[nateman_doo]

I am trying to figure out what is a good feed & speed for cutting copper.

I have an X2, with belt drive conversion, so I can't give any accurate RPM, aside from their max speeds on each gear.

I did read that a surface speed per minute is something that is a given, and i read it was 100 for copper, but I am drawing blank on the concept of chip load per tooth. Can someone clarify what that is?

[mannymade]

chip load is the amount of material being removed per tooth per rev per feed rate. It is also dependent on your set up and your tooling.

[eartaker]

Nate,

Buy this and you can check your RPM Digital Laser Photo Tachometer Non Contact RPM Tach,205 | eBay

This is the same seller I bought mine from. If you are up to it you could order the C3 card from CNC4pc but this will get you going if you want something simple and quick.

[nateman_doo]

once I have the tach, then what? What is the C3 card for? I still have no idea how to calculate.

[michaelthomas]

The sfm figure will tell you what rpm to run at. It will be different depending on the diameter of the end mill you are using.

Milling Formula Calculator

Here is a calculator that is useful.

In the second one down (revolutions per minute).....type in the recommended SFM (you said 100) and the bit diameter. It will tell you the rpm to use.

Then you will need to use that rpm figure and factor in the amount of material that each tooth will remove (chipload) and you can determine the cutting speed in inches per minute. Type your rpm calculated from the first calculation, chipload, and number of teeth (d) in the fourth calculator down (inches per minute feed rate). You now have your feed speed.

The manufacturer of your endmills will usually specify a chipload for their bits. The chip load will vary depending on the operation. These will be good starting points......but everything can vary some.

The Gwizard is a very nice calculator that will do everything for you. All of the sfm data for different materials, chipload, and way more is in the calculator.......and you can try it for free for 30 days. It will be a good learning tool, too.

GWizard: A CNC Machinist's Calculator

[nateman_doo]

I found this link as well:
Carbide
HSS bits

Now if I understand this, cutting copper with a 3/8 2-Flute Carbide Endmill, This is the details:

Tool Diameter: .375 (given)
Flutes: 2 (given)
IPT: 0.004 (from link)
SFM: 350 (from link)
Spindle: 3500 RPM (calculated)
Feed: 28.5 IPM (calculated)

Does this sound right? Where to I get the depth of the cut? I have been using 0.02 as the depth per cut. This is a home made machine, so it doesn't have the rigidity of a commercial one.

[michaelthomas]

The chip load is per tooth. .004 inches per tooth may be a little aggressive. About half that would be a good starting point.

The inch per minute calculation is rpm x chip load x number of teeth. So 3500 rpm x .002 x 2 = 14 inches per minute.

1/2 diameter is pretty safe for a depth of cut.

[eartaker]

Nate just to start out try this you can adjust on the fly.

With a .375 2 flute endmill
10 IPM
2500RPM
.05 to .125 Depth of cut.

This is where you need the tach to check you RPM.

[nateman_doo]

Why is the RPM so important?

[SCzEngrgGroup]

Why is the RPM so important?

RPM, along with chipload, determines feedrate. Excessive RPM for a given tool wears the cutting edges very quickly. Low RPM means slow going, and/or broken tools.

Regards,
Ray L.

[nateman_doo]

Wow, so there is a method to the madness. I have been using max RPM, and a feed rate of 2IPM. Probably wearing the crap out of my endmills.

[SCzEngrgGroup]

Wow, so there is a method to the madness. I have been using max RPM, and a feed rate of 2IPM. Probably wearing the crap out of my endmills.

That is about the worst thing you can do. You want to run as heavy a chip load as the tool and machine will allow. If your tools load up, and chips weld to the tool, or the tools gets hot, then you're feeding too slow. Get the feedrate right on a shallow cut (on the order of 0.100" for a small machine with any but very small tools), THEN start going deeper, until surface finish degrades. Do NOT slow down feedrate unless you have no choice.

For a small machine, don't waste your money on carbide tools. You can't take advantage of them, and a good HSS tool will work just as well, if not better.

When used properly a good quality tool cutting aluminum will last a loooooooong time. I've used a single 1/2" HSS endmill for months of nearly every day work.

Regards,
Ray L.

[nateman_doo]

vey good info! But HSS and copper also?

[SCzEngrgGroup]

vey good info! But HSS and copper also?

The rules are the same regardless of the material. What changes with material is optimum SFPM and chipload.

Regards,
Ray L.

