevity.

I have never seen anyone sell an aluminum specific end mill with TiAlN on it - uncoated, TiCN, ZrN, TiB2, and DLC are the only ones I can remember seeing. I've also never seen aluminum as a recommended material for TiAlN or AlTiN.

It doesn't really matter - you want to run carbide with smaller cutters. For one, the price difference is usually minimal compared to HSS. Carbide is significantly more rigid that HSS, which is especially helpful for small diameter cutters. And even uncoated carbide has almost no speed limit in aluminum. Cuts weld if the SFPM is too high, chip load is too low, or the chips aren't being ejected from the cut. So to fix the first you use carbide, to fix the second you use a single flute cutter so you can maintain proper chip load at lower feeds, and that also fixes #3 by giving room for chips to eject.

If it's on a mill and not a router, then you still want to use carbide if only for the rigidity benefits.

Re: CNC Tooling
 

If you have a choice you would never use TiN, TiAlN, or AlTiN in Aluminum. If it was all you had, you could use it without immediately destroying your end mill. All the things Scott said are true though, regarding surface finish and BUE. You can definitely notice the latter occurring.

If you tried to run one of those end mills under aluminum specific parameters (1000+ SFM, .003"+ chip load) you will load it up and break it-guaranteed. This is as much because of the geometry being wrong as it is because of the coating, as the only tools that are ever coated with those are meant for ferrous materials.

I'm not sure why they told you that you don't want to run the tool at elevated temperatures. I forget where it is exactly, but somewhere between 700-800C the coating dramatically increases in hardness. As previously mentioned this is why people don't cut ferrous metals with coolant when using those coatings.

Re: CNC Tooling
 

Not so sure about the $$ I paid < $10 for those 2 flute end mills including shipping and handing quite some time ago. In a production operation with various tool paths I can't say I consider that expensive.

I called both because I was curious if one would say the opposite of the other. I've never experienced the issue you have.

I did expressely mention that other people were telling me they were having issues with TiAlN in aluminum and they both stated it depends on a lot of factors like the feed rate, the coolant, the rigidity. So your mileage may well differ from mine.

I can't say that any of the TiAlN coated end mills I've used expressely stated that they were designed for aluminum. I don't necessarily use a rule of thumb for setting up for aluminum either. However I can't really say that router typically used for wood or a RotoZip was really designed for this purpose either. I don't use TiAlN coated end mills unless the RPM of the spindle is for some reason high and I can't adjust it down.

Most of all these bits with TiAlN coating are carbide inside anyway so I agree this is one of those little things.
The core advice is still the same.

Well if you try the calculator on the page I linked before:
1,000SFM with an 1/8" mill gets you a spindle RPM of around 30,500 RPM.
With a tooth load of 0.003 and 2 flutes you get: about 183 IPM feed rate.

I have a lot of people I've worked with that only dream about 183 IPM feed rates their systems could not achieve that.
They would be missing steps.

If you increase the diameter to 1/4" you'll get down to about 15k RPM and 91 IPM or so that's more practical for large steppers and closed loop servos.

There are many studies on TiAlN here is one that specifically mentions 800 degrees Celsius.
http://www.geocities.ws/sarangrh/report/seminar.pdf

Further we can ask a company that does coating what they recommend:
http://www.pvd-coatings.co.uk/coatin...tialn-coating/

Though I never try to machine aluminum without coolant.
It does not specifically say you'd want to machine aluminum dry.

Niagara Cutter 86002 Carbide Square Nose End Mill, Inch, TiAlN Finish, Roughing and Finishing Cut, 30 Degree Helix, 3 Flutes, 1.5" Overall Length, 0.125" Cutting Diameter, 0.125" Shank Diameter

Niagara Cutter A245 Carbide End Mill for Aluminum, TiAlN Coated, 2 Flutes, Square End, 4-1/8" Cutting Length, 1" Cutting Diameter

http://www.drillmex.com/img/PDF/NIAGARA/A245.pdf

Re: CNC Tooling
 

Thanks! We'll try this next time.

Re: CNC Tooling
 

Shop vacs are low pressure, high flow. Really not even close to ideal for a vacuum table.

We got a surplus vacuum pump from a mentor we've been using (looks like a large old KOP thomas compressor) for a small table. I know do do anything of meaningful size you need something decent and beefy.

I'd try to find someone local in industry with knowledge in routers (cabinet shops often have some HUGE ones) to point you in the right direction, it can be a tough thing to google if you don't already know what you're looking for.

