Speed and feed...

[kombayotch]

Ok, I just finished converting the x and y axis of my knee mill to CNC and decided to try her out.

Milling 6061-T6 aluminum with a 3/16 endmill. Would like to cut a slot 0.120" deep.

When I calculate the RPM rates using the SFM number from the endmill mfg., they are way higher than my max RPM (2500). When machining manually, I just use my fastest RPM and adjust the feed rate based on the feel and sound. It worked.

I did some reading and leaned that I have to match the feed rate to the chip load per tooth. Had trouble finding formulas to do that. Ended up finding a program from Robb Jack that calculates the feed rate based on the limitations of my machine. It came out to be 20 ipm and suggested that I cut the slot in 1 pass. That didn't seem right to me based on my manual machining experience. So I used 10 ipm. The endmill broke... which I kind of expected.

Would somemone be kind enough to point me to right formulas and show me an example of how this is calculated. I assume that the approach that I should take is to run the spindle at max RPM and then calculate a feed rate. Also, how do you calculate the depth of cut to use per pass?

[borrisl]

I use a program called ME Consultant. It's free. I ran your specs and came up with a max of 7 ipm.

[borrisl]

http://mrainey.freeservers.com/

Just in case you wanted to try it. The author of the software is a great person. Very helpful. I use this as a guide.

Hmmm. After checking the link, it appears the free version isn't avail anymore.

[WhiteTiger]

Aw, that's just too cute (and eminently useful!).

Thanks for posting that borrisl. Made today's online time worthwhile all by itself I love concise little programs that give you something you can make use of without an overload of bells and whistles.


Tiger

[little bubba]

The simple manual way,

(3.8/cutter diameter) * SFM = RPM

Take that RPM or whatever RPM your going to use (2500 max spindle) and multiply it by how far you want the cutter to advance with each rotation.

quick example, 2500rpm * .004 per rev = 10ipm.

Really easy.

[One of Many]

If you have a feedrate overide knob, it gives you the control to increase or decrease based on conditions at present. I have my CAM defaults set to 5ipm on steel, 10ipm on aluminum and use the feedrate overide 10-150%.

I have always used the calculation of:

IPM Feed rate=(chip load per flute)*(number of flutes)*(spindle RPM)

You can look up the SFM rating of the material being cut as a guide to find the RPM values based on the cutter diameter, but IMHO, use it as a guide conservatively. The strength in the cutter influences this to a greater degree than relative load assumptions in the next step to calculate a feed rate. Keep in mind that this is the MAX feed rate. Actual feed rate may be between 0 and reality to sound and feel as it is in any manual operation.


A typical standard length cutter is (more or less) designed to take a full length cut at .002-.004 per flute on 1/4 of its circumference. See attachment for detail. Cutting a path using 1/2 of the circumference is twice the load it should handle at the same feed rate or depth of cut. From my experience the depth of cut needs to be about 1/3 the diameter in that usage. Lowering the feed rate only increases the chances for chatter.

Even so, you cannot trust a 3/16" cutter to produce a 3/16" slot. Do not count on success if a no slop fit is required. Most cutters will cut oversize between wander and spinning off center.

DC

[kombayotch]

OK, that seems to have worked. 30-35 though depth for cut was about the limit before vibration became noticeable.

Where does the chip load value come from? Is 2-4 though a standard? I was always missing this value when I tried to use the formulas. That was one point of confusion.

And it turns out that my max RPM is 2300. I adjusted accordingly.

[One of Many]

Originally Posted by kombayotch OK, that seems to have worked. 30-35 though depth for cut was about the limit before vibration became noticeable. Where does the chip load value come from? Is 2-4 though a standard? I was always missing this value when I tried to use the formulas. That was one point of confusion. And it turns out that my max RPM is 2300. I adjusted accordingly.

I think of it more as a constant than a standard. Pushing a cutter beyond that envelope is flirting with trouble. It can become an issue of poor precision, wasting a cutter, which can waste a part.

There is a relationship between the Machine, the cutter, the part and the work holding. Each one has its limits. There is forever a need to realize that balance before something starts to suffer.........


Or you get to be good friends with the E-stop and Scrap bin.


