[X35 Design]

I bought my Tormach to make several parts for a machine I sell. The worst offender is this one, which is made of a 3x3x6.5 aluminum block.

My question is almost one of general machining, but since the Tormach 1100 is all I have, the solution needs to work with it, and not a 40hp Haas or such.

So far I have been drilling and tapping the NPT hole on the one side, then turning the block on the tall end, and drilling /milling in sort of two steps.
Step 1 - drill with 1/2, 3/4, 1, and 1 1/4 bits down to the 3.15 depth and then milling those two contours with the Tormach 25mm inserted endmill
Step 2 - drill as above down tot he 5.45 depth, then finish the bore by ramping down with a long 3/4" endmill

The NPT hole makes a nice vent for most of the chips of Step 1 but Step 2 is the hard one.

I am having trouble with the drills either chattering or stalling out. I bought new Hertel HSS S&D drills for this. I thought I was taking reasonable pecks at .06" each step and RPM in the <300 range for the larger ones.

I am using the Fogbuster from Tormach, with the coolant flowing very generously during these operations, and the air turned up.

Questions-
1. Do I need to step up the holes as I have done? I tried going from 1/2 to 1 1/4 and the result seemed about the same
2. Are my feed/speed reasonable? The recommended ones from GWizard seem really fast and agressive, even at the conservative setting
3. Is there a better set of tools to do this? I am not opposed at all to spend some $ on some good tooling to make these a much more pleasant and secure process, as long as those fancy tools will fit into the 1100.
4. What else am I missing? I am self-taught at all of this, so possibly I am missing something....

Thanks for your help

[Hirudin]

I'm self-taught as well, and I'm using a different machine (a Novakon Torus Pro). Hopefully this will help a little...

Looks like there is a smaller hole at the end of the large hole. Maybe you could also drill that first and hook an air hose or something up to it to help blow chips out. Whenever I use an S&D bit I spray lubricant into the hole after every few pecks, are you using any kind of supplemental lubricant in addition to the FogBuster?

60-thousandth pecks might actually be a little aggressive. When I use large drills I take 0.5 mm (~20 thousandths) pecks. I picked that number because larger pecks would stall the spindle. The largest drill I can remember using was 7/8" though, I was only going ~1.75 deep, and I wasn't doing any pre-drilling. That's several changed variables, I know. :/ I figure the depth is of little consequence though when using a peck cycle, and the fact that you're using a larger drill bit suggests that an even shorter peck might be called-for, then again, with the pre-drilled hole maybe it would basically even out.

Here's a video I recorded a while ago... The first half is drilling with what I'm pretty sure is a 5/8" S&D bit.
https://www.youtube.com/watch?v=4zXj7LT5Q6g

[LSM]

Flood coolant works better for drilling you need the lubrication on those deep holes,
one problem you are running into is with the larger diameter bits when the rpms get low you lose torque.
your peck isn't unreasonable I was pecking 0.100 with a 5/16 .
The other thing to do is go for an aluminum specific bit.
115 to 197 sfm .008 to .010 in per rev.
use an aluminum specific high performance rougher finisher end mill say a 1/2 with 2'' loc for the first 2'' then you have to start going extended reach.
just get the bulk of the material out , use lots of air to get the chips out of the pocket.

forget hsm tool paths you don't have the travel or spindle speed to use that.

use a boring head to get the exact size on your hole

flood coolant for drilling lots of air for pocketing.

[Hirudin]

Pecks of .1 aren't unreasonable for 5/16, but that doesn't say much about 1-1/4 (4 times the diameter, 16 times the area). I found, with large bits my machine can only push the drill for a short period of time. I'm not sure if it's momentum, or maybe the VFD is kicking into overload, or maybe the brief retract is allowing the bit to cool or something. Whatever it is, short pecks work much better with my (similar) machine.

I almost always do full retracts (G83), but maybe the the G73 cycle would be sufficient if you're worried about how long it takes.

[LSM]

The larger the drill diameter the larger the peck you can take and the deeper you can go with out pecking.
you can only push so much diameter until you run out of horsepower, 1.25 at 367 rpm isn't going to cut it way out of the power zone.
try just using a 3/4 bit and then suitable length end mills ,
Ideally you would have threw the spindle coolant and more power.

[Hirudin]

Are you answering the question that was asked LSM?

...
the solution needs to work with [a Tormach], and not a 40hp Haas or such.
...

Just do this. Easy.
https://www.youtube.com/watch?v=CqhL_-hchFo

[Steve Seebold]

I'm self-taught as well, and I'm using a different machine (a Novakon Torus Pro). Hopefully this will help a little...

Looks like there is a smaller hole at the end of the large hole. Maybe you could also drill that first and hook an air hose or something up to it to help blow chips out. Whenever I use an S&D bit I spray lubricant into the hole after every few pecks, are you using any kind of supplemental lubricant in addition to the FogBuster?