They'll also give you great tips all around on how to run the machine, what to fixture with, etc...

Re: CNC Tooling
 

"It might work" isn't the same as saying it's a recommended coating. If you call and ask "What tool coating is preferable for machining of aluminum?", they will not respond by saying TiAlN. That's why they don't sell it as a coating on their aluminum specific geometry tools, just uncoated or TiCN. Other companies run coatings designed for Aluminum - ZrN, TiB2, DLC, etc. Niagara and Duramill don't offer those for whatever reason, but SGS, OSG, Havey Tool, Melin, Maritool, Destiny, Lakeshore Carbide, etc, etc all do.

Again, conflating routers and mills here. For routers - use the Onsrud single flute carbide cutters. They solve all of the issues with having high minimum RPM and limited feed rates and acceleration profiles. 1/8" end mill - 20,000 RPM @ 40 IPM. 1/4" end mill - 20,000 RPM @ 60 IPM. Doable on any junky stepper machine.

If the feed is too extreme for the router, just drop the spindle speed. If you're cutting aluminum on a router you should really skip the silly hand routers and buy a model with a VFD controlled spindle anyway. Good uncoated carbide is perfectly happy at 1,000 SFPM and up.

For mills - you're going to be spindle speed limited in aluminum on most cutter sizes, but they're able to maintain higher feeds without issue. Even the Haas TM machines are rated for 400 IPM, and that's still plenty considering the machine size/HP.

Your feeds will be much slower just based on the max RPM for the machine. 1/4" 3 flute end mill - 6000 RPM, 54 IPM @ 0.003"/tooth. 1/2" 3 flute end mill - 6000 RPM, 90 IPM @ 0.005"/tooth. You will probably get higher MRR at lower RPM just because the HP falls off on the Haas machines at higher RPM's anyway.

Not exactly the most reputable site. Find any cutting tool company that recommends TiAlN for aluminum. Find any cutting tool company that sells aluminum specific geometry, and see what coating they put on the tool. It's not TiAlN.

Re: CNC Tooling
 

In fairness I just added the links for that exact product offering from Niagara to my post above. So you probably didn't see that when you posted this.

Again look up at the end of my last post. Niagara sells those bits with TiAlN coating specifically for aluminum. So let's not so hastily assume that the coating company I linked is also self-promoting.

Here:

Niagara Cutter 86002 Carbide Square Nose End Mill, Inch, TiAlN Finish, Roughing and Finishing Cut, 30 Degree Helix, 3 Flutes, 1.5" Overall Length, 0.125" Cutting Diameter, 0.125" Shank Diameter

The end mill above led me to the end mill below...

Niagara Cutter A245 Carbide End Mill for Aluminum, TiAlN Coated, 2 Flutes, Square End, 4-1/8" Cutting Length, 1" Cutting Diameter

Which gave me a reference to search for this...

http://www.drillmex.com/img/PDF/NIAGARA/A245.pdf

Here's the 1/8" TiAlN end mill for sale as factory stock:
http://www.kaufmanco.com/itemdetail/NIA%2061489

Parting that series at the same distributer:

61351 = Uncoated = $13.98
http://www.kaufmanco.com/itemdetail/NIA%2061351

61443 = TiCN = $24.21
http://www.kaufmanco.com/itemdetail/NIA%2061443-030

61480 = TiAlN = $15.63
http://www.kaufmanco.com/itemdetail/NIA%2061489

Re: CNC Tooling
 

The first EM listed isn't for aluminum. No idea about the second one. Looks like you found an outdated catalog page from a French tool supplier. Note how TiCN is the one highlighted as "recommended".

Here's the real A245 catalog page from Niagara's website in case anyone else is interested (uncoated or TiCN only). We've used the A345 (3 flute) with great success, they're good quality end mills.

http://www.niagaracutter.com/solidca...um_ss/a245.pdf

It's pretty clear you have your mind made up and don't want to listed to what Cory and I are saying. For anyone else following this boondoggle - here's what I would recommend.

Using a router? Buy Onsrud's singe flute cutters (63-600 series) - McMaster under "Router Bits for Aluminum" (ex PN 3317A21, 3317A25).

