CNC Feed Rate, and CAM software

[apples000]

So, our team is going to try making some parts on a CNC machine, and we were curious as to what speeds and feeds people have successfully used in the past. We are cutting a small plate of 7075 aluminum, and a larger plate of 6061.

Here's the setup I'm planning, but I have no idea if the numbers are right at all.

W're cutting 3/8" plate in three 1/8" passes with an HSS 3/16" 2 flute end mill using flood coolant. The CNC machine we're using isn't a super-heavy-duty one, but it isn't that wimpy either. We are considering going with a feedrate of 8 or so IPM, and a plunge rate of 5. The spindle rpm will be maxed at 5300 rpm, which I may decrease because I'm worried some aluminum will melt.

We're also curious as to how people make their toolpaths. We have MasterCAM, and a free solidworks plugin, and this is the first year we've used MasterCAM (we have just upgraded from x2 to X4). MasterCAM has many more features, but takes a little bit of getting used to. The software feels like with was written in the early 90's. The "undo" feature only works on certain things. You can't undo a change to a toolpath.

We plan on using climb milling, where outside cuts are clockwise, and inside cuts are counter clockwise (I think), but we'd like some input from other teams as to what works best.

[scottandme]

Look up feed and speed calculations in your Machinery Handbook, or any online reference.

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

GWizard is great as well if you're looking for more data (cutter deflection, MRR, HSM calcs, etc).

You might want to jump up to a larger/carbide endmill to avoid deflection in that cut. For a 3/16" HSS end mill taking a full width slot with 1" of tool stickout, you can only take ~0.04" per pass before getting noticeable deflection.

[apples000]

I don't have G-Wizard, but do you think that if we went with a carbide end mill and lowered the tool stickout to about 0.5", we'd be ok? Also, how much deflection is noticeable?

[Cory]

What machine, specifically is this?

If I were running 3/16" HSS I would run it at 200 SFM or so and .0015 chipload, which works out to 4266 RPM and 12.8 IPM. You would have to adjust from this point based on whether you had flood/mist/no coolant.

I would take .090 depths of cut, so 3 passes of .083", plus a finish pass.

Carbide would definitely be a more forgiving option, but that cutter in carbide wants to run at a MINIMUM of 17,000 RPM, so you're not going to get much advantage out of it other than rigidity.

[Karia]

Regarding climb milling: it depends entirely on what sort of machine you have. If you're running a converted Bridgeport or some really cheap machine, you might not have ballscrews, and thus doing climb milling is a bad idea (good info is here. In general, CNC Cookbook is a pretty good learning site.) Stick with conventional milling, and don't use carbide, it hates conventional cutting. If it's got ballscrews, definitely climb milling.

I'd personally second the call for a bigger end mill, if possible (remember, rigidity increases with the fourth power of diameter for cylinders. It's a reasonable approximation. Switching to a 1/4" will get you three times the rigidity.) That being said, you can get a 3/16" with 7/16" length of cut from McMaster, which isn't terrible. 2.5xD stickout. Shouldn't really be any big problems with that. If I'm recalling correctly, carbide has about 2.5x the elastic modulus of HSS. So it's roughly equivalent to the 1/4".

One thing to note: if you're going to be slotting at any point while cutting, you'll need to turn down the parameters. Slotting is very hard on the tool. Start by reducing the feed and speed 20%, and make sure you're dumping on coolant. For plunging, try 1/5 to 1/7 of your XY feed. End mills hate plunging.

I'd advise running some test cuts on some scrap material. Get a feel for how it cuts. Don't worry about breaking the cutter, just be ready to E-Stop the machine. You're playing with $13 of endmill (McMaster.) Tooling is disposable. If it doesn't take the cut, switch to a carbide or 1/4".

For CAM programs, try HSMXpress. It's free, and while I haven't used it, it looks pretty user friendly, and is totally integrated into SolidWorks.

[DampRobot]

I'd run at around 8 IPM and about 3000 RPM, but that's just me. I'd primarily be worried about breaking the tool rather than, say, chips melting or chip evacuation, especially since you're using flood coolant.

There's probably a reason why you need a 3/16" cutter, but if you have the choice, 1/4" cutters are really the "sweet spot" (at least in my experience) for cutting aluminium with coolant, because you can push them up to some quite high speeds without worrying about breaking the tool, or the part vibrating too much. I've done 1/4 inch passes at 18IMP and around 5000 RPM with flood coolant and 1/4" two flute endmill on a relatively "weak" machine, a Tormach. On our Haas, I probably wouldn't push a 1/4" endmill past 15 IMP because we only run mist coolant on it. In general, 3/16" endmills I'd be wary to push too much, because we've broken the only one we have in the shop many times by being too aggressive.

