[mc-motorsports]

I'm planning to pick up a TiALN coated carbide tool to see if I can get the SFM cranked-up a little higher.

Make sure you get a variable helix, Gorilla mills work good! Variable helix is much better than the TiALN coating. I've used standard 30* helix endmills that were coated, wern't much better than uncoated.

[HuFlungDung]

If possible, I'd recommend a carbide face mill to do the light facing cuts if you are simply cleaning up some of the faces. This is because I think you will get better tool life if you are climb milling, or milling with tools that are of large enough diameter that they do not create a shoulder on the part. Notice that when exiting the cut with a face mill, that to some degree, the machine could be climb milling and could de-stabilize the setup.

Conventional milling rubs the hell out of the corners of the tool whenever the tool forms a shoulder and causes premature tip failure. Carbide is very sensitive to edge wear when conventional milling, and even moreso when using inserts with honed edges. These require a significant chipload to get the insert forming a chip with the face of the insert as rapidly as possible, thus minimizing the amount of time that the honed edge is trying to get under the surface.

For a small mill, probably a 3/4" insert endmill would work better for you than the 1.25" one that you have, and could even be more productive in a slotting situation. This is because you can still get a 3 insert endmill in 3/4" diameter, so you can take as many chips, except that you can now run the smaller tool faster and still obey the 400 SFM rule. And the smaller tool requires less torque to turn, so you can get the feedrate up into a healthier range that increases chip thickness. This will increase the amount of material removal before the edge wears out.

Make sure the axis that you are not using are clamped. Clamp the knee, the Y axis, and the quill when milling in X (longitudinal with table). Some of these older machines may have worn variable speed pulleys and belts that may be worn. A worn out variable speed belt gets narrower, and significantly decreases the effective pressure of the spring loaded pulley. This can result in a failure to transmit sufficient torque to the spindle (and subsequent tool chatter). If the variable speed pulleys seem noisy, an overhaul would be in order. The sliding bushings in a variable speed pulley can and do wear over time, resulting in sloppy fitting (noisy) pulleys, and this may destroy the pulley faces as the pulley faces tilt away from the belt in the pressure zone.

Rough mill dry with carbide. Intermittent coolant is worse than none when roughing because of thermal shock which will quickly cause the edge of the carbide to degenerate. BTW, 3 in 1 oil is not coolant, and the smoke generated by all petroleum oils in the cutting zone would be bad for you to breathe as well.

I cannot emphasize enough that conventional milling is to be avoided with carbide tooling. With a bit of drag created by the table gib clamp, you should be able to take light (.01") finishing cuts about 1/2" deep (Z depth) without the tool grabbing the part out of the vise. This latter phenomena is a real and ever present danger with acme leadscrews, but the tool also pulls the work along, so feeding pressure seems almost nil. That doesn't mean you should allow the feed to become too aggressive. Be particularly viligent when entering or leaving a cut as that is when conditions change the most.

Now you didn't read this here , but you could hang a counterweight from the table to help resist the backlash for light finishing cuts. You'd need to rig up a pulley and cable system for the counterweight so that the force is applied effectively in the proper direction, different rigging for each direction of feed would be required.

Some lead screw mills have an anti-backlash nut on the lead screws. This adjustment can reduce the clearance between the nut and the screw to a small amount and make climb milling a bit less nerve racking. However, the wear of the screw is often greater in the center of travel, so it might be impossible to cope with varying backlash with this method.

However, a lot of table backlash can be due to simple wear / poor fitting between the thrust surfaces at each end of the table screw, where the handwheel collars are fitted. This, you can do something about, by machining thrust surfaces smooth and square and installing shim spacers or washers where required to eliminate looseness. Or better yet, install some sort of antifriction bearings (aka ball thrust bearings) at each end of the table screws, to reduce the table/thrust clearance to near zero.

After this, then the total backlash of the table will be confined to the screw/nut wear. If the nut is extremely worn, it should be replaced, and perhaps the screw also, since the screws do get worn out in the center. However, some guys on these forums have injected various compounds (Moglice) into worn nuts to improve the fit. You'd need to study up to do that.

Near zero backlash is desirable from an accuracy viewpoint on cnc machines, but if you are just hogging material, a few thousandths of backlash (like .003 to .005") should still make climb milling feasible on a lead screw machine table, since the chipload is often that much anyways.

[panz]

Hey guys, sorry to dig up this thread but I wanted to post what worked successfully for me on my machine. I talked with the tech support from Lakeshore Carbide and they clued me in what cutters they offer that would work well for my setup. Right now I'm roughing with a 1/2" 4 flute AlTiN roughing endmill. My speed is 1000 RPM (about 125 SFM), feed around 4-5 IPM, with a DOC of 0.200" and step-over of 0.25". Beyond these settings I start running out of horsepower. I ran with "Universal" synthetic coolant via a spray bottle. I've chewed through around 6 cu. in. of material tonight and the endmill is in great shape. I also picked-up a variable-flute endmill from Lakeshore for finishing. It is surprising what a difference the vari-flute makes in reducing chatter and increasing feed.

