[whitehedr]

Well, I was able to find a 3/8-16 in a suitable length that allow me to get my 11/16 size cutter spinning. That is the good news. The bad news is my machine makes an egg shaped hole when I use that large 2 flute cutter. The first test hole was an absolute disaster. I tightened all my locks and the vise as tight as I could get it and the hole did get better but still not close enough in my estimation. I had an email conversation with Hoss and he told me if I had more than say .005 slop in the hole it would not be a good thing as far as accuracy in the Y axis. The first hole was .008-.010 out of round. The second hole was .005 .007 out of round. The head was bouncing around pretty good while I was cutting and I was going down at .001 size bites. I tried slow spindle speed and high spindle speed with high speed seeming to give the better results. I think I am going to try and find a local shop with a beefier mill to cut this hole. I could possibly try and shim it but I do not like that option. Anybody have any other comments, concerns or criticisms?

RWW

[SCzEngrgGroup]

You give nowhere near enough information for anyone to help you. It would sure help if we knew:

What machine are you running?
What material are you drilling?
Are you drilling with an endmill??
What is it you're trying to accomplish?

Regards,
Ray L.

[whitehedr]

Ray,

Here is more info for ya'll.

Grizzly X2 Mini-mill
Drilling with an 11/16 2 flute endmill
Material is aluminum
Hole depth is .285
Hole diameter is .6875
Use is the Y axis spacer block that Hoss designed for his X2 CNC Conversion.

The hole is the thrust bearing for the Y axis ball screw.

There are two holes for the thrust washers. One on the inboard side and one on the outboard side of the Spacer block. They are held in position by two jamb nuts on the ball screw on the out board side of the spacer block.

There is also a thru hole of .4730 diameter for the ball screw to pass through. The shaft of the ball screw has been machined to about .375 which allows the thrust washers to slide over the ball screw shaft.

I have a message in to Hoss to get his opinion on another concern of mine.
I also mentioned my test hole failures so maybe he will have some insight on what I need to do.

Sorry I was not clear in my other post on what I was trying to accomplish.

RWW

[SCzEngrgGroup]

Well, you've got a couple of problems. First, endmills make lousy drills. They won't make a terribly round hole. Seconds, trying to use a large endmill, or drill, in a flexy little machine like an X2 will aggravate things, and the machine will be flexing all over the place in response to the high cutting forces. You'll get a far better result with drill bits, starting with a smallish one, and working your way up to a large one. If you must use and endmill to get to final size, pre-drill the hole as large as you can first. But it still won't come out terribly round. And a 4-flute will probably work better than a 2-flute.

Regards,
Ray L.

[Starleper1]

The best way to accomplish this is to helix ramp with a smaller endmill. Like Ray said drilling with an endmill on a small mill is very tough to do accurately. Especially for a bearing bore.

Reading back seeing that you said it is for the Y axis, I assume you don't have CNC capabilities yet. In this case I would try using drills and a boring head to get the final size.

[br1]

Have you checked for backlash?

[yantra3d]

Nothing to add really but I can vouch for Ray's comments regarding the large endmill on the small mill. I have an x3 and I don't bother using anything larger than a 1/2" endmill. Over 1/2 puts too much cutting stress on the mill and will lose cutting accuracy. Part of learning the limitations of your machine.

Both alternatives recommended here would yield better results (or atleast be less stressful on your machine).

[yantra3d]

Also, if you require he close tolerance for a bearing hole then you might consider investing in a reamer and finishing the hole that way. Another alternave...

[Crevice Reamer]

From the Grizzly G8689 page:

Description
Now here is a mini milling machine that has more features than some Mill/Drills and is affordable for everyone! This little brute will handle any kind of job up to 1/2" drilling, 1/2" end mills and 1" facing. No belt changes necessary! The variable speed control and gear drive saves you time and hassle. Truly, a remarkable machine.

http://www.grizzly.com/products/g8689

It's a miracle you haven't shredded your plastic gears yet.

CR.

[whitehedr]

Well guys, I did have an epiphany last night when I was trying to fall asleep and failing miserably because of thinking about my problem with the mill and
the wind howling outside the house. Damn it was a miserable night, but anyway (Drum roll please) SNEAK up on the hole by starting small and remove less material. DUH DUH DUH on my part.

Now my next question in this endeavor ... should I drill the through hole first or sneak up up on the counter bore hole and then drill the through hole. I am guessing that drilling the through hole first is the correct answer as having the through hole will make aligning the counter bore hole easier when I flip that bad boy over.

Thank you al for your responses. I DID learn a very valuable lesson here. Start SMALL and work up. Kinda like what you do when reloading. Start small and work up with the powder.

RWW

[Starleper1]

If your interested in converting that X2 to belt drive, hit me up

[whitehedr]

I have a belt drive conversion kit waiting in the wings for the R8 spindle conversion to arrive. They became available yesterday and mine is on the way. Probably gonna go under the Christmas tree though. I only want to take that thing apart one time.

RWW

[whitehedr]

Well I had a real good test today. I drilled the through hole first and then snuck up on the counter bore by utilizing two preliminary cutters before going to the final size. The mill did a real nice job when making smaller cuts. Here is a video of most of the cutting. Not a lot of chatter and the final hole is da** near perfect. I am really happy!!!!

RWW

[ame="http://www.youtube.com/watch?v=RN7fXP0BSXo"]YouTube- Test hole for thrust bearing web.mov[/ame]

[Starleper1]

Nice job. One suggestion though, don't start the endmill in the work piece. Stay above and slowly feed down.

[whitehedr]

Thanks for the tip on starting the cutter Starleper1. I am going to make the part today.

RWW

[cornbinder23]

just another note on starleper response you probably dont want to stop the cutter in the workpeice either, raise it out of the workpiece first

[SCzEngrgGroup]

So, almost 9 minutes to drill a hole less than an inch deep? You're feeding WAY too slow, which will dull your tools very quickly. For that size endmill, you should be at about 1500 RPM, and feeding about 10 IPM, which would make that cut in under 10 seconds. Even allowing for the flexy X2, it should not have taken more than a minute.

Calculate RPM using: RPM = SFPM * 4 / Diameter
SFPM is 300-400 for aluminum, 80-100 for steel, 30-50 for stainless
Calculate Feed using: Feed = RPM * #Flutes * Chipload
Calculate Chipload using: Chipload = 0.004" * Diameter

These will get you in the ballpark, On an X2, you may have to reduce chipload, but don't reduce it any more than necessary to maintain good surface finish. A too light chipload will ruin tools MUCH faster than a too heavy chipload.

Regards,
Ray L.

[whitehedr]

Thanks guys, Pleaase keep the tips a flowwing.

RWW

[Starleper1]

tips come from experience. There's definitely a wealth of wisdom here.

[whitehedr]

Well, I am now at a standstill until I can get my hands on a new
M12 drawbar. Some how I managed to strip the threads on the one I have.

All the local hardware stores have some metric cap screws, but they are either
to big or to short or the wrong thread pitch. There is one more store in my area that might have what I need. I hope they are open on Saturday Morning. I do have a replacement on order with LMS.

I was working on the stepper motor mount for the Y axis and the drawbar jammed while I was changing out my drill chuck for a collet. When I finally got it free the end was pretty buggered up and now it will not hold a collet tight.

I guess I will do some of the wiring I need to do for a control box while I wait. That and get ready for Christmas.

Wish me luck tomorrow when I once again try and find something local that will work.

RWW