Table jumps around when drilling with an end mill

I think I know what's happening, but I'd like people's take on this:
I was drilling six 5/16" holes (in a line, spaced 0.4037" apart),
carefully centering the Millrite spindle over the crossed layout lines, and drilling using a two-flute 5/16" endmill held in a 3/8" R-8 collet, with the workpiece (mild steel) held in the mill vice, and black sulfur oil brushed on as the lubricant/coolant. The table X and Y ways are clamped, and the quill is moved manually to drive the endmill into the work. As drilling proceeded, I continually brushed the chips away and replenished the oil.
For most of the holes, it was slow, but no drama and the holes ended up where they belonged.
For two holes, the table jumped around visibly, and the holes ended up displaced.
The holes are all a tight fit on a 5/16" drill rod, but there are signs of galling in the bores of a few. The endmill is undamaged, and still quite sharp.
My theory is that a chip managed to get in between the side of the mill and the wall of the bore and welded to the wall, only to be torn loose a short while later, and that this is what generated the large forces needed to throw the machine table around. The hole sometimes ended up displaced because the table ended up somewhere else from intended. This would be more likely near the beginning of the drilling operation than the end, and the more wall there is, the more constrained the table is by the stubbly little endmill captured by the hole it just made.
I suspect that a 1/4" twist drill followed by boring to 5/16" may be faster and more reliable, and less dramatic.
Comments?
Joe Gwinn
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

you nailed it on the head. end mills really aren't designed for drilling. even ones that say "center cutting" will wind up pinching a chip between the face or wall of the bore and the mill. only takes 1-2 thou to set that galling and vibration up. better to have just drilled them out without a mill, but otherwise, yes use a drill to get some clearance and then finish with the mill so you have less chance of the chip loading.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

A few thoughts come to mind. You might want a four flute for that, as a two flute generally is better for aluminum and other lighter materials. (Two flutes just aren't as rigid, and also wear faster, and generally have a more radical rake meant for softer material). Second, did you consistently dial the table to remove the backlash? Sometimes people inadvertently dial back a little to locate the cutting tool where they want it, but you have to do a final approach it in the same direction each time so the table's pressure on the feed screw isn't just "free floating". You may also be developing a little bit of play in the spindle, too, but that may be for a couple of reasons that I won't go into. Lastly, I don't know that I would do that in one pass, as you pointed out, a pilot hole is always a good idea, and putting the wear on a center drill and drill (something you can sharpen yourself) is a LOT less expensive than sending out your endmills to the tool grinder. It's not always easy to tell if your endmill is sharp, signs of galling in the bore really is a huge indication that it needs to be sharpened because it's probably the hollow-ground secondary peak possibly starting to drag- that means your primary edge is toast.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

[snip]
I have a few 4-flute mills that size, none center-cutting (if memory serves). But, as discussed before, roughing out with a 1/4" twist drill is probably a good idea.

I didn't dial it in at all, I put a conical-point Starrett edgefinder in the 1/2" R8 collet, centered it, and steered the table so the cone point is exactly over the crosshair. This is verified by carefully bringing the cone point down and kissing the workpiece, making a very small mark that landed exactly in the intersection of the two scribed lines.
The table is then clamped, and is not expected to move. Quite the contrary.

It's certainly possible in a machine made in 1965. How do I test this?

It looks and feels pretty sharp, but roughing with a twist drill seems like a real good idea.
Joe Gwinn
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
Joseph Gwinn wrote:

Put a dial indicator against the side of the spindle (not the quill) and apply force to the spindle, possibly by a solid bar in a collet. apply about 50 Lbs force radially both toward and away from the indicator. A movement of .001" or so is not a surprise as the non-rotating bearings have clearance that is supposed to be filled by the bearing lube. This much radial play will not happen when the spindle is running.
If the movement is more than .001" you can then move up the assembly, first to the quill, then to the main spindle housing, and wee how much movement you get at each part. If this is a lighter machine, you may have to mount the indicator support to the head to separate flex in the vertical column from the quill and spindle.
If the play is in the spindle, you may be able to tighten a nut on the spindle to take up the slack in the bearings. Depending on the bearing type and lube used, you may want to go to zero clearance, or leave some clearance there to be taken up by the lube. Without specific instructions, you may need to creep up on it until the results improve. Or, leave well enough alone unless you are sure there is a problem here.
Jon
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

