X3 milling

Edited By GaryM on 03/06/2013 08:45:53

I also have an X3 and would say you were scratching at the surface.

If using a 12mm endmill I would set it centrally over the work and cut the whole width rather than just 3mm and take a bit of a deeper cut 0.75-1.00mm should still be OK. I assume you have got a sharp cutter?

What I tend to use quite a lot is a small flycutter as they are quick and easy to sharpen and you get far more "new edges" out of them than an endmill. At the weekend I reduced the end of this bit of 1/2" square down to the 7/16" that I needed with one cut to each face thats 1/32" or 0.8mm with no problem at all, just a dab of soluable oil applied with a brush.

Speed and feed were what felt right, I find that better than charts and FPM calculations.

J

Edited By JasonB on 03/06/2013 10:42:59

Thanks for the reply Jason. I started this job with a brand new cutter as I think my previous one had been blunted a little on the S50 castings. I'll try your suggestion on some spare metal and see how it goes, I'm usually over-cautious.

I bought the common set of three fly cutters at Harrogate and just the other day sharpened the largest one to the shape 'Bogs' suggests on Mad Modder. Haven't tried it yet though. I also need to get some soluble oil and use it. I tried some non-soluble cutting and tapping oil but it seemed to make matters worse by making the chips stick around the cutter.

Gary

Those are the ones I use most of the time, had them for years. I've added the picture above and that was bone with the middle of the three.

J

GaryM,

While speeds and feeds do not need to be slavishly followed, they can give useful guidance for particular combinations of cutters and materials. Knowledge of cutting speeds in low carbon steel may have saved a few ruined cutters in the recent slitting saw thread on this forum.

As a guide 1hp will allow the removal of 1 cubic inch of low carbon steel per minute. With the figures you mentioned I calculate that you're removing about 0.01 cubic inch per minute. Your mill should be capable of at least an order of magnitude increase on that.

For HSS steel cutters in low carbon steel a rough rule of thumb is 100sfm cutting speed. For a 12mm cutter that gives about 800rpm. So you could go faster, but 500rpm is fine, it's not that critical.

I'll make an assumption that your end mill is four flute, so at 500rpm and 100mm/min you have a load per tooth of 0.05mm, ie, about 2 thou. If the power is available you could probably double the feedrate, but it is perfectly acceptable as is, and is large enough to avoid chatter.

Personally I find that 'dabbing' coolant on is a waste of time; either nothing or flood coolant for me. However, I would agree that soluble oil is the way to go, and is what I use on all my machines. Tapping oil is designed to be 'sticky' so that it adheres to the tap, and holds the chips. Which is opposite of what you want for milling.

I also have one rule for cutting tools:

Never buy cheap cutting tools - they're a waste of money

Oh, and if anybody says that as amateurs we don't need to worry about feeds 'n' speeds my response would be that the metal doesn't know it's being cutting by an amateur on a small machine, so why not at least be aware of the information available.

I hope that helps, or at least provides food for thought.

Regards,

Andrew

It is often a bad idea to be over cautious in feed rate as if the depth of cut per tooth is less than a thou and the cutter is blunt it might just be rubbing not getting into the metal on some individual tooth passes. That generates heat and further bluntens the tooth.

It is also better to only cut on < half the width of a 4 flute endmill. This is so that only one tooth is actually in the metal cutting at a time. A slot drill , 2 teeth, can be used full width. (horizontal milling is a bit different and in the form of a slitting saw it is better to have multiple teeth in contact.)

Edited By Bazyle on 03/06/2013 12:36:18

I like flycutters for the pretty surface finish they leave but unless your mill head is set exactly square to the table the surface will not be as flat as a surface machined using multiple passes with a narrow(er) endmill. Also, I hate the way flycutters throw chips all over the wrokshop! Generally I use a re-ground cranked lathe tool, either HSS or carbide tipped (I know carbide is not ideal for interrupted cuts but they seem to survive quite well in my experience, and it only takes seconds to sharpen them if they do chip). I used one for the backplate for my tool grinding setup (adapter for the mill) and that was 4" x 18" long - a relatively big surface area for my small A2S mill. Took it in one cut each side.

Edited By Chris Heapy on 03/06/2013 12:41:35

Soluble cutting oil for HSS tooling,I put it on with a squeeze bottle, carbide, either flood tjhe work and cutter, or cut dry. Other than cooling and lubricating, the cutting oil is designed to make the hot bits of swafe stick to bare skin long enough to hurt. Ian S C

0.22" is not a lot to remove. I would have used a larger cutter than a 12mm and would have machined the full width of the flat. The standard tool on my SX3 mill is a 25mm carbide end mill. Can't remember the last time I had to replace the tips. Seems to last forever.

Flood coolant is the way to go. Allows heavier and faster cuts. Cooling of the cutter should be constant as repetitive heating and cooling causes heat stress and leads to tip breakdown, especially with carbide.

Look at adding a power feed to the main slide. Seig have them for your mill for $350. Worth the outlay and saves a lot of arm ache.

This is where theory and actual use of the machine in question differ. with 100mm/min feed and a 12mm cutter that would in theory allow a 12mm wide x 12mm deep cut with some to spare. In practice the X3 won't do 15% of that without complaining, 2mm depth would be as deep as I would be happy to go in one pass.

Also for the same given 3/8" bit of steel on the same out of tram mill the larger swing of a flycutter would produce a less concave surface than a smaller dia endmill.

J

Thanks for the comments Andrew, Bazyle, Chris and Ian.