Using a mill? Check out Maritool (Uncoated, ZrN, DLC) or Lakeshore Carbide (ZrN). McMaster sells the TiCN Niagara tools (High-Performance Carbide End Mills for Aluminum).

http://www.maritool.com/Cutting-Tool...201/index.html

http://www.lakeshorecarbide.com/vari...raluminum.aspx

Re: CNC Tooling
 

Considering that you are basically telling me I am not doing what I am actually doing? Yeap.
Even your own link points to the same part numbers.
Even if you want to say they don't make these any more you wrote they did not make them at all.

Never said TiAlN was the only option. Go back and look. Don't much like people assuming I did when there's no evidence to support the claim. None the less I will once again agree with you with the right machines these are perfect tools.

I *only* use TiAlN mills with specific circumstances and *never* suggested otherwise.

I am very disappointed in the way you are reacting to this.
However it is utterly irrelevant to the fact that it does work.

Before it was implied that people were surpised that Niagara would suggest the applicability of TiAlN even though they don't sell it well that can't be a fact.
If you simply look through the Niagara price list the TiAlN end mill part numbers are still very much in there.
Both the PDF and the ASCII price list dated January 7th, 2013.
Old or not they obviously have experience with this coating on aluminum.

Now if I were in Niagara's shoes and I was selling a product that a whole bunch of people made a directed effort to dismiss I would probably shelve it as a matter of business as well. Regardless of the product quality or track record if enough customers simply decide it is not for them the volume of sales would plummet (like what would happen if a bunch of people kept going after people over it...sort of like what people often do to BobCAD and MasterCAM). It sure seems like this is a little too much peer pressure for a simple matter like this. So I guess I know why Niagara outright said to me it's just not worth worrying if they disagree. I haven't even bought these products from Niagara so I guess this is an issue they've had pushed on them before.

Besides on their actual page:
http://www.niagaracutter.com/news/fall99/

Maritool also has this:
http://www.maritool.com/Cutting-Tool...duct_info.html

So on this I agree to respectfully disagree.
Frankly I just get paid too much to sit around worrying about whether TiAlN is acceptable to anyone.

http://www.emastercam.com/board/inde...howtopic=33219
http://blog.cnccookbook.com/2012/03/...tting-success/ (list item #3)
http://www.practicalmachinist.com/vb...-tialn-121066/ (note the top post and who)
This little game of cat and mouse has after all been played out over and over.

Re: CNC Tooling
 

This thread inspired me to try to push my endmill a little harder on a big job I'm doing the first run of.

Lakeshore Carbide 1/4" carbide square corner 3-flute variable helix ZrN coated.

HAAS Mini Mill @ 6000 RPM. Flood coolant.
Cutting .2 deep, 20% stepover.

It's loving running at 144 IPM. If I had a 12k RPM spindle, I'd probably be able to run it at 300 IPM.

HSM toolpaths really do wonders.

Re: CNC Tooling
 

I love to see how passionate the FIRST community can get. Some time we all need to step back and look at who our customers really are. This thread has advance well above 99% of our customers and it still does not cover all of the parameters to be safely successful. Coatings are just one of many. There is still machine, work piece, and work holding rigidity that has not been addressed.
I have included a picture to show what may happen when something is not right with set up ,speed and feed , and or coating.
If I remember right, we were cutting 2024 aluminum running the spindle around 8k with a ½ carbide ball end mill with TIALN coating. Feed rate was around 80-100 ipm and we had a 6 nozzle halo coolant at 75 psi. Everything was fine until the machinist started to hear things hitting the enclosure. As long as the cut was in the climb direction it was fine. There was a section, in the program, where it started to slot out a groove. That’s when thing went bad.
If we were setting up a high volume operation there is some very good information here. In FRC we may make 10 similar parts. Look at the cutter and machine recommendations and start safe. My biggest fear is someone takes a portion of the information and gets hurt.
On the subject of vacuum chucks, make sure the work piece is also blocked to help keep it from moving. If you are using coolant there needs to be a filter between the chuck and the pump. If fluids get into the pump it may lock up.

Re: CNC Tooling
 

I found this free feeds and speeds calculator. I'd been looking for a while, and have no idea how I didn't come across this sooner: http://zero-divide.net/

They have an Android app too.

From my preliminary tests on it, the numbers it generates looks good for milling.

For drilling, with a regular uncoated HSS 1/4" drill in 6061, I'm getting about 4900 RPM and 40 IPM. Does that sound right? I've been running much slower than that, and would be thrilled if I could drill this fast.