Thanks. I'll try this.
The bearings do sound OK.
Joe Gwinn
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

Oh, and you can't put a 5/16 shank in a 3/8 collet, you might get away with a 1/64 difference but even that's not real great. If you did that, that is probably a large part of what the problem is and your collet is probably not real happy now either.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

No, the shank on the endmill is 3/8, and fits the collet perfectly.
Joe Gwinn
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
Joseph Gwinn wrote:

[snipp]
Lesson learned (?): 1.) Facemills aren't good for drilling, because they cut on the side too. 2.) Your spindle needs an overhaul before doing 1.) again.
Nick
--
***********************************
*** Available now in NZ and AUS ***
  Click to see the full signature.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

That should be an advantage in a rigid mill, I would think: the hole will go where the mill wants it to go, even if the hole becomes a bit larger. But these holes are tight on a 5/16" drill blank, so it can't be much.

Why? Chip welding happens even to new machines. Nor does the spindle on my machine seem all that loose. What moved was the table, not the spindle.
What I've found with this machine is not that things are worn, but that they are caked with hardened oil, which gets in the way in various ways.
Anyway, how does one measure the spindle play without special equipment?
Joe Gwinn
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
Joseph Gwinn wrote:

Wrong concept! Repeat: A mill is bad for drilling, because it cuts on the side, a drill does not (except if you abuse it; we all did that). Also, a mill is not self centering, because he has a flat face, a drill has a conical face just for that purpose. As soon as one of the face cutting edges of a mill gets a bit more work, the mill (or the spindle) will bend and will cut on the side and he will be happily dig on that side until the deflection is too big for the cutting force. Then he will bounce back and try to catch the other side. :-) As gunner said, bore the hole (as big as possible) and then use the mill to drill if you need to. Abuse: If I need to make a bigger hole than I have a drill or a mill, I use a mill and feed quickly. That *guarantees* to make a bigger hole (and it *is* a hack). That's why they do ramping for milling slots and do not plunge mill the start. And if you need more passes, all are done in the same direction (preferably). Mills *do* bend under cutting forces.
If you want to locate holes precisely, start with a center drill (or better with a NC-starter drill, they are even better) and drill the hole with a drill. The drill will follow exactly where you started.

Not chip welding. Make a test and feed a face mill (drilling op) *fast*. You will notice that the mill tumbles. Even with the table clamped like mad.

Dial-indicator and some bar in a collet. Grab the bar and move it. The dial-indicator's tip is on the spindle nose or the collet holder (depending on your setup).
This discussion only reminds me, that I have to overhaul my spindle. :-)))
Nick
--
***********************************
*** Available now in NZ and AUS ***
  Click to see the full signature.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

Yep!! I agree.

That's true! End mills are not intended to be used as a drill-----there are far better ways to remove the metal. The fit may be tight, but the hole may or may not be round, and likely has a pattern, developed by the end mill walking about. If you don't have a reamer, and don't wish to bore the holes, start with a center drill, followed by an undersized drill, then open the hole to the desired drill size. Common practice is to drill the hole 1/64" undersized, then open it. If your drills don't cut size, drill the hole 1/32" undersized.
. Also, a mill is not

That's not true. An end mill, typically, is short and rigid and intended to cut where you aim it. Even when drilling. You get in trouble with drilling with an end mill because there's no provision for discharging the volume and shape of chip generated, so you get chip loading of the flutes, resulting in a winging end mill. It's not uncommon to get a hole that's generously oversized as a result, assuming all flutes aren't loaded equally. If they are, the end mill more or less refuses to cut.

