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?