Re: CNC Tooling
 

4900 RPM and 40IPM are doable. Now we need to add the rest of the parameters. This will work for a CNC not a drill press. Flood coolant is a must. The deeper the hole the shorter the peck depth. If the chips are long and stringy, shorten the peck depth to get them to fly off the tool. If the chips will not fly off, find out how to stop the machine and spindle in the middle of a program. Clean off the chips and restart.

Re: CNC Tooling
 

I forget the rpm, but we run a #7 drill (.201) at 30 ipm on our router all day long without issue.

Re: CNC Tooling
 

I tried the FSWizard suggestion of 4968 RPM and 40IPM for the 1/4 inch drill and it worked great. Nice chips. This saves me SO much time!

By the way, I really like this very technical thread. Back in the day, we had a lot more of this sort of thing here on CD.

Re: CNC Tooling
 

I agree we're above the 90th percentile in this thread, and lots of topics are not yet covered...but perhaps there's a teachable moment here: Not every topic can be covered adequately in a Chief Delphi thread.

My personal approach is to get a basic idea of what I don't know (from here) and go out on the Internet and research it in great depth. I never trust one source on the web, I always need verification from an unrelated source. Books are great for this, since there is usually a vetting or verification process - call it a reality check - before someone commits to setting 10,000 copies onto paper.

Once I know enough to be dangerous (meaning I think I know enough), I start actually applying what I have learned, take careful notes, and figure out what went wrong. I find the edges of the envelope by fiddling until something 'breaks' and then remember to not make the same mistake.

Once I buy my Onsrud upcut bit (63-620) I'll be breaking using it in some scrap aluminum, and eventually figure out what doesn't work. But to start, a conversation with Onsrud helped me set the 'middle of the road' parameters so I can start safely. Then, always making sure my valuable hide is well-protected, I'll push the edges and see what I can learn.

What I learned so far: SFM is important, so consider RPM and bit diameter to get this right. If your tool can't go slow enough, decrease flutes until SFM is in range. Then set movement to get the recommended chip load. Set depth to manage tool deflection, and you should be good. Be sure to consider cooling and be sure chips are cleared fanatically.

Safety, including workholding, is not optional. For me, full face shield (I want to protect my nose and teeth, too...), and ear protection. Lots and lots of hold-down clamps. Slow and steady progress, triple check everything. Dry runs (on a CNC) to verify no problems. And the dog stays upstairs for all this.

Re: CNC Tooling
 

Good conclusions all.

Just a quick clarification - SFPM (surface feed per minute) is independent of the number of flutes and tool diameter. It's more of less the equivalent of tangential velocity - how fast should the edge of my tool be moving as it spins (feet per minute). This is the starting point for speed and feed calculations.

N = SFPM * 12 / pi * D

Where:
N is Spindle Speed in RPM
SFPM is in feet/minute
D is tool diameter in inches

The 12 is just a conversion factor to make the SFPM into surface inches/minute so that the tool diameter units work.

Remember that it isn't a problem to lower the SFPM, it's essentially a measure of how much heat the tool/coating can tolerate. No aluminum coatings are heat activated, so slower is fine. The onsrud tool is uncoated/polished carbide.

Then you plug your RPM (N) into this formula to find your feed rate.

F = f(t) * n(t) * N

Where:
F is the feed in inches/minute
f(t) is the feed per tooth (or chip load) in inches/tooth
n(t) is the number of teeth/flutes
N is spindle speed in RPM from the previous formula

This is where you see the benefit of the 1-flute. It allows you to have a high spindle speed without needing to increase the feed rate. Perfect for routers where there are normally high RPM minimums (unlike CNC mills), with limited capacity for high feed rates. n(t) comes from the manufacturer recommendations - too low and the tool "rubs" as opposed to cutting a clean chip, too high and the tooth fails from high load.

After that you have your spindle speed and feed rate, the only parameters left are to determine the cut width and depth. For slotting (full tool width cut), the rule of thumb is 1/2 the tool diameter or less. You might also want to check the cut to make sure it's within the HP limit for your router, as well as the rigidity of your machine.

I like the calculators on this site, although if you know the formulae it's easy enough to just make a little excel sheet for everything. They do speed and feed as well as HP/Torque calculations (can normally get the HP/Torque curve charts for your router from the mfg).

http://www.custompartnet.com/calcula...speed-and-feed

Re: CNC Tooling
 

Hey - this is a little unrelated to the rest of the thread but I would appreciate some input. I bought a Bridgeport for 1296 to use this season. It is in good shape and has a recent Centroid CNC kit. It came with the Eriksson NMTB 30-ish spindle. Had anyone ran across a good place to buy tooling?