Andrew: I think I am just getting the hang of these tooth load calculations. 2 thou per tooth per rev doesn't sound much does it. It is a four flute end mill. I think I'd struggle to wind the X feed much faster than 1 rpm which is how I got my approximate 100 mm/min. I was going to try a squezee bottle as Ian suggests as I don't have a facility for flood coolant and was hoping not to go down that route as it will entail a lot more mess. The cutters were about £6 each from one of the usual UK suppliers so I don't know if that's cheap or not.

Bazyle: I think it may have been rubbing for some of the early cuts as I started off with about 0.25mm DOC and feeding slower. I was keeping to D/4 for width as various people suggest although when I machined between the flanges on the cast iron cylinder for the S50 I'm making, the cut seemed fine.

Chris: As they are parallels I think the flatness is more important than appearance but I'll try the flycutter sometime soon on some scrap.

Ian: I'll get some soluble soon. I hadn't realised at first that some people apply it with a bottle, I thought it was only useful if you had a coolant pump.

Gary

Thanks for the comment Paul. I'm beginning to get the feeling that I'm pussyfooting around here with tiny cuts. That's why I put X3 in the thread title as the experience of someone who owns the same machine is invaluable. I've seen your pics of your flood system and you're right about the power feed, I hadn't even considered one until now although they are a lot of cash and a bandsaw might be a better choice for saving time.

I'll try some of the suggestions and let you all know how I get on.

Gary

Wot? My assumption was as follows; let's assume that the 1000W quoted for the X3 is at maximum speed, and that power is proportional to speed. So, with a top speed of 1750rpm, a speed of 500rpm gives 285W available. I suggested an order of magnitude increase should be possible, ie, to 0.1 cubic inches per minute. A 12mm cutter full width at 2mm DOC and 100mm/min feed is 0.146 cubic inches per minute. So both are comfortably within the power available, allowing for a few losses in the drive train. As a first approximation the results seem fairly similar to me?

Gary: I think that 2 thou per tooth is perfectly respectable, particularly in steel. I only mentioned it as a common error is to think that going slow to start with is being sensible. As you have already twigged all that happens is the tool rubs, and then cuts, and then rubs. So you end up with chatter, a blunt tool, and a lousy finish. Can I assume that for 1rpm on the handle you mean 1rps, as 1rpm seems awfully slow! In terms of width of cut I normally use less than D/3 or greater than 2D/3. I've never had problems using the full width for cutting. In theory D/2 is to be avoided as it hammers the teeth as they enter a cut.

Interestingly I never run coolant on carbide tooling, except on the CNC mill for steel and aluminium, to get rid of the swarf. Carbide is quite happy running red hot, so let it. It helps with the power and finish too. To some extent the power needed per unit of material removed goes down as the speeds go up, particularly with harder materials. Of course you still need to have the horses available, which most people, including me, don't have. If everything is cutting as it should then most of the heat leaves in the chips; just don't get them on your hands, or worse down the shirt!

Regards,

Andrew

Andrew, sorry for the delay responding, been in the garden all afternoon. Of course you are right about the handle speed it should have been 1 rps, doh! I can't even go back and edit it now.

Comments like "In theory D/2 is to be avoided as it hammers the teeth as they enter a cut." are really useful to newbies. I've not read that in any of the articles, books and forums. I'm not sure I understand why though.

I only have one item of carbide tooling at present and that is a boring bar.

There's a lot more to this lark than meets the eye.

Gary

To throw a further query into the mix, one cut resulted in this:-

I'm sure this will tell most of you quite a lot, but it didn't tell me much apart from something might be wrong.

Gary

Assuming you took your first 3mm cut off the front (towards you) side of the work what direction was the work traveling in?

Oh it also tells me you need a vice.

Edited By JasonB on 03/06/2013 18:52:14

Cutting blanks for my QCTP I had to make slots 0.250" deep by 1" wide in steel. If I recall correctly I used an 11mm slot drill in three passes to start the slot to depth, and then took another three to get ~22m wide and then a final cut at full depth to get the full width. That's essentially the same as Andrew's 2mm deep by 12mm wide cut.

Didn't wreck the cutter or overheat the motor but broke the gears in the head!

That was on my X2 before the recent bearing and bracing modifications.

Neil

Work was travelling right to left (conventional milling). I've been very careful to avoid climb milling until I know better what I'm doing.

I have a vice, it is further along the table. I was using Harold Hall's technique for making a parallel by using two cylinders bolted to the angle plate. Then take a light cut off the top of both cylinders and mount the workpiece on top. I think it is supposed to ensure that the two sides are parallel to a much better accuracy than just mounting in the vice.

Gary

Looking at that machined workpiece... your chips are like dust which means the endmill isn't cutting like it should. Looks like you cut it dry... and the stringy swarf again suggests the cutter isn't cutting cleanly. The finish doesn't look good either (difficult to tell from one photo at one angle), it should be smooth and shiney. Might be too high a speed on the cutter, might be a blunt cutter, might be very 'sticky/gummy' steel. Best to play around with different parameters on a piece of scrap )of this material) to familiarise yourself with what works best for it - they all respond differently.

For your machined parallel - if you turn the piece end over end (180deg flip) it will come out parallel even if the bottom of the vice is not perfectly aligned with the lathe bed.

> Also for the same given 3/8" bit of steel on the same out of tram mill the larger swing of a flycutter would produce a less concave surface than a smaller dia endmill.

Would it?

Imagine the extreme case of having the cutter tilted right over. the endmill would make a smaller furrow than the endmill. As the out of tram gets less, the difference remains in proportion.

I agree with Chtris, that cutter isn't working hard enough. That stringy swarf suggests it's pretty tough steel too.

Neil