That's not true----although I fully agree with starting holes with either a center drill or spotting drill. Twist drills are notorious for not drilling straight, round or on size holes. The slightest thing will deflect the point, resulting in a hole that runs off in any direction. You see evidence of this when you drill a long object in the lathe. Rarely does the hole meet at the center when drilled from both ends. If you want holes located precisely, the best way to achieve that is to rough drill, then bore on location. While I don't endorse the use of end mills, they will provide a hole on location, but you risk the oversized condition so common with any tool that is side cutting.
Harold
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

I did a trial piece with the 1/4" roughing twist drill followed by either the same 5/16" endmill or by boring. What a difference! That endmill really needed the hole to be roughed out first. It was far faster to rough drill then use the endmill, rather than to push through with the endmill alone. The holes were quite tight on a 5/16 drill blank, especially the last holes drilled, as I gained experience.
Boring also worked well, but it was slow and fiddly to hit the desired diameter accurately. Next time, I would use a 9/32" roughing drill, to reduce the number of passes required. The advantage of boring would be that I can then easily make the holes slightly larger than 5/16", useful so that the jig doesn't require too much precision (and tramming of floppy drill presses) to be practical. An alternative is to lap the holes with a brass rod, after the plate has been hardened.
So, it has to have been chip packing between the face of the endmill and the bottom of the hole that was causing the problem.
The holes are still not quite where they belong, especially in the X direction. My suspicion is that the X table lock isn't tight enough, allowing some movement. The little cast iron knob on that lock is not original, and is far too small for the purpose. It looks like one I've seen in the MSC catalog. I have not seen anything suitable in the MSC catalog: the knob requires a deep 3/8-16 thread and a nose not exceeding (or machinable to) 3/4" in diameter, to fit into a spotfaced ~0.100" recess in the bottom of the saddle. I already have a brass washer down there, to reduce friction between knob and saddle, so more of the tightening effort goes into clamping force, and less into hurting my hand.
I had to turn the tip of the knob I have down to fit into the recess to get even semi-solid clamping action. Not having a lathe, I used the mill (running in reverse - no, the boring head cannot unscrew) with a backwards boring bar to bore an inverse ~0.750" hole in the tip of the knob. Champing that odd-shaped knob to the table with hub straight up was quite the trick. I used a clamping ring from a 5C collet holder as a rest (to clear the knob's hub) and clamped the knob's arms to the table through the ring.
Joe Gwinn
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
Harold and Susan Vordos wrote:

It is true. :-) It is not *self*centering. Self, that's the difference. It sure is rigid. But it also doesn't cut where it was aimed to. That's why final cuts are done. If you have made a pilot hole and move the table a tad and then drill, the drill will bend and start where you centered. We both know where it will *not* end. :-)

Not my observation. Even if the chips come out freely (or you wash them out with coolant). If only one edge on the face has a bit more to cut (or is standing out just a tad more) the troubles beginn. I don't think it is chiploading. But we both agree on what happens.

Talking of mills? ACK.

They do that (with a little trick). And if they aren't hand-ground by me. :-) The trick is: If the work is in a vise and do it on a drill press, rotate the vise every once and a while for a quarter.

The tailstock is nearly never absolutely on center and dead parallel to the spindle. Much better in the mill.

ACK
ACK. Hard for small holes.

I never checked how much off-center the holes were when drilling with mills. Because when I did, I never cared for the quality.
Nick
--
***********************************
*** Available now in NZ and AUS ***
  Click to see the full signature.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

Ah! I see we're talking about two different things. Yes, I agree-----a drill is self centering in that it will go to a pre-drilled location even if the location is not in line with the spindle. That, indeed, is self centering. I should have said that an end mill will cut where you want it to cut----or----said another way-----it centers where it is located-----but that isn't the same thing you said. I was wrong.

Depends on the rigidity of the machine. Spindly machines would have some difficulty with such an operation, but they'd have difficulty with milling, too. A rigid machine won't give a damn if there's dissimilar amounts of metal to cut, not as long as the chips can be easily discharged. That's a tall order when drilling with an end mill unless the size of the chip is smaller than the width of the flute.
I've used end mills to properly locate holes that are in the wrong place enough times to know it works fine----especially if you're opening the hole by a small amount, so the chip is insignificant. I think I can honestly say that such an operation is the only time I endorse the use of end mills for drilling.