TIA

Re: CNC Tooling
 

Part geometry effects feed rate do to cutter engagement. If we are cutting the outside of a box the cutter engagement stays pretty much the same. Now if we are cutting the inside of a box and the corner radius is equal to the cutter radius. A cutter engagement of 25% will jump close to 75% when it hits the corners. As a rough rule of thumb, anything over 50% cutter engagement drop the chip load in ½.

Keith,
Check out Enco or Tools4Cheap for tool holding and work holding. When it comes to cutting tools, check out a local cutter regrind shop. Some in our area have regrinds at a marked discount over new.

Re: CNC Tooling
 

I think this bit of advice should be highlighted.

With aluminum depending on the cooling in operation and the tool wear it's possible to have an operation that works just fine stand alone. Wrap that same operation in a larger more complex program and run into trouble.

You've got a tool that is hard and durable spinning in a material that can easily melt and flow. Stand the operation alone and you start with a nice cool part being machined with a nice cool tool. Come off a previous operation and the aluminum being machined is probably already above ambient and the tool is hot. Start to have problems in this otherwise successful operation and it might roll down hill into the next operation (potentially literally).

Slowing down risks operating the tool at a feed rate that will cause issues (for example rubbing). Withdrawing and/or stopping on the other hand removes that issue.

Plus if you have an ATC (Automatic Tool Changer) you can go for tool better suited for the operation or earlier in the tool's lifecycle. I do want to reinforce here for the sake of saftey that CNC machines often have no idea you are within their work envelope. An ATC lets the CNC machine change the tool. Always be aware of when there is software sitting somewhere waiting to move things.

I think that often times in production environment people are in a hurry to increase production. Fast spindles. High feed rates. Interesting coatings. All balanced of course with the math already presented to insure things are productive and pass quality control in the end. In that environment sometimes people just do not want to stop but as professionals you recognize the need when it happens. On the other hand, I think that while FIRST deadlines are tight they don't warrant rushing every single operation and just because a high IPM feed rate or fast spindle might be workable (say because you have a nice industrial quality VMC) or warranted doesn't mean you have to blow through every operation without halting.

Re: CNC Tooling
 

I also recommend Enco, and they run specials all the time for discounts and/or free shipping. Get on their mailing list.

That being said, if you know the manufacturer model number sometimes a Google search can find a less expensive supplier. Amazon often sells things less expensively than Enco.

If you are new to the milling world, get a set of plain High Speed Steel mills, and when you break one replace it with a 'better' one, maybe with a coating or made from carbide. I use 3/8" square end, center-cutting mills a real lot, almost exclusively, for almost everything - 2 and 4 flute. Ball-end also on occasion. The rest of the sizes are 'as needed'.

@Scott: What you wrote is what I meant. Yes, SFPM depends only on diameter and RPM. The part about fewer flutes has to do with chip load when faced with a high-RPM router. As you wrote.

Oh, and I am jealous that a McMaster warehouse is in Robbinsville.

Don

Re: CNC Tooling
 

On an semi-related note, I just discovered that one of my favorite vendors is carrying a line of aluminum specific HSS end mills that is 1/4 of the cost of the equivalent carbide tool.

I've never used these, but this guy doesn't sell stuff that isn't high quality, at a good price. Looks like a great alternative to carbide for many people with smaller/less rigid/slower machines, or those just learning that don't want to blow through a $50 end mill in one stupid mistake.

Re: CNC Tooling
 

At least for me that comes up with:
http://www.latheinserts.com/
Future home of something quite cool.
With a picture of a very "Magnum PI" tropical print shirt in a closet.

Works now....

Help: Recommended Tooling? Haas TM-1P
 

FRC Teams,

If you had a Haas TM-1P in your FRC workshop, what kind of tooling or accessories would you consider must haves?

Re: Help: Recommended Tooling? Haas TM-1P
 

It is not much of a 'what if' if you have the Haas TM-1P in your shop :]

Is it equipped with the Haas ATC?

If so you want the kit for the ATC:
6 ER32 collect holders for the ATC
6 size American sized ER32 collets (you probaby need to add to this)
4 Jacobs taper ATC holders (different sizes)

Note that the kit from Haas for some reason does not seem to come with a collet spanner wrench.
These collet nuts need to be tight you need the wrench.