[nateman_doo]

So for a HSS 3/8 bit:

RPM: 611-815
Chip load per tooth: .001-.003
SFM: 60-80

[nateman_doo]

For Carbide:

[mannymade]

I can't give you the scientific break down of why Rpms are important in terms of metalurgy. Tools are created with a rating in reference to set standards of material as well the cutting tools used. I was always taught 4xcs/dia. Others get down to the decimals of 3.82 and use an average on sfm. Hope this helps.

RPM CALCULATIONS
RPM is the abbreviated form for Revolutions Per Minute (the amount of times the
tool or the work rotates in one minute). There are two factors that must be considered
when determining the correct RPM.
1) The dimeter of work or tool being used. (If a drill bit is being used then it is the
size of the drill bit, if a round shaft is being machined in the lathe then it is the
diameter of the shaft).
2) The type of material that is being machined. (Easy to machine material or difficult
to machine material, refer to chart on reverse).
Using an RPM that is too slow will cause unnecessary pressure and wear on the tool.
This slow RPM will mean that the drilling pressure will be too much and the drill bit will
probably break.
Using an RPM that is too fast will cause a great deal of chatter and vibration on both
the work and the tool. The heat generated from this fast RPM will damage the cutting
edges of the tool.
RPM FORMULA 4 X C.S.
Diameter
4 = A given value for the formula (does not change)
C.S. = Cutting Speed of the specific material (changes when the material changes)
Diameter = The diameter of tool or work (size of the drill when drilling)
The cutting speed is defined as the rate at which a point on the work circumference
travels past the cutting tool in one minute. Cutting speed is expressed in either feet per
minute (ft./min.) or metres per minute (m/min.). For our purposes and because most of
the industry shops work in imperial we will be using feet per minute. Please refer to the
chart on the reverse when determining the correct cutting speed for each material.
Material Feet per minute
(ft./min.)
Machine Steel 100
Tool Steel 70
Cast Iron 60
Bronze 90
Aluminum 200
These cutting speeds are based on cutting tools made from a material called “High
Speed Steel” (HSS). If the tools are made from carbide, a much harder and more
durable material then the final answer should be multiplied by four.
Sample Question:
Calculate the RPM when parallel turning a 2.5" diameter piece of tool steel.
RPM = 4 x C.S. = 4 x 70 = 280 = 112 RPM
Diameter 2.5 2.5
If the question stated that you were using carbide tooling then multiply your final
answer of 112 x 4 = 448 RPM
Questions: (Show all work)
1. Define cutting speed.
2. List the formula used to calculate RPM. Explain each part of the formula.
3. Calculate the RPM when drilling a ½" diameter hole in a piece of machine steel.
4. Calculate the RPM when drilling a 1-1/4" diameter hole in a piece of cast iron.
5. Calculate the RPM when drilling a 1/16" diameter hole in a piece of bronze.
6. Calculate the RPM when drilling a 1/4" diameter hole in a 3" diameter piece of
aluminum using the lathe.
7. Calculate the RPM when center drilling (1/4" diameter)in a piece of 4" diameter
machine steel using the lathe.
8. Calculate the RPM to turn a 2-1/2" diameter piece of machine steel using high
speed tooling.
9. Calculate the RPM to end-face a 3" diameter piece of machine steel using
carbide tooling.

[mannymade]

It also depends on your setup. How rigid your machine is as well and how the chip is being evacuated and heat is being dispersed. There are a few things to consider. For example, I use a a 6mm 2 flute ball nose endmill on white chilled cast iron that tests at 50 to 53 hrc. The tooling I chose requires a 5,000 rpm with a .050 depth of cut for a length of 36 inches and a feed rate of 30 ipm. Things for me to consider, my machines tops out out at 2000 rpm and I've created a 4th axis using a 50,000 to 1 ratio to achieve the right helix angle. There's more but for the sake of explaining, I will simplify by stating that I'm tied to a certain rpm and feed rate. So I basically break everything down rpm and feed rate to a little less than half and increase my depth of cut double and blow the chips out. I get great results and the tool is still within its rating.

[nateman_doo]

Since I have a max RPM as well (1100/3000) I have to do the same correct?

[packrat]

For a small machine, don't waste your money on carbide tools. You can't take advantage of them, and a good HSS tool will work just as well, if not better.

When used properly a good quality tool cutting aluminum will last a loooooooong time. I've used a single 1/2" HSS endmill for months of nearly every day work.

Regards,
Ray L.

@Ray - do you realize that you have just committed BLASPHEMY on this site? Every one here says that you need carbide/insert tooling for every thing on all machines. That HSS is worthless in todays world.