[sanddrag]

Personally, I use FSWizard online for all my feeds and speeds calculations and I've found it to work quite well. http://zero-divide.net/?page=fswizard

I've done parts out of 3/16" 6061 aluminum plate, with a .25" 3-flute carbide endmill, 10% stepover HSM toolpath, 6000 RPM, and 144 IPM.

I'm setting up today to do our gearbox plates from 1/4" 6061 aluminum plate, with a .25" 3-flute carbide endmill, 25% stepover HSM toolpath, 6000 RPM, and 29 IPM.

Both cases have flood coolant, and both took the full thickness of the part in one pass. What I haven't tried is comparing the job time between say a 10% stepover and a high feed, and a 25% stepover and a lower feed. That would be interesting to see which is faster.

In aluminum, you're limited really only by your spindle RPM (for smaller cutters). Next machine I get will be 10k RPM.

As mentioned above, avoid slotting, and avoid straight plunging wherever possible The tool does not like either of these much, specially straight plunging.

What machine do you have?

[Levansic]

The proposed plunge speed is what caught my eye. A good rule of thumb is 1/10th the fully engaged (100% cutter width cutting) feed, and avoid straight plunges like the plague.

If you plan to do NC cutting, as opposed to hand cranking, you really should step up to carbide cutters. They can cut 2-4 times faster and last 10 times longer in total cut. Additionally, you can get some great ZrN coated mills, with edge geometries suited to cutting aluminum (proper rake and adequate clearance), and cut up to 10 times faster, without suffering the dreaded aluminum buildup on the cut edge. Aluminum buildup leads to galling, essentially friction welding. This breaks endmills.

I will second the 3-flute cutter as a great go-to for aluminum. It is more rigid and allows 50% more feed than a 2-flute, and has better clearance than a 4-flute. Chip evacuation is critical for aluminum.

-- Len

[mplanchard]

Sounds like you're learning.
What ever you use, first make certain any long hair is tied back, no baggy clothing and safety glasses. Never machine alone.

Mastercam has been around since the early 1980s. Started in Conn. USA.

Having the SolidWorks - Mastercam experience is a good one.

Mastercam has a lot of teaching materials and a certification. I would check with them but a machining handbook is good for any team for mfg.

Before you machine, run your part through DFM Xpress inside of SolidWorks. You will get a series of messages if holes are too close to edges or too deep or tools just can't machine that square hole.

You can design features in SolidWorks that cannot be machined or too expensive or will add too much stress. DFM Xpress helps answer questions before manufacturing.

Try to review with a mentor if you can. Marie

[Jared]

I just got back from cutting 0.25" aluminum plate on a Tormach PCNC 1100. We used a 1/8" and 3/16" two flute endmill. Like Cory said, we started with 12.8 IPM from G Wizard, but we got a bad finish on some of the bearing holes, so we slowed down to about 8 IPM, and got a great finish. It's hard to tell in the picture, but we got a pretty rough finish on the part. You could probably use the 12.8 IPM for roughing, then take a final pass with a really small cut width as a finishing cut. When we slowed down, the little scrape marks from tool deflection went away. It's also really important that you get the coolant on the actual bit.

Also, you should definitely slow down the plunge rate. We had 6 to begin with, and broke a 3/16" end mill, and we were fine once we brought it down to 4.

I also agree with your opinion of MasterCAM, but once you get used to the silly setup, it's actually really powerful. It'll automatically do all sorts of cool stuff, like tabs, finish cuts, and depth cuts for you. I do agree that it's not perfect though, the command "regenerate all dirty operations" isn't exactly obvious.

[Mr. Mike]

Roy uploaded this to CD-Media back in June.

ME Consultant
By: roystur44
New: 06-21-2013 12:12 PM
Updated: 06-21-2013 12:12 PM
Total downloads: 62 times

Machining Calulator

ME Consultant is a powerful collection of machining calculators and data tables organized inside a graphical interface. It's intended primarily for CNC programmers, engineers, planners, machinists, and hobbyists involved with machining or machined products. ME Consultant is freeware and there are no restrictions on its use

[DonRotolo]

Cutting speed and spindle speed are both functions of the tool manufacturer's recommended chip load. Too little and too much chip load are both bad.