DC

[DareBee]

The cutter manufacturer always recomends chiploads for their cutters, each cutter style and material is different.
As a general rule of thumb generic type cutters in steel
up to 1/4" dia .0005-.001
1/4-1/2 dia .001-.002
1/2-3/4 dia .002-.004
3/4-1 dia .004-.006
this is chipload per tooth.
chiploads for aluminum are double this.
obviously a 4 flute cutter runs twice the IPM of a 2 flute cutter.

[borrisl]

Now that I have Mikes' permission to post this:

This is ME Consultant 2.0. It is a free version. Mike has a pro version that is much more comprehensive.

http://mrainey.freeservers.com/

It it really fast for calculated gerneral feed speeds on all types of tooling in almost all materials. For a newbie, like myself, it has been really helpful.

[Clawsie Machine]

Ok a couple of questions here first.

1. I usually use MasterCam's recommended feeds and speeds when setting up a tool, BUT how acurate are they?

2. How do I load in this "free" ME consultant 2.0 software. I tried to play with it and it looked up my system?

3. I would like to get a couple examples for some cutters I'm looking at:

A. 3/8 2 Flute carbide cutter for Aluminium. From there manufacturer site:
" Slottling up 1 X "D" .008 with SFM up to 5000."

B. 1/4 2 Flute carbide cutter for Aluminium.
"Slottling up 1 X "D" .004 with SFM up to 5000."

Now how would l figure these out? Basic, well explained process would be best, I don't want to assume anything with this due to the amount of work with this production job coming up. Machine has Max RPM of 6500!

Would like to run these E/mills under max RPM, say +- 5500 RPM or there abouts.
I have really know idea on how to figure out the IPM or RPM for a material by using the SFM rule. I usually use RPM X Chipload in load per tooth X # of teeth. Like 2500 RPM X .003 X 4 teeth = 30 IPM!

I want to convert ALL my programs to "G95" for inches per tooth in relationship to RPM and not IPM. I feel that with production this might be a better way to get the most out of each cutter?

Thanks in advance, John

[One of Many]

Originally Posted by Clawsie Machine Ok a couple of questions here first. 1. I usually use MasterCam's recommended feeds and speeds when setting up a tool, BUT how acurate are they? 2. How do I load in this "free" ME consultant 2.0 software. I tried to play with it and it looked up my system? 3. I would like to get a couple examples for some cutters I'm looking at: A. 3/8 2 Flute carbide cutter for Aluminium. From there manufacturer site: " Slottling up 1 X "D" .008 with SFM up to 5000." B. 1/4 2 Flute carbide cutter for Aluminium. "Slottling up 1 X "D" .004 with SFM up to 5000." Now how would l figure these out? Basic, well explained process would be best, I don't want to assume anything with this due to the amount of work with this production job coming up. Machine has Max RPM of 6500! Would like to run these E/mills under max RPM, say +- 5500 RPM or there abouts. I have really know idea on how to figure out the IPM or RPM for a material by using the SFM rule. I usually use RPM X Chipload in load per tooth X # of teeth. Like 2500 RPM X .003 X 4 teeth = 30 IPM! I want to convert ALL my programs to "G95" for inches per tooth in relationship to RPM and not IPM. I feel that with production this might be a better way to get the most out of each cutter? Thanks in advance, John

This is what I can offer.

The first value needed for any material is the SFM in which that particular alloy can be cut and with what cutter material is being used. Obviously higher with carbide than HSS. This will relate to the spindle speed in RPM for the circumference of the cutter itself.

If the material has a SFM window of say 200-300SFM and the cutter is .375 in diameter, then:

RPM=(sfm*12)/(Cutter Dia * Pi)

2037 RPM=200SFM for a .375 cutter.
27,500RPM =2700SFM for a .375 cutter.

Use whatever the limit for the recommended SFM of that particular alloy and adjust accordingly. If your spindle does not meet that SFM, then go to the top RPM and chip load as you already are. It should not matter how the feed is applied, as long as the IPT feed rate is relative to the RPM while still in harmony with the present conditions. Ultimately the operator must make some of those decisions with the programmer. Preferably before the unforeseen is found too late?

The chip load that the OEM gives may very well be for perfect conditions in all other areas of rigidity. If the application can handle it, then push it as hard as you dare. Those conditions just do not happen very often. Something will put limitations on full tilt chip loading. Efficiency must take into account the weakest link, including susceptibility to chatter, surface finish and dimensions. Just because someone puts a spec on the capacity of the cutter, won't mean that it applies in all cases. To many variables to count on there.

DC