X Axis Stepper Mount

[whitehedr]

Here is the video I made showing the cutting of the clearance hole in the X Axis stepper mount with the LMS 4" rotary table. First time I have ever done anything this complex on a mill. I know it is kinda cheesy but at least I was successful in making the part.

RWW

"http://www.youtube.com/watch?v=HBY3HC9NhCs"]YouTube- Stepper Mount LMS Rotary Table.mov

[SCzEngrgGroup]

Looks good! I did my first ones on a lathe. You're lucky to have a rotary table.

Is that a 4-flute endmill? You'll have much better luck with a 2-flute in aluminum. 4-flutes will clog on anything but very light cuts.

Regards,
Ray L.

[whitehedr]

Ray,

I thought you got a better/smoother cut with the 4 flute cutter. Thats why I used it.

RWW

[Crevice Reamer]

Good Job RWW!

CR.

[SCzEngrgGroup]

Ray,

I thought you got a better/smoother cut with the 4 flute cutter. Thats why I used it.

RWW

That can be true, but save it for a light finish pass. In aluminum, you want to stick with 2-flutes for removing material as fast as possible. 4-flutes have much less space to eject chips, and aluminum tends to be "gummy", so the space between the flutes on a 4-flute will clog easily. I do virtually all my work with 2 or 3-flute endmills, and usually use 4-flutes only on steels. A good 2-flute (not the cheap Chinese crap) will still give an excellent surface finish.

Regards,
Ray L.

[whitehedr]

Thanks for end mill 101 Ray. I really do appreciate the tips that come from the masters. I am a complete noob when it comes to making stuff with a mill so all the help I can get is useful to me.

Next up is the mount for the Y axis. I might eve try another video. That was kinda fun as well.

RWW

[bladehunter]

Good to see some actual machining, especially for us, ahem, chip virgins

Look forward to seeing more

[hoss2006]

Nice one Roger, that looks familiar.
Hoss

[BobWarfield]

Cool, and like the man said, it is nice to see some actual machining, even if you're whatever the opposite of a "chip virgin" might be (I shudder to think!).

Some thoughts on flutes and all that jazz:

- It is not a sacred rule that you have to use 2 or 3 flutes on aluminum and reserve 4 flutes for steel. There are good occasions to want to use 4 flutes with aluminum.

- The advantage of more flutes: it is like having a "virtually" faster spindle. All things considered, the 4 flute cuts twice as fast as the 2 flute for a given spindle rpm. That means you can feed it faster.

- The dark side of the flutes, as Ray mentions, is chip clearance. In a confined situation, the chips pile up, stick to the cutter, and eventually you can even wind up with them welded on which makes a real mess. Don't worry, if you are curious, it will happen to you sooner or later on your journey. Wait for it, it is not a thing to wish for too soon!

- With fewer flutes, the chips have more room to escape.

- The 3 flute is a wonderful compromise as it cuts 50% faster yet has adequate chip clearance for even tight situations in aluminum.

- You can use a 4 flute productively whenever you are performing an operation that naturally leaves room for the chips. Cutting a full width slot increasingly deep like you were doing is not one of those cases. OTOH, you didn't go all that deep, so you got away with it. Some judgement is called for there, obviously.

- I like 4 flutes when machining around the outside of a part, instead of being down in a slot or pocket. Lots of room for the chips to go. They can just fall off the part entirely in many cases.

- In the video, you've just let your chips pile up, but you can help that out too. Get a little air jet going. You don't need much pressure, just get it directed where you're cutting and the chips will be cleared. Recutting chips is hard on the cutter and messes up your surface finish anyway. Really nice to have that air jet.

- A little coolant can make the chips less likely to weld. WD-40 is an easy solution for aluminum. Kerosene (quite a bit of it in the WD-40, actually) also works. Get a pump sprayer and the big can, it's cheaper than the aerosols.

If wanted to do the job you showed with a 4 flute, here is what I'd do:

- Start with a central hole done with a twist bill that is larger than your endmill.

- Drop the endmill down the hole and move the X axis to engage the cut. Take relatively light cuts, certainly less than 1/4 of the endmill's diameter.

- You'll need successive rotations while moving the table to engage wider and wider cuts, but you can feed pretty quickly with a 4 flute at those DOC's. Probably faster than you can turn that rotab handle if your setup is rigid enough!

- Put a little shot of WD-40 on it each revolution.

- Keep an air jet on it.

The chips will fall out the hole at bottom and out of the way. All in all, probably faster to go the 2 or 3 flute.

BTW, next time you have a job like that, rather than stopping to downfeed, try downfeeding while you keep rotating the work (or feeding in a straight line). This is the "ramping" or "helical" move you see CNC's make a lot to start a cut. With handwheels, you'll be amazed at how much easier it is to turn them than to plunge cut. Much smoother too!

Now you know why the CNC's do that.

Cheers,

BW

[SCzEngrgGroup]

Alll good advice. One additional thing to keep in mind - There is a tendency amongst "newbies" to try to "go easy", using higher RPM, and lower feedrates. This is actually bad, as it will lead to heating of the tool, welding of the chips to the tool, and very slow removal rates. The right way to go is pick your RPM (based on SFPM), then push the feedrate as hard as you can, until either surface finish degrades, or the machine starts complaining (spindle stalling, machine shaking, etc.). The idea is to keep the chipload high (but not TOO high - aim for ~0.004"/inch of tool diameter, so 0.001" for a 1/4" tool), as thicker chips do a far better job of carrying heat away from the tool. If your tools are getting hot, or you're having problems with chips welding to the tool, either increase feedrate, or decrease RPM. Probably a but counter-intuitive, but it works. When you get the right combination of RPM and feedrate, the chips will be coming off hot, the tool will stay cool, you'll need relatively little coolant, and you can remove a lot more material, in a lot less time.

Regards,
Ray L.

[whitehedr]

So to those veteran machinists that viewed the video, did my feedrate look about right for a 4 flute cutter? I tried to maintain a steady rate and not go to slow.

RWW

[BobWarfield]

It's actually pretty slow. A HSS 1/2" 4 flute in aluminum ideally wants to go more like 60 IPM.

With all that said, you're main risk going to slow is it just shortens the cutter life. Going too fast, OTOH, will break something.

Send me a note per the details on this page:

http://www.cnccookbook.com/CCGWizard.html

I'll put you in the G-Wizard Beta Test. G-Wizard has a feeds and speeds calculator you might find handy. It looks like this:



Cheers,

BW