Feed rate

[chris123]

This doesnt seem right, I put these numbers into GWizard

Tool - 3/16"
Flutes - 2
Max RPM - 10,000
Max IPM - 50
Depth - 0.1"
HP - 0.1

and this is what it said

It says to run at 10,000rpm and 27IPM

I have a pretty much a stock taig but it seems to fast to me

[Dean W]

Tool - 3/16"
Flutes - 2
Max RPM - 10,000
Max IPM - 50
Depth - 0.1"
HP - 0.1

For what material?
And, 1/10 hp?

[chris123]

I'm milling through 6061 aluminium
The mill had no problem with 10IPM but my dodgy supply and wiring fried a driver. So I'm replacing everything with a proper switch mode supply and new stepper drivers with out the 10u steps. This will allow it to run theoretically 10 times faster.

HP is actual 1/8 so 0.125hp but I can't enter any more then 1 significant digit so 0.1hp is the closest

Carbide end mill

[themedulla]

Something seems a little dodgy... You put in max ipm at 50 and it still tells you to run > 200ipm?

I wouldn't rely on a feed rate calculator anyway when using a Taig - they generally assume a perfectly rigid machine. You should start to think about things in terms of chip load. However you run your machine, you will want your end mill to remove the same amount of material every revolution. Try to remove more than the ideal chip load and you are going to hammer your end mill or stall your motor (or both at the same time). If you aren't removing enough of a chip load then you can also run into problems - mostly because you are not removing enough heat from the material. This can hammer your tool pretty quickly as well.

The amount of material you want to remove per flute depends on things like geometry, coating, etc, but your manufacturer may give you some recommendations. Here is Niagara's recommendation page for their carbide cutters:

http://www.niagaracutter.com/solidca...speedfeed.html

So then for any given spindle speed you are going to have to adjust the DOC and feed to remove the right amount of material. The faster you run the spindle, the more horsepower you are going to have to have to remove the right amount of material. Once your motor starts to stall out, drop the spindle speed down a bit.

[chris123]

that should be 27 ipm
ok I'm still lost as to what i tell the CAM program how fast to feed the cut

[themedulla]

Sorry I misread that.

From personal experience I am not sure you will be able to drive your Taig through a 0.1" DOC at 27ipm - maybe with a roughing bit.

So if you look at the Niagara web page referenced above, I would base calculations off of the 3/16" chip load (on the chart they call it feed in/tooth). On the table the value I get for the 3/16" end mill in aluminum gives me a feed of .002 in/tooth.

Now use this formula to get your feed rate:

feed (in ipm) = RPM * chip load * # of teeth

You will need to first pick your RPM - the higher you choose the more horsepower you're going to need. Let's say 3000RPM for starters.

feed (ipm) = 3000RPM * 0.002in/tooth * 2 teeth (flutes)

Calculating it out you would get 12ipm. That may not sound like a fast speed, but you can work with a deeper DOC - just under where your motor stalls.

Likewise if you want to drive it at 6000RPM your feed would be 24ipm. Work with different DOC to figure out what your motor can handle.

If you were to set your machine to 3000RPM and drive it at 20ipm even if you are using a shallower DOC your motor may not stall but you are loading your end mill too much - you are driving it through the material faster than the teeth can clear the chips out.

Likewise if you were to set your machine at 6000RPM but drive it at 12ipm you are not removing heat from your workpiece quickly enough and are not being nice to your end mill.

Does all that make sense?

[themedulla]

I should also mention that I used the info from niagara's table - your end mill may have different attributes. If you can't find a recommendation for your specific end mill then just search around and find a nice average chip load (listed in inches per tooth) to run your calculation.

It took me a while to figure this out. Before I was just kind of guessing around, but your tools will last longer and cut better if you base your feeds on reasonable chip loads. Every RPM will give you an ideal feed rate - the DOC will determine how much horsepower you are using.

[chris123]

cool, i understand now, thanx
i will try again once i get my machine working with the new controller and end mill
I shall ask the manufacture for recommended chip load and go from their
DOC doesn't matter with that calculation, how would I work out an appropriate DOC?
What if I am profile cutting and not cutting deep, does it make any difference?
My CAM package allows me to adjust the entry and exit speed should these be the same

[themedulla]

Usually they will specify a range of DOC for their chip load - on the Niagara page at the bottom it covers 0.5 * diameter of your end mill up to 1.5 * diameter of your end mill.

I would suggest starting with 0.5*D and then step it up until you get too much vibration or your motor stalls out - then back off a bit. That value would be for cutting a slot. For profiling you can go deeper.

[chris123]

In that table what does the speed S.F.M. mean?

[ee_t]

http://en.wikipedia.org/wiki/Surface_feet_per_minute

[chris123]

That doesnt seem right
The SFM from the link below is 800-2000 and the SFM from the wiki page is 250-350?
So I'll use SFM of 300
Now I'm using a 4mm 0.15" tool bit
I get the following
rpm=7300 ipm=29