60-thousandth pecks might actually be a little aggressive. When I use large drills I take 0.5 mm (~20 thousandths) pecks. I picked that number because larger pecks would stall the spindle. The largest drill I can remember using was 7/8" though, I was only going ~1.75 deep, and I wasn't doing any pre-drilling. That's several changed variables, I know. :/ I figure the depth is of little consequence though when using a peck cycle, and the fact that you're using a larger drill bit suggests that an even shorter peck might be called-for, then again, with the pre-drilled hole maybe it would basically even out.

Here's a video I recorded a while ago... The first half is drilling with what I'm pretty sure is a 5/8" S&D bit.
https://www.youtube.com/watch?v=4zXj7LT5Q6g

You are obviously using a Fog Buster for your spray coolant.

I use the Fog Buster as well, and I love it. I have used one for the last 10 years. When I had my real CNC shop, I had one on every machine.

The Fog Buster is fantastic for contours and surfaces, bit it sucks for drilling, tapping and deep pockets. There just isn't enough air pressure to get coolant to the bottom of the pocket and blow the chips out.

I have one on my PCNC 1100 now, and when I make contours, that's what I use for coolant.

[Moggot]

Out of curiosity, what speed range are you in?

The 1100 has two ranges selected with a belt. The high range allows between 250-5140 RPM, and the low range 100-2000 RPM. The overlap is convenient but, at the extremes, places the motor/VFD into a pretty marginal area of it's capabilities. I suspect that, if you are working predominantly in aluminum, you probably have it set to high, correct? If you haven't already I would suggest that you switch to low range to get the best performance possible at 300rpm.

Do consider the impact that low range will have on other operations though. 2000 RPM will drastically limit what you can do with smaller tools and switching ranges back and forth in the middle of a program would be a huge pain in the neck (though I'm sure someone here will claim they do it all the time without issue). Remember that the 1100 isn't really intended to swing large diameter drills and you may be better off using an endmill to interpolate these holes. Plug some numbers into Gwizard to gain a sense of what sort of parameters will work how they'll impact cycle times.

For reference, maximum spindle power is supposedly reached at around 3000RPM in high range. I'm not sure where that same point is reached in low range.

[sansbury]

At first glance this strikes me as being in the "doable but miserable" category of jobs. Assuming normal tolerances, I'd think you could outsource the big hole to somebody else relatively cheaply--it'd be a fast hit with a >1" coolant-thru drill and a 1.25" endmill (or just the EM), then do the other holes yourself. Even with a 3/4" EM I shudder to think how much chatter and deflection you're going to have at ~6" down. I'd throw this up on MFG.com and see what kind of quotes I got--sometimes it's less than you think. I'd let them source the stock and supply first-op finished parts.

Leaving that aside, which I know isn't what you want, I think the one obvious thing I would change is to use flood coolant. Get yourself a watering can and mix up some suds and pour in a steady stream while it runs, see how that works. Oh yeah, wear a raincoat and keep your mouth closed. The base Tormach flood pump doesn't actually supply a lot of coolant and this is a case where you can't really overdo it. Since you're not going to get a lot of pressure either way, might as well make sure you have enough volume. If it doesn't work, you saved $300 not buying the flood kit.

Does Tormach have a long enough arbor for the 25mm endmill that you could use that for the bottom contour? That would get you a fair bit more rigidity even over the 3/4" EM. If so, I might just stop with the 3/4" drill and plunge into that with the 25mm EM (assuming you have the center-cutting version?) to do the rest.

Anyway, this is one of those parts I could see making one or two of, but if I was going to need a bunch I would look for other options because they're never going to be fun. Not so much 40HP, but deep holes scream for thru coolant. Often literally

EDIT: G-wiz speeds often look high, but if you're not experienced, your intuition (i.e. from woodworking/general tinkering) may not be very good. I use FSWizard which is similar and I've come to trust it a lot more. In particular one of the worst things you can do is feed too *slowly*, especially with carbide, which leads to the tool rubbing rather than cutting, which leads to many things that end with PING as the tool snaps followed by a stream of curse words.

[LSM]

Hirudin get a clue.
that piece of 2'' isn't deep pocketing. actually having owned and used a Tormach yes I did tell how to do it on a Tormach.
in low range once you get below about 900 rpm the torque drops of fairly fast.
It will punch 1/2 and smaller hole all day long not problem in aluminum not so much in steel.
You might get away with using a larger carbide insert drill to get your rpms up
you punch your 1/2 or 3/4 hole then go to work with with your end mills and interpolate.
using high performance aluminum specific end mills will help, you wnt to be running flat out at 5000 rpm
a hole that deep will be crappy so you clean it up with a boring head.

You might get away with using a R8 1'' endmill holder with a long 1'' carbide em once you get down a bit.

now if I had to do that I would put it in the 4 jaw on my hydroshift lathe punch a hole with a and hen clean with a boring bar.

there isn't a quick and easy way to do it with a Tormach

[Hirudin]

I hope the remainder of this thread will help me get a clue. I have a lot to learn.

[X35 Design]

Follow up -

I initially tried drilling on the high speed pulleys, but switched to the low speed pulleys. I noticed my 3/4 bit had some chip broken on the cutting edge of one of the flutes so that was not helping any...

Thankfully the bore at the bottom is only for press fitting a liner, so it doesn't have to be super pretty.

