I have a Dore-Westbury milling machine which is in good condition, and allowing for its light construction, has generally given me good results. However, I had a problem recently when I needed to do some heavier work than usual. I needed to cut some 5/16 slots in a 1/2 inch thick cast iron baseplate. I used a sharp 5/16 Dormer long-series slot drill held in a ER25 collet chuck, and took ~100 thou deep cuts at a fairly fast feed (I estimate 3 to 4 inch/min). Spindle speed was
500 rpm. The metal cut cleanly, and everything sounded fine.
However, when I examined the slots I'd cut I found they were very ragged on one side. While the "climb" milling side of the slot was smooth and even, the other side showed tracks corresponding to the 100 thou cuts I'd taken. Surprisingly (to me) the tracks were undercut, i.e in cross-section they would look like a sawtooth, being a few thou deeper at the bottom of each cut.
Is this a problem of machine or technique (or both)? I have searched the various books I have, but can find no explanation. George Thomas in his Model Engineers Workshop Manual give a good analysis of the problems of using end mills to cut slots, but implies that there are no problems with slot drills. What am I doing wrong?
I believe you would get that pattern if the spindle was slightly out of alignment with the column, with the tip of the cutter being slightly further away than it should be. It may not be as serious as it looks; such tracks can look very pronounced even if they are only a fraction of a thou. If it needs correcting, you may be able to shim the head (not familiar with that particular machine).
There may be other explanations involving the dynamics of the cutter, but you may be able to test this by making a similar cut in the other direction. If it is misalignment of the spindle, the pattern will be the same; if it is cutter dynamics, you should get the saw-tooth on the opposite side of the slot.
I check the spindle alignment fairly regularly. Checking just now, using a dial gauge on an arm in the chuck, it's within a thou over 4 inches in both x and y. Moreover, the pattern is always on the "conventional" (i.e non-climb-milling) side of the slot, whether cutting towards or away from the operator, so the problem is not spindle alignment. This is what puzzles me - how can a truly vertical cutter cut at an angle on one side of the slot?
I check the spindle alignment fairly regularly. Checking just now, using a dial gauge on an arm in the chuck, it's within a thou over 4 inches in both x and y. Moreover, the pattern is always on the "conventional" (i.e non-climb-milling) side of the slot, whether cutting towards or away from the operator, so the problem is not spindle alignment. This is what puzzles me - how can a truly vertical cutter cut at an angle on one side of the slot?
Mike
Is the cutter flexing? It obviously does flex like any loaded beam, but is perhaps the flexing the cause of your problem?
I've never had great success cutting slots to the width of the cutter
- quite possibly because both of my machines are small (a Taig and an X3) - in your situation I would probably choose an undersized cutter (say, 1.4") and cut the slot in 2 passes.
Is cutter flexing a known problem in the situation I describe, and would it produce the effect I'm getting?
If this IS a recognised problem, how do others get around it?
Mike
Cutters will always flex due to cutting load, so you should arrange your cuts to be of a size that the amount of flexing is small compared to the tolerances that you are working to. Cutters will also flex more if chips are not being cleared away by a stream of coolant or air.
As Tony says you would do better with a cutter narrower than your finished slot, then clean up. I prefer three passes. One up the middle that can wobble all it likes, then a clean up cut down both edge to finished size. The central wobbly cut can be multi-pass to keep loading down, and the finish cuts can be full depth to avoid the striations.
I can certainly get a good result by the method you suggest. However, being an inquisitive soul, I would still like to understand how the problem comes about. Do the users of bigger, more rigid, machines also have problems cutting clean slots, or is it a fundamental problem with small, and necessarily flexible, cutters? Would different cut depth/feeds/speeds make a difference?
I can certainly get a good result by the method you suggest. However, being an inquisitive soul, I would still like to understand how the problem comes about. Do the users of bigger, more rigid, machines also have problems cutting clean slots, or is it a fundamental problem with small, and necessarily flexible, cutters? Would different cut depth/feeds/speeds make a difference?
Mike
It's a fundamental problem of the vertical milling cutter - you can hold the cutter as ridgidly as you like, but as it cuts it flexes. You can reduce the cut per flute/rev by either slowing down the feed or increasing the rpm - but you need to clear the chips and keep the cutting edges cool. Large commercial mills use a constant and very high flow coolant. I doubt that your Dore Westbury is coolant equipped - a constant blast of compressed air helps but isn't as good.
A horizontal mill is of course far better in this respect, and it is common practise to cut slots with a cutter ground to finished slot width.
