[juniormachinist]

i no this is probably the wrong forum to post on about this but we have a fadal vmc 4020 with carbide cutters and we're not sure what feed rates and spindle speeds to run. we're mainly machining 6061 aluminum. we have run something but the finish on it was crap. any ideas on a good way to work them out?

[BobWarfield]

Google "speeds and feeds calculator". Tons of 'em out there!

Cheers,

BW

[juniormachinist]

yes there's tons out there but they all give different numbers and it's hard to no which one to use to get the best finish I was hoping someone has an all round formula preferably something that's a free program or formula

[txcncman]

Buy a Machinery Handbook and read it.

Machining is as much of an art as it is a science. Most of the recommended numbers are just starting points.

For cutting aluminum with uncoated carbide, depending on your set up, axle depth of cut, and radial depth of cut, you can probably run 400 SFM and 0.008 chip load. If that did not mean anything to you, then you have a lot to learn.

[BobWarfield]

Unfortunately, it takes more than a simple formula. It even takes more than Machinery's Handbook offers, and you still won't be done.

There's quite a lot of information in our Milling Feeds and Speeds Cookbook:

CNC Milling Feeds and Speeds Cookbook and Tutorial

You can choose to do a little or a lot. The basic formulas linking chipload, feedrate, sfm, and rpm are great as far as they go, but they're wrong if you take a cut width that's less than 1/2 the diameter of the cutter due to something called "radial chip thinning". So, you want a calculator that does the basics, but that also factors in radial chip thinning. Then you'll want to account for the effects of deeper cuts, slots, through spindle coolant, tool deflection, yada, yada.

You're welcome to try our G-Wizard calculator. The 30-day trial is free. It is worth your while to check out several of these calculators and see which one you prefer. Also, do take a look at the aforementioned Cookbook. It'll give you a feel for some of the tradeoffs at work. Two of the short articles of particular interest might be:

Calculating Feeds and Speeds:

Calculating CNC Milling Feeds and Speeds

That article gets into some of the factors and calculations that will affect the cut.

Toolroom vs Manufacturing Feeds and Speeds:

CNC Milling Toolroom vs Manufacturing Feeds and Speeds

There are really 3 levels of master:

1. Generic "default" feeds and speeds. Available in varying degrees of sophistication from the calculators.

2. Manufacturer's recommended feeds and speeds. Usually a bit more performance there. A calculator is still very useful for dialing the recommendation to your particular cut (e.g. handling radial chip thining and such from the mfg's start point), but it needs to be possible to dial it into the mfg's numbers.

3. What I call "Manufacturing Feeds and Speeds". These are feeds and speeds that you've tuned by trial and error to fit your machinery, your tooling, your best practices, and even your exact projects. This is where you really dial in on chatter and that sort of thing. This is more of a database problem, since you need real data from your shop usage, coupled with a calculator to create a Cut Knowledge Base.

Hope that helps. Sorry it's not an easier thing, but dialing in the best feeds and speeds winds up being a competitive advantage at every level. CAM programs that have HSM toolpaths are more money than ones that don't and they're worth it.

Cheers,

BW

[txcncman]

@Bob - What does your cookbook say about side milling 1.750 deep with a 0.3125 diameter 2 flute solid carbide uncoated endmill with 0.650 flute length necked down 0.015 for clearance cutting 7075 unsupported aluminum web 3 inches long by 0.093 thick?

[BobWarfield]

@Bob - What does your cookbook say about side milling 1.750 deep with a 0.3125 diameter 2 flute solid carbide uncoated endmill with 0.650 flute length necked down 0.015 for clearance cutting 7075 unsupported aluminum web 3 inches long by 0.093 thick?

txcncman, if I pump all that into G-Wizard it says its not happy!

Let me expand and clarify. A full slot, with 1.85" stickout (wanted to leave 0.100" clearance between holder and top of workpiece) and 0.65" cut depth, gives about 0.003" of deflection. That's what's not happy. You want to keep it to 0.001" max for roughing and much less for finishing.

So, I then asked it to run the cut optimizer and tell me how much cut depth I could accomodate with a full slot and that much stickout. It responded with 0.097". So, if I were going to rough down with a slot, I would limit the levels to that depth. Feeds and speeds for that cut would be 7500 rpm (dunno your max spindle and that's the default max) and 37.5 IPM feedrate. That's a chipload of 0.0025, so it's trying!