I've drilled more than my fair share of holes in a mill that was dialed in within limits to find the hole coming out in the wrong place. It's the nature of twist drills to drift, often for what appears to be no apparent reason. That's not to say that they can't drill straight holes, but it's not guaranteed. Chances are better that a hole will drift, regardless of how it's drilled, than it won't. The amount of drift is the only question I'd have, not that it would, or wouldn't.

It isn't attributed to that alone. I've drilled holes in one piece that come together beautifully, followed by one that is off a half drill diameter. Twist drills simply do not drill straight holes reliably. If they did, there'd be little need for gun drills.
Harold
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

Two things make me wonder about this:
1. You say it's worse at the start of the cut. It makes sense in that there is not as much wall to constrain the endmill at the start of the cut. At the start of the cut, however, there is also not much wall for the chip to weld to and throw the mill around.
2. Why would a drill bit be any better? The difference between an end mill and a drill bit is in the cutting end - the flutes and lands are just about the same. If it's chips welding to the side of the hole, they should be equally susceptible to it.
It's my guess that it's the cutting end that is doing the grabbing. Possibly due to chips welding on to the end mill itself, rather than the workpiece.
Try Aluma-Tap or another aluminum cutting fluid rather than threading oil. Run the cutter fast - a faster cutter has less time to overcome the inertia of the table. Use a drill bit instead. If you need a flat bottomed hole, start with a drill bit and finish up with an end mill. The drill bit could be full size, or slightly smaller. If nothing else works, you might try tightening up the quill locks so the end mill cannot pull the bit ahead as easily.
John Martin
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

That's my assumption and impression. No measurement or careful observation made.

The drill bit is smaller than final size, has a conical point, and is intended for the purpose. The twist drill would be followed up with a boring head and bit to make the final bore.

It's certainly possible, and the endmill would soon destroy the evidence.
I'm thinking that a 1/4" twist drill for roughing followed by the same 5/16" endmill for the final pass might be the ticket, and be a lot quicker than a boring head (albeit less precise).

Why would aluma-tap be better in steel than black sulfur oil? I have some Tap-Free on hand; I could try this. Now that you mentione it, Tap-Free worked better for countersinking in my now-neglected floppy too-fast drill press.
Faster may well help, but I'd like to understand and eliminate the root cause.

I don't need the flat bottom. What I need is an accurately placed and sized through hole. This is a dry run before I try it in A2 or O1 steel. The workpiece will become a woodworking drill jig.
Thanks,
Joe Gwinn
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
flat bottom. What I need is an accurately placed and

Joe,
You are working way too hard for a drill jig. Make the jig from aluminum or Plexiglas and use drill guide bushings.
See McMaster Carr Pg.2530 to 2536 http://www.mcmaster.com/
--

Roger Shoaf

About the time I had mastered getting the toothpaste back in the tube, then
  Click to see the full signature.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

I did think of this, but the holes are too close together for standard bushings to fit. Plexiglas isn't likely to stand up, so it would have to be aluminum.
Actually, the holes have to be pretty good for a press fit to be reliable, and have to be accurately located, so I might well have the same issues, only with a larger hole and a softer material.
The dry run isn't because A2 and O1 are so difficult to handle, it's because they are expensive so I want to learn on cheap stuff. I'm still learning this mil.
Joe Gwinn
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

I have made a bunch of drilling jigs out of both plex and aluminum. For close holes you can use the thin walled bushings and for fit you can get knerled bushings or just use a dab of CA glue. If the holes are so close that even the thin walled bushings are no good, then still make the jig from aluminum or plex, but make the guide bushing from O1 and press that into the plate.
Trying to make the whole jig out of steel also has disadvantages. First you have a large plate to heat treat, so DIY with a torch is not going to happen, and when you eventually get wear in the holes, you are facing an expensive repair, whereas if you use bushings you remove the oversize hoes and replace only the worn components.
How close does the hole placement have to be? Your end product is going to be wood, and you are still using a drill bit to make the hole. If the design calls for a +-.005 placement you are going to have big problems anyway.
--
Roger Shoaf
If you are not part of the solution, you are not dissolved in the solvent.
  Click to see the full signature.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

Polytechforum.com is a website by engineers for engineers. It is not affiliated with any of manufacturers or vendors discussed here. All logos and trade names are the property of their respective owners.