[X35 Design]

I am guessing that I could probably go straight to 1" but haven't tried yet. I drill the first two depths with the 3/4" and use a 1/2" endmill to pocket them out, then drill to the bottom with 3/4 then 1"

Just the fogbuster nozzle does a surprisingly good job of getting the chips out, just have to not drown it in coolant or the chips will stick to the sides and not fly away in the air blast. To blow air straight from the bottom with the 3/8npt hole would be even better I'm sure, and will get tested next time.

What are the pro/con to doing a spiraling down ramp plunge style of cutting vs milling from the side of the cutter?

Did you ever try to just dive right in with the 1" drill bit without using the 3/4" first? I wouldn't be surprised at all if the Tormach in low gear has more torque than my machine, and I can just go straight to the full diameter, provided the pecks are shallow enough.

Wow, you really are going in deep! I agree with you and the others: You're going to have to reduce your depth of cut considerably. I.d drop it all the way down to .200" and see how it goes. Thankfully, I'm sure you'd be able to increase the width of cut. I wouldn't think .010" would be too much, and that depth/width combination would give you a similar material removal rate.

And about hooking air up to the bottom hole: you have the NPT-threaded hole already, right? Stick a short fitting on there and hook it up to you air compressor. Sure, 80 PSI would probably work better, but 10 PSI would probably be helpful as well. I mean, what are you feeding into you FogBuster? 15 PSI? That blows out chips, right? And it does it from several inches away I bet. Flood might work, do you have that option? If you have thousands of dollars you can retrofit your machine you can try that threw(sic) spindle coolant option someone suggested earlier.

[bill south]

Hirudin;
Without hijacking this thread which is full of information (I too am self-taught wanna be a machinist), what software are you using for your tool setter in post 2?
Bill

[Hirudin]

^ It's SolidCAM with their "2D iMachining" add-on. I don't love it, but it does seem to do a lot of stuff well.
Oops, are you asking about the probe routine? I wrote it myself based on something I found on the internet. Send me a PM (or start a thread or something) if that's what you're asking about and I'll send it to you. The main reason I haven't shared it yet is because it still needs some work. In other words: I'm willing to risk my own probe tips, but I'm not too keen on risking other people's.

What are the pro/con to doing a spiraling down ramp plunge style of cutting vs milling from the side of the cutter?

I wish I could give you a better answer than I can. :/ All I can say with confidence that is I frequently get chip-weld when plunging. These days I crank up the coolant knobs on my FogBuster when doing any plunging, which seems to help a lot.

I wouldn't be surprised if it's because a good portion of the tool is cutting at an inefficient speed - the center of the tool technically has a cutting speed of "0". So, if you're spinning a 1/2" tool at 1200 RPM the outside of the bottom edge might be going the correct speed, but halfway in, it's the equivalent of a 1/4" tool rotating at 1200 RPM, then if you divide the diameter in half again in it's like an 1/8" tool spinning at 1200 RPM. Eventually, the center might-as-well-not be spinning at all. Since the machine is still forcing the bit through the metal I'm guessing it makes a lot of heat that eventually leads to melting and chip-weld. - I hope this explanation makes a little sense.

I imagine evacuating the chips while plunging is much more difficult as well, compounding the problem. On top of all that, it's harder for coolant to get to the cutting lips if they're too deep down.

[SCzEngrgGroup]

Doing a straight plunge with any tool is a "stressful" operation, and requires reducing feed by 30-60%. However, doing a helical spiral can be very efficient, and if you keep the angle reasonable (typically 2-5 degrees), you can move surprisingly fast. It won't remove material as quickly as a drill, PROVIDED you have enough power to use the full capability of the drill. On machines this size, and 3/4"-1" drills, you don't have that power. I'd be willing to bet a helical plunge, taking advantage of chip thinning, would be a faster, easier way of getting the job done. To get maximum MRR, use several tools, starting with a short endmill, going as deep as you can with that, then switching to a longer endmill and continuing down. As the tool gets longs, you'll have to reduce MRR to avoid tool deflection. But, with a hole that large, using a 3/4" endmill, you should still be able to do pretty good. As an example, I typically do roughing of pockets in 6061 using a 1/2" HSS 2-flute endmill, running 6000RPM and 77 IPM. Once at depth, I'll use a constant radial engagement of 0.050" at 1/2" DOC and 110 IPM. That clears out pockets pretty darned fast (abour 3 cu. in./min) without stressing the machine at all.

Regards,
Ray L.

[X35 Design]

Is there much of a benefit to having a pilot hole down the center if I did the helical down ramp? The bore is dia 1.368" x 2.3" deep, so a 3/4 endmill could theoretically cut it all in one path spiraling down. Or would it be better to take it in steps outward from the center? Speed is not a huge concern, as long as it comes out nice and doesn't make that godawful screeching sound.

[LeeWay]

You would be cutting almost the full width of that large end mill.
I would say use a 1/2" to 5/8" drill bit first, then you can pretty much blow through when interpolation.

[sansbury]

I'd bet a good six pack that you'll get the hole done faster and better by roughing with a twist drill and taking the rest off with an endmill. I'd consider doing it if only to save on wearing out more-expensive endmills which aren't needed for carving out 90% of the material. You'll also have a lot less chip evacuation issues with a twist drill versus an endmill, which is no small thing in a deep hole like this.

[X35 Design]

More Testing Last night-
I tried a variety of speed/feed, ramping down onto a predrilled hole with a .2 width of cut (2 passes). Went back and tried to side mill at .188 deep passes with .02-.06 thicknesses of cut.

Nothing seems to work very well. The finish is crappy every time. I ran with RPM as low as 400, up to 2000. Feeds from 6-60, nothing seemed to make it happy.