For example, I use an Onsrud single-flute cutter on a router. It needs to see 0.004-0.008 chip load. At 10,000 RPM, that means I need to move about 0.006 per revolution, which comes to cutting at 60 IPM. (With 3 flutes, you'd need to move 3x faster, or 0.018" per rev - so speed would be 3300 RPM for 60 IPM, assuming the same recommended chip load)

Now we consider cutting depth: My machine is definitely unable to cut at 1D (meaning 1/4" deep for a 1/4" cutter); instead I cut at 1/2D. If my machine was beefy enough, the tool can handle 2D.

That's for conventional milling around a perimeter. For slotting, I'd cut it down near the minimum 0.004" chipload.

Lastly, this includes either an air blast (wood, plastic) or air with mist coolant blast (for aluminum) to make sure all chips evacuate the cutitng path. Re-cutting chips is very bad. Also, there is a vacuum system (a 2.25" shop vac) that scavenges the chips and keeps the machine clean.

The bottom line: There is science behind selecting feeds and speeds, the tool manufacturer is your friend, so go and do the math.

[apples000]

Originally Posted by Cory

What machine, specifically is this?

If I were running 3/16" HSS I would run it at 200 SFM or so and .0015 chipload, which works out to 4266 RPM and 12.8 IPM. You would have to adjust from this point based on whether you had flood/mist/no coolant.

I would take .090 depths of cut, so 3 passes of .083", plus a finish pass.

Carbide would definitely be a more forgiving option, but that cutter in carbide wants to run at a MINIMUM of 17,000 RPM, so you're not going to get much advantage out of it other than rigidity.

It's a converted bridgeport (of mine) with ball screws from an older CNC, stepper motors, and a Mach 3 controller that an older mentor put together for us. Now that I've checked, I've realized that I don't have 3/16th carbide bit, so I'm just going to use the HSS for now. If bad things happen, we can make the part bigger and use the 0.25" end mill. We've got plenty of spare aluminum.

I currently have two plans (all at max rpm of 4400 ish, and 3 IPM plunge)

1- Cory's 3x 0.090 deep cuts with a finish pass with 12.8 IPM
2- Jared's 0.125 deep cuts with a slower speed of 8 IPM with an optional finish pass at 12.8 if the tool deflection/machine sloppiness is significant

We're also going to try to see how accurate it really is. Right now, I'm doing the bearing holes undersize, then reaming the hole to press-fit, but for fun, I'll try doing a bearing hole with a 0.01 width finishing cut and a bigger 0.25" HSS end mill to see if I can get accurate enough.

[sanddrag]

I realize many of you are not working on full VMCs, but I'll post my experience today nonetheless.

I had toolpaths to pocket our gearbox plate. 1/4" 6061 plate, 1/4" 3fl carbide endmill, 6000 RPM, flood coolant. At 25% stepover, and 30 IPM (what FSWizard recommends), my CAM package said it would take 16 minutes. At 10% stepover and 120 IPM (again, what FSWizard recommended), my CAM package says it will take 11 minutes. That's quite a savings. So, that's what I'm running. I should also mention, I'm feeding at 300 IPM through air on the "backstroke" of the HSM toolpath.

Now on the machine, I realize considerable time is being lost due to limits on acceleration and deceleration. I enabled the trial of the HSM parameter on the HAAS control, and saved 2 minutes and 40 seconds, with the exact same program.

I'm doing the outside contour of the plate with a 1/2" 3fl carbide, at 5500 RPM, 25% stepover, and 100 RPM, and it runs fantastic.

If your machine can do it, it seems like high feedrates with a very thin chip are the way to go, if you have the spindle speed for it.

Now, I have two questions:

Don, where are you buying your Onsrud router bits. Link?

For anyone, what feedrate should I be using when going on a helix plunge into the material with a 3 flute square corners endmill? My CAM package always puts the plunge rate at half the pocketing feed rate, but I worry and back it off a bunch, to like 20 IPM. I'm ramping down on a 3 degree helix.

[scottandme]

Ramp in to the cut, don't straight plunge. Should be trivial to do in Mastercam.

4075 RPM @ 12.2 IPM (200SFPM & 0.0015 inch/tooth) - full slot with 0.09" DoC gives me an estimated 0.002" of tool deflection (1" stickout guess). Not good when your chipload is smaller than the cutter deflection.

4075 RPM @ 8 IPM has 0.018" of deflection, but chip load is only 0.001 inch/tooth there.

Unless there's some crucial need for a 3/16" cutter, go with a bigger end mill. If you need to you can always do a cleanup pass with a smaller endmill after roughing out the shape.