Now additional tool holding you probably want some chucks for HSS drills (mill with ER32 collets not the drill chuck).
A set of HSS drills.

Some carbide end mills suitable for your work material.
So in that you probably will quickly consider:
ball nose, flat nose, center-cutting end mills
This machine has axis feed rates and spindle enough for more than 1 flute on aluminum so pick the tool with that in mind.
Consider your feed rates as well.

You also need a suitable work holder (aka vise).

Did you get the coolant kit?
If so consider what coolant you plan on using.
For example Hocut 795-CU or EcoCool S761 (Haas factory outlet has this).

How are you getting G-code to the machine: USB mass storage or drip feed (DNC)?
Do you have the necessary cables?

Re: Help: Recommended Tooling? Haas TM-1P
 

This is kind of hard to answer until you've actually started making stuff, or you know how much you have to spend-everyone's needs are different.

Certainly you'd want two vises. Kurt D688 is the go to here, with similar quality offerings available from Chick. You can find cheaper stuff, but the quality is hit or miss. That'll run you ~$1200.

You'll need tool holders. I would get 1/4" 3/8" and 1/2" set screw end mill holders, maybe 3 ER-32 and 4-6 ER-16 collet chucks, a keyless drill chuck, and a shell mill arbor. You can add more sizes as you need them. You'll definitely want more ER-16's than 32's as you will probably need more drills/taps than end mills, and almost every drill/tap you'd use is going to be under 3/8". Having a couple 32's is nice for bigger tools (up to 7/8"), but you can hold any end mills in the set screw holders as well. This should run you $1100-1300

A full set of collets (you'll also need to buy duplicates for some sizes so you can chuck drills and their corresponding taps that use the same collet) for whatever style you purchase. $300-500 depending on if you stick to one or two types.

Don't forget pull studs for the toolholders. They don't come with them. Haas sells them and 3rd party vendors sell them. Get the right kind and torque them properly. It makes a difference.

A quality #1-60, A-Z, 1/16-1/2 by 64th's 118* or 135* (more expensive) HSS bright finish drill index. No Chinese bits. Only ones worth buying are made here in America or in Brazil (by PTD). I prefer having jobbers (long) and screw machine (short) length indexes, but having just one would do. This could be $200 or twice that, depending on whether you get both lengths. Also buy like 10 of each drill for whatever clearance and tap drills you would need for your common bolt sizes.

A spot drill. Technically you want this to have a tip angle greater than that of the drill that will follow it, but I use 90* because the mental math to figure out the depth to drill to is infinitely easier.

Various assortments of end mills. This is really where you'll need to see what your specific needs are. I've recommended specific cutting tools previously in this thread and others for a variety of budgets.

A face mill that can cut aluminum/steel (might need different inserts for each). $100-200.

Two sets of reasonably high quality 1/8" thick parallels. $300 or so.

One or two sets of 1/32" thick parallels (important for parts where you have through features within 1/8" of the edge). Nice sets are going to set you back $200 ea. This was one area where I was willing to buy Chinese to save a lot of money on something we don't use often.

Soft jaws. "MonsterJaws" on Ebay sells fully machined 6"x3"x1.5" jaws for all 6" vises. 10 pairs for like $200 or so. Basically cheaper than machining them yourself.

A plain back 3 jaw chuck that you can either bolt to a plate and grab in a vise, or bolt to the table. Very useful for holding round parts. If you have a lathe you could get an adapter plate for your lathe chuck, so that you can hold it flat. Couple hundred bucks.

Coolant, as mentioned previously. Make sure it's a synthetic water soluble oil. Using something else can void your warranty. Probably going to be in the range of $130/5 gal.

indicators/edge finders/etc that you'd need for a manual mill.

Re: Help: Recommended Tooling? Haas TM-1P
 

The preference you have for the ER16 collets is it merely to get a smaller end on the tool holder so you can clearance into the work piece? Or is there another motivation?

Just a few general things I do:

I pour coolant concentrate into water, not the other way.
Also I tend to use distilled water the first couple of times I use a machine.
This way I know if I start using tap water if the tap water is causing problems.

Re: Help: Recommended Tooling? Haas TM-1P
 

That and you get less coolant loss due to misting after hitting the larger nose on the tool holder. It can also be tough to get proper coolant coverage of small/short tools while still covering your other tools due to needing the line to clear the nose of the tool.

Everyone should always remember this. OIL-Oil In Last. Never mix water into oil.