I realize that to use a 6" reach endmill is not an easy thing...but arg!! There must be a magic setting that will work.

Would spending some $$$ on a SECO inserted setup do me any better? Part of me thinks so, but I don't want to spend $300 or so to find out. If I knew it would work, I'd gladly pay more lol...
Considering the Seco Minimaster, or their plunge inserted endmill with 3/4 shank, 1" diameter of cutter
Or buying their combimaster extension to use with my Tormach Inserted 25mm mill to gain the extra length required

Attached is a sad sample finish quality picture

[SCzEngrgGroup]

Perhaps your spindle bearings are not properly pre-loaded? That can cause chatter.

You may well be seeing a limitation of the machine - very deep holes are difficult.

Regards,
Ray L.

[sansbury]

According to FSWizard, a 2FL 6x.750" carbide EM should be run at 5k RPM, .003" WOC, 1.3" DOC, and 54IPM in 6061. Double the feed rate for 4FL. I haven't tried that so don't take my word for it.

FSWizard - Free Advanced CNC Speed and Feed Calculator

Worth a try. My guess, you're going to get some chatter no matter what, if you want really smooth you'd need to take the last pass with a boring head.

[X35 Design]

That is an interesting thought about the bearings, though when I use my 1/2" hi helix carbide mill, I can get beautiful mirror like finishes when running at 3775 rpm and 40-50 feed cutting at 1.44 depth and .02 passes, so I know it is possible to get nice finishes, so I am guessing that they are OK, though I could be totally wrong on that...

Perhaps your spindle bearings are not properly pre-loaded? That can cause chatter.

You may well be seeing a limitation of the machine - very deep holes are difficult.

Regards,
Ray L.

[johnedward]

That is an interesting thought about the bearings, though when I use my 1/2" hi helix carbide mill, I can get beautiful mirror like finishes when running at 3775 rpm and 40-50 feed cutting at 1.44 depth and .02 passes, so I know it is possible to get nice finishes, so I am guessing that they are OK, though I could be totally wrong on that...

the bigger diameter cutter you use the better off you will be to avoid chatter, that and carbide for stiffness unlike what some pseudo-pundits think for these size machines. if your 1/2" carbide works keep using it but for much deeper look at 3/4 to 1" diameter tools.

[SCzEngrgGroup]

the bigger diameter cutter you use the better off you will be to avoid chatter, that and carbide for stiffness unlike what some pseudo-pundits think for these size machines. if your 1/2" carbide works keep using it but for much deeper look at 3/4 to 1" diameter tools.

Once again, it would help if you would READ the posts, before responding. He IS using a 3/4" endmill.

Regards,
Ray L.

[johnedward]

Once again, it would help if you would READ the posts, before responding. He IS using a 3/4" endmill.

Regards,
Ray L.

Then he should move up to 1 inch or as big as he can if he is still getting chatter like i suggested, mmkay?

[vertcnc]

How about following up after the end mill with a boring head. A little time consuming, but would leave a nice finish.

[Hirudin]

Darn, I was hoping going down to 0.2 would be enough. :/

For kicks, maybe testing different depths of cut with that tool on the outside of that piece of stock would be a good idea. Like, just find out if there is ANY hope at all that the tool you already have will work.

I'd try running it along the top, like a facing operation. Take 5-thousandths and see what happens. If it chatters and squeals you just might be SOL. If that works, and if push-comes-to-shove, you could do 300 passes at full width and just get it finished, even if it's going to take 3 hours. Maybe you can get it down to 50 passes at 30-thousandths each.

[LeeWay]

That is a good suggestion, Hirudin. I haven't seen it mentioned, but some aluminum machines better than others. 6061 machines very well. 6063, not so much. It can still be machined, but it is a lot more gummy. I have to go to extremes to get any sort of nice finish with it. It would snap an 1/8th" carbide EM about twice a day, where I typically get one or two changes a month in 6061. That is using the feeds and speeds designed for 6061.
It will finish out with a face mill easy enough, but leaves a peanut butter burr.

[TurboStep]

You may have mentioned how you're holding the 6" end mill but I couldn't find a reference in you posts so this comment may be irrelevant, but I assume that you are holding it directly in the TTS R8 Collet. If this is the case, have you verified how well the collet is mating with the spindle taper? These have been reported not to match terribly well and I know that mine doesn't. This is less critical for TTS holders due to the flange contacting the spindle nose so it hasn't concerned my up to now, and as you also say:

...when I use my 1/2" hi helix carbide mill, I can get beautiful mirror like finishes ... so I know it is possible to get nice finishes...

but it won't improve your finish if the end mill is only being pinched at then end of the collet. I would definitely recommend checking the contact area with engineers blue.
Have you considered making this item in 2 parts as I suggested in a previous post?
Step

[X35 Design]

Hey guys
Lots of good ideas here. I will make some more tests today.

A redesign is definitely part of the plan. This is way too much pita.

I have the tts press fit collar on the shank. I also have one without the shank collar and the results are the same...

I really appreciate the help with this challenge. I'll be back with the results later.





Sent from my iPad using Tapatalk

[X35 Design]

I guess it has been a while, but I did get this to work.

I bought a long XMill from YG USA (through Travers Tool)

http://www.yg1usa.com/itemimage/drill/394-bottom.jpg

YG-1: BEST VALUE IN THE WORLD OF CUTTING TOOLS


I start by drilling the hole up to 3/4" (in two steps) and then use this to circular interpolate the 1.368" dia. hole, ramping it down to the bottom.
Lots of pressure on the fogbuster to keep the chips from clogging up.

It is not super fast, but it gives me the finish I need, so I'm happy.