It is a common problem which is exacerbated on smaller "lightweight" machines. If you think about it the cutting forces (particularly with a two flute slot drill), acting on the spindle/cutter are acting in the same direction, ie the climb milling forces the cutter away from the surface the conventional cut tends to drag the cutter into the opposite slot surface. So with this much force on the cutter it is more likely to flex and produce the problem you have. If you have a three flute cutter try that it sometimes (although by no way always) helps the finish. Other issues like, long "overhang", can cause spindle/chuck/cutter flex on small machines and is more likely when you use a collet chuck rather than directly mounted spindle collets. Any play in your spindle bearings will also cause the problem even if they are fairly widely spaced; the top one can be the issue here as the lower one acts as a simple pivot. I don't know much about the Dore Westbury but if they are the typical pair of taper rollers then they might need to run slightly tighter. Obviously with the sideways force on the cutter in this instance doubled then any play in the table slides will also show up so make sure the gibs are well adjusted and of course the non moving axis is well locked. Also with the round column machines (like my old RF25) it is fairly easy to get some column flex, if so a change of speed can be a help if the normal speed is too close to the natural frequency of the column.
To be honest most people use the multipass method of slot cutting if you want either two good surfaces or an accurately sized slot. I certainly do on my Bridgeport but then again many would call that a lightweight machine as well. As always a smaller DOC will help, cutting a 1/2" slot on my RF25 with 0.100 DOC would shake the machine considerably.
Good point Andrew, I forgot to mention the "re-cutting chips" issue which is by far the most likely cause of problems cutting full width slots - must be age getting to me.
There was a post on this NG back around the 14th Nov entitled "Metal engineering models" where a collection of videos was mentioned. T save you looking them up there were as follows :
formatting link
formatting link
formatting link
formatting link
formatting link
formatting link
formatting link
formatting link
formatting link
formatting link
formatting link
formatting link
In the 7th video in the first list ("videos/896.flv") at around 12 minutes in the presenter mentions the deflection of the tool due to the cutting forces. He doesn't specifically discuss the effects that you have seen but just suggests keeping the cut small to avoid deflection. It is quite well known that climb milling gives a better finish for small cuts so I think you have just run into an extreme of that common effect. If you can reduce the feed rate it would be interesting to see if the effect disappears as it may be partly due to chatter.
In any case I've found the videos to be interesting and informative so they might be worth your time to look at.
Not really surprising, in fact pretty much predictable. You'll always get some patterning on one side of the cut because the cutting forces are different. You reduce that with rigidity, high speeds, low feeds and smaller depth of cut. In your case you had everything working against you. A small diameter long series cutter which will be very flexible, a small machine, low speed, high feed per tooth and trying to cut to final width with one cutter.
Also when you're climb milling the tooth meets the workpiece at the top of the cut and vice versa for conventional milling. This alters how the cutter pushes away and whether top or bottom of the cut gets more metal removal. That's probably where your sawtooth came from but it might also be partly due to misalignment of the quill and bed. If you altered the cutting depth on the quill that shouldn't have mattered but if you altered it on the knee it might have done.
At 500 rpm and 3000 to 4000 thou per minute you're feeding at between 6 and
8 thou per revolution or 3 to 4 thou per tooth. That's a roughing feed. For finishing you'd want 1 to 2 thou per tooth.
I'd also say you can't ideally cut a smooth slot in several passes of depth with the final sized cutter, especially with a flexible cutter. You need a final cut with a decent amount of metal removal with the whole depth of the slot being machined in one go. In your case the cutter would have been bending towards one side on each pass and when you reached the final depth you'd already have removed more metal somewhere than the final pass cleaned up. If finish is important I always machine a slot by making a smaller one and then cleaning up each side in the same direction of cut. A half-way house to that is make a smaller slot and then clean up in one pass at full depth with a higher speed and lower feed, ideally with a short rigid multi tooth cutter rather than a long series slot drill.
Try making a smaller slot first and then using 1000 rpm and the same or slightly lower feed for a finishing cut at full depth and see how you go. If that still doesn't cure it you'll have to machine each side separately.
A twist drill removes metal a lot faster than a milling cutter and only costs pennies if you break or blunt it. I'd probably have chain drilled at
7mm to get the bulk out, run one fast roughing pass by hand with a smaller milling cutter to make the small slot and then one pass under feed with the finishing cutter. I never peck away at a slot in several passes of different depth with the final size cutter. That's a guaranteed recipe for a poor finish on one side and in fact the wrong final width. It'll always be a bit oversize on the ragged side.
When you've got a rigid machine, rigid cutter and no backlash in the feed you can get away with almost anything. When you have one or more of those issues present you adapt your technique round the problem.
There was a post on this NG back around the 14th Nov entitled "Metal engineering models" where a collection of videos was mentioned. T save you looking them up there were as follows :
formatting link
formatting link
formatting link
formatting link
formatting link
formatting link
formatting link
formatting link
formatting link
formatting link
formatting link
formatting link
In the 7th video in the first list ("videos/896.flv") at around 12 minutes in the presenter mentions the deflection of the tool due to the cutting forces. He doesn't specifically discuss the effects that you have seen but just suggests keeping the cut small to avoid deflection. It is quite well known that climb milling gives a better finish for small cuts so I think you have just run into an extreme of that common effect. If you can reduce the feed rate it would be interesting to see if the effect disappears as it may be partly due to chatter.
In any case I've found the videos to be interesting and informative so they might be worth your time to look at.
PolyTech Forum website is not affiliated with any of the manufacturers or service providers discussed here.
All logos and trade names are the property of their respective owners.