Now, if we're gonna ramp our way into a pocket and then take it easy, and we want to cut that full 0.650 flute length, I can run cut optimizer on that and it suggests a max cut width of 0.084" for roughing to yield a max deflection of 0.001". That's 7500 rpm at 20.8 IPM. That's actually not so bad since we get to do so much without going down level by level.

If you have a constant engagement angle (HSM) toolpath on your CAM, and you turn that on, that last cut can be cranked up a bit. Let's do this with a toolchange, and use one tool that has 0.9" stickout and will run the HSM path, and one that has the full 1.85" stickout. First tool can go quite a bit faster--40 IPM. We can then swap tools, and the second tool has the full stickout, but let's say we only have 0.3" more to cut. I can make that last deepest level at 47 IPM with the HSM toolpath.

There's a lot of other combinations you could choose to play with to see what might optimize your job. Or, you can just avoid the fancy stuff and understand what would work at a particular cut depth and cut width combination. This is also with default tool data. You could add a particular manufacturer's data pretty easily. You can also use the built in database to record your own trial and error results to exceed mfg's limits based on your shop's best practices. Like I say, you can take it easy as a beginner or play with the bells and whistles to improve productivity.

Hope that helps,

BW

[txcncman]

@Bob - Just to let you know, when I have had to mill such parts, I am not happy either and would love to catch the engineer in a dark alley somewhere. But thanks for the explanation of your cookbook. These are things that younger guys do not take into account or can even imagine about the physics involved in machining that become second nature to true veterans in the shop.

[juniormachinist]

is there anything thats free and does the same thing?

[txcncman]

Milling Speed and Feed Calculator

[austin.mn]

Excellent answers Bob. I saw that you added engraving bits to the calculator. I just updated yesterday and will check it out later tonight.

Even though I don't use the calculator as often as I probably should (I think that it would save me some roughing time if I were to do a double check on my speeds) It is an excellent value and I recommend it as often as I can. I even use it to check the kids geometry homework... He said I was cheating, but I told him we didn't even have a basic calculator when I was school, all the math was done long hand, now I try to just work a little smarter.

Thanks again for the Gwizard program.

[Rstewart]

@ txcnc

Milling something like that (thin wall) is gonna require very small step-downs to get your part in tolerance.

I would start at about 5000 RPM 55 IPM and .09 step down. I always perfer a three flute tho. My Two cents.....

[juniormachinist]

guys i need something that's free and is easy to we are just doing this as a hobby sorta thing to make our own parts for projects and want stuff to have a good finish

[txcncman]

Machining (quality machining) is not easy. It takes months and years of study and practice and experience.

[Shane1234]

and a good ear i always say....... you can usually tell how your machining is by sound.....

[cygnus x-1]

Even for hobby use, I would strongly recommend you at least try out Gwizard. It is truly an exceptional program and has saved me from a huge amount of frustration and guess work. Being fairly inexperienced I always found it difficult and time consuming to come up with efficient feeds/speeds, especially since I tend to do mostly one off parts and prototype stuff where it's not feasible to do much tweaking of machining parameters. I also tend to have a seriously tight tooling budget so I need to come up with safe feeds and speeds to extend too life as much as possible. Even a single scrapped part or broken tool can cost as much as the yearly fee for Gwizard. It could very well *save* you money to use it.

And BTW, I have no affiliation what so ever to Bob or CNCCookbook, other than being a very happy user.

C|

[DMF_TomB]

side milling 1.750 deep with a 0.3125 diameter 2 flute solid carbide uncoated endmill with 0.650 flute length necked down 0.015 for clearance cutting 7075 unsupported aluminum web 3 inches long by 0.093 thick?

parameters
Carbide end mill 2 flute
0.3125 dia (less because necked down)
Stickout 1.750"
Aluminum 7075 with Machinability rating of 3 cubic inches per hp per minute
at only
590 SFPM
RPM 7513
max chip thickness 0.0019
max Feed 28 ipm
max Depth of cut 0.196"
..... at max parameters that is 32 pounds of force at end mill tip using 0.54hp
BUT with thin wall aluminum i would much less than the maximum settings if nothing else 32 pounds can distort thin aluminum only 0.093" thick