[Darth Yoda]

I m using MC7 to make some .3125 wide slots. A four flute uncoated .3125 carbide endmill 1. inch.deep. I have broken 3 endmills going from 2650 rpm to 3500 rpm at around 5 ipm (full depth) in A36 soft steel with flood cooling. I knew that wouldn't work but my boss saw a video........

I actually got 1 finished part by doing depth .100 cuts 1528 rpm and 5.1 IPM if I remember correctly.

What proceedures would you guys use with what tools?

Its NOT a good setup but it seems to be vibration free while running. Its an "L" shaped part kinda like a your hand with the fingers bent. The palm area is 5x5x1 and has four slots .3125 x 1 and the leg or your fingers has 2 slots. I have the palm resting on a square tube 13.5 inches high with the leg hanging down. There are 3 strap clamps holding it.

Hope I described it clearly. Thanks again for the help.

Yoda
PS
If anyone is near Sherman - Denison Texas and wants to meet up, let me know!!!!

[Tom-AMS]

several suggestions:
first go to CNCcookbook.com and download a free trial copy of G-Wizard fee & speed calculator. Take time to watch the videos on how to get the most out of the calculator.
buy a subscription - what it will save you in broken tools will more than pay for the subscription. (I'm not affiliated with GW, just a very satisfied customer)
next, there are several ways to skin this cat, ...start by trying this:
1. remove the bulk of the metal by Chain Drilling with a 9/32" screw machine length drill bit with 135° point, to just shy of finished depth. Let each hole overlap the previous hole by about 0.030 to 0.040". Drill both ends of the slot and work toward the middle as you space the holes.
2. Assuming your endmill sticks out of the tool holder no more than 1.3" AND if the slot's width does not require great precision, then try 4 passes, each
at 0.220" deep with a 5/16 4-flute carbide endmill at 3375 rpm & 9 ipm. For the final pass with a 0.120 depth of cut, run 3525 rpm & 7.6 ipm.
3. Run flood coolant or air to blast the chips out of the slot - you must not re-cut chips or it will break the endmill.

If all you have are HSS endmills, then try 8 passes at 0.120 deep at 1735rmp and 5.2 ipm. For the final pass with a 0.040" DOC use 1775 rpm & 5 ipm. Make sure to blast the chips out so it doesn't re-cut them.

If your CAM software & mill support trochoidal tool paths (high speed milling), then take advantage of it.

[CitizenOfDreams]

Whenever I do deep slots in plastic or wood, I use a mill that's smaller than the slot width. Is that a good advice for metal milling as well?

[ERUS]

Whenever I do deep slots in plastic or wood, I use a mill that's smaller than the slot width. Is that a good advice for metal milling as well?

Yes.

Chain drilling also isn't a bad idea.

The problem with milling a slot that is as wide as the diameter of tool being used is that if for example the slot is 0.3125 +\- 0.001 it will be very difficult to achieve a tight tolerance. The tool will vibrate in the slot with full engagement on the cutter diameter. The side of the slot that the endmill is cutting conventionally will tend to pull the tool into the material thus making the slot larger in width by a few thousands than the tool.

It all depends on what the goal is. If its something that is just quick and dirty then its not big deal. If the slot needs to be something like +0.0005" -0.0" then a little more thought and effort needs to be put into it.

[Tom-AMS]

Whenever I do deep slots in plastic or wood, I use a mill that's smaller than the slot width. Is that a good advice for metal milling as well?

yes this is why i included " AND if the slot's width does not require great precision" in my earlier reply :-)
ERUS gave a good explanation.

when cutting metal, keep the endmill length sticking out of the tool holder as short as possible. Rigidity of both the tool and the work piece, and not recutting chips is a key factor.

When I cut a slot, such as for a key that requires greater accuracy, I use a next size smaller endmill; I use G-Wizard (set for the mat'l being cut) to compare the different mills I have available. For example
- carbide endmill is more rigid than HSS, but for some material a sharper HSS endmill may be more suit able.
- extra chip clearance of a 2 Flute vs 4 flute may be better, depending on the mat'l chip formation.
- flute length differences, shorter is better
- diameter differences; sometimes using a metric endmill instead of the next size smaller imperial diameter endmill will offer enough more rigidity to get better Mat'l Removal Rate.
- optimal depth of cut vs. tool flex
unlike most feed & speed calculators, G-Wizard computes all the variable to let you choose a tool with speed & feeds to give you the best MR Raste that will yield reliable tool lfe and part accuracy. Saves a lot of grief caused by breaking tools :-)

In many cases, when cutting slots I find a stubby, 3-flute, carbide endmill, with good chip evacuation, and GW's recommended F&S gives me the fastest MMR, with the lowest tool breakage risks.
Respects,
Tom - AMS
automotivemachine.com

[CNCenforced]

If you are still in need of help, let me know, I live in San Antonio TX by the way.