Oddly I tried a 47/64 bit that I had from an unknown vendor/source, and it cut much more easily and happily.

One question though, if I want to drill up to a 1.25" hole before interpolating the final bore at the bottom, would it be better to go 1/2 to 3/4 to 1 to 1 1/4, or just go from 1/2 to 1 1/4" drill?

Also..if I could drill a .156 hole from the bottom and connect air to that, how much advantage would that give me? The hole would not be at the center of the big hole, but about .3 from the center. I may be able to change the 2" dimension to 1.85 and then drill a dia. .156 from the bottom and the 1/2" could just intersect at the very bottom.

Also, to keep the depth of drilling down, I plan to do this in 3 stages. Drill and mill out the 1.758, then the 1.60 level, and then all the rest of the way to the bottom.

Like this sketch, as viewed from the bottom of the block:

[X35 Design]

Another question..assuming I could get good airflow through the .156 hole idea above to blow the chips out, could I then do helical interpolation to make the holes instead of drilling?

[TurboStep]

Does it really have to be machined out of one singe piece? Would it be possible to make a separate end plate? The first 2 diameters could be machined from one end and the last diameter from the other. The end plate would then just bolt on.
Step

[LSM]

The idea is to drill the 1/2 or 3/4 hole then use that to plunge the end mill in that hole,
then you do a spiral interpolations so you are using the side to do the cutting not the end.
it takes a good air flow to blow the chips out like 60 to 80 psi out of a blow gun.

you are dead in the water if your drill bit is even slightly dull.

try running the 1.25 bit at about 900 rpm with about .008 per rev feed with flood cooling
see if that gives enough torque, that's pushing the sfm so it needs cooling or aluminum will start sticking to the bit
you have to feed it heavy enough so the bit is cutting not rubbing.
plug the holes so the coolant doesn't drain out the bottom you want the hole to fill up every time the bit retracts on a peck

when the drill chatters you probably aren't feeding hard enough, when it stalls you ran out of power

[X35 Design]

Update-
I've figured out the drilling issues, but now the milling of the lowest portion is giving me some trouble. The two upper sections I have milling very nicely using a 1/2" high helix carbide mill.

I have drilled out the hole to the bottom with a 1" dia. and tried to side mill to the final diameter as you suggest.

I am using this endmill:
Square End Mills | MSCDirect.com
It has a reach of 6", OAL of 8.25" 4 flutes HSS with 2" length of cut

The bottom portion is 2.3" depth, so I set it to mill it in two depths at 1.15" each. I put that info into Gwizard and got that it should be a .002 cut per pass
to avoid excess deflection. I can't recall the RPM but I think it was 2700ish and 45 feed rate. When I ran it like this, it shreiked and made the most horrible noises until I backed
the RPM down to around 700, and even then it was not great, and the finish was pretty bad.

Should I do it in more, shorter depth of cut passes? Did I put something wrong into Gwizard possibly to get those #s? I am going to try again tonight so any advice would be very appreciated.
Would it be any better to interpolate and ramp down into the hole instead?

Thanks

The idea is to drill the 1/2 or 3/4 hole then use that to plunge the end mill in that hole,
then you do a spiral interpolations so you are using the side to do the cutting not the end.
it takes a good air flow to blow the chips out like 60 to 80 psi out of a blow gun.

you are dead in the water if your drill bit is even slightly dull.

try running the 1.25 bit at about 900 rpm with about .008 per rev feed with flood cooling
see if that gives enough torque, that's pushing the sfm so it needs cooling or aluminum will start sticking to the bit
you have to feed it heavy enough so the bit is cutting not rubbing.
plug the holes so the coolant doesn't drain out the bottom you want the hole to fill up every time the bit retracts on a peck

when the drill chatters you probably aren't feeding hard enough, when it stalls you ran out of power

[SCzEngrgGroup]

Reduce your depth of cut. With a tool that long, 1.15" is way too deep, even at shallow width. You'd do much better taking fast, shallow, narrow cuts. You need to keep a good heavy chipload, but minimize deflection. That is a REALLY Long tool! You may also be hitting a machine resonance, in which case you'll have the change RPM to get away from it. Either that, or get a toll with a different number of flutes.

Regards,
Ray L.

[Hirudin]

I've figured out the drilling issues

Cool! What are you doing?

[X35 Design]

A combination of:
1. Proper speed/feed (Gwiz does work, just need to move the slider to the second from leftmost position)
2. Use the low speed belt position
3. Drilling only at 3/4 and 1.0" diameters, use the endmill for the rest
4. Shoot wd40 in the hole from time to time while drilling, every 4-5 pecks seems to work
5. Pecking .032-.06 at a time

It's not perfect, as I have to babysit to do the WD40 spraying, but it works well enough without getting itself stuck.
WD40 is probably not the greatest lubricant to use, but it was nearby and has the spray straw thing which makes it handy.

Didn't get to try the milling, as I gave up for the night after I broke my $150 threadmill by specifying an overcut of .4 instead of .04" and didn't realize until it was too late. Arg....:nono:

Cool! What are you doing?

[Hirudin]

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.