[mc-motorsports]

Hey guys, sorry to dig up this thread but I wanted to post what worked successfully for me on my machine. I talked with the tech support from Lakeshore Carbide and they clued me in what cutters they offer that would work well for my setup. Right now I'm roughing with a 1/2" 4 flute AlTiN roughing endmill. My speed is 1000 RPM (about 125 SFM), feed around 4-5 IPM, with a DOC of 0.200" and step-over of 0.25". Beyond these settings I start running out of horsepower. I ran with "Universal" synthetic coolant via a spray bottle. I've chewed through around 6 cu. in. of material tonight and the endmill is in great shape. I also picked-up a variable-flute endmill from Lakeshore for finishing. It is surprising what a difference the vari-flute makes in reducing chatter and increasing feed.

Those are good parameters for a knee mill, but I still vote for more DOC and less step-over. You're not using half of the cutting edge you paid for, your cutters will always wear out at the corner first, so use as much of the cutting edge that you can so you're getting the most chips out of the tool's life. In some cases, you can even increase your feeds and speeds a little.

But like I said, what your doing will work. Good luck!

MC

[Geof]

....Right now I'm roughing with a 1/2" 4 flute AlTiN roughing endmill. My speed is 1000 RPM .....

..... I ran with "Universal" synthetic coolant via a spray bottle..... I've chewed through around 6 cu. in. of material tonight and the endmill is in great shape.......

The end mill will be in great shape because you are going so slow. There is nothing wrong with that but if you are paying more for the cutter than you would pay for an uncoated one you are wasting a bit of money. At that speed and with coolant the coating is not doing anything.

[ryansuperbee]

What's up? Hey I was just reading this post and a half inch bit at 1000 RPM is way too fast!!! He needs to slow that down to 400-500 RPM If he did that he would actually be able to increase feedrate. He is work hardening the material at that RPM. The trick with steel is low RPM and high(er) end feedrate. Hope this helps!

[Geof]

What's up? Hey I was just reading this post and a half inch bit at 1000 RPM is way too fast!!! He needs to slow that down to 400-500 RPM If he did that he would actually be able to increase feedrate. He is work hardening the material at that RPM. The trick with steel is low RPM and high(er) end feedrate. Hope this helps!

I am sorry but you are wrong in more than one way.

The material under discussion is hot rolled steel, low carbon steel, not an alloy steel and it will not work harden.

The surface feet per minute using carbide on hot rolled steel can be anywhere from 300 to 600 depending on the depth of cut, tool engagement and chip load. Normally for roughing the lower end is appropriate with the higher end used for finishing. With coated carbides much higher sfm can be used but this is not applicable to lightweight machines in most cases.

A 1/2" cutter running at 1000 rpm is only doing 130 sfm.

[mc-motorsports]

I am sorry but you are wrong in more than one way.

The material under discussion is hot rolled steel, low carbon steel, not an alloy steel and it will not work harden.

The surface feet per minute using carbide on hot rolled steel can be anywhere from 300 to 600 depending on the depth of cut, tool engagement and chip load. Normally for roughing the lower end is appropriate with the higher end used for finishing. With coated carbides much higher sfm can be used but this is not applicable to lightweight machines in most cases.

A 1/2" cutter running at 1000 rpm is only doing 130 sfm.

Yep, what he said...

Any slower is wasting time. Any faster and you start getting too much flex in the spindle and head and or just run out of HP. Not the best production machines, but very versitile, inexpensive, low operating/repair/maintence costs, and can be quite precision when you know what your doing. The Bridgeport knee mill is not to be under-estimated, but should not be compared to a Mori either.

The only time I have ever had a problem with "work hardening" 1018 or 1020 is tapping smaller holes when you use a dull tap drill to make the hole.

MC

[roundman]

That vise must be bolted down very good or it is not rigid. Rigidity is key for machining. Making sure your quill is locked in the Z axis (up and down) is very important. For your vise do not be afraid to snug the nuts good and you can also add a toe clamp on each side if you wish also.

[handlewanker]

Hi, I thought this thread was laid to rest back in 2009 as the poster must have solved his problem by this time, but for what it's worth, when you have to do significant metal removal in a short time then the choice of machine is more important than the cutters.

Back in the '50's, last century, I worked on a TOS universal mill, that is a horizontal mill with a heavily built vertical head directly attached to the mill body and driven by the horizontal spindle.

With that type of mill the head is a fixed component, rigid as a cadaver in rigour mortis, and does not have a quill for the vertical movement, the knee being the source of Z travel.

Now a vertical head on a horizontal mill is, by comparison, as solid as you can get, there being no overhanging ram to vibrate with a variable angle head and quill assembly like the turret mills of the Bridgeport type have.

The mill I mentioned used to machine flat material with a 10" diam Sandvic Coromant T-Max inserted carbide bit cutter.

So, for the record, if you are contemplating heavy metal removal consider a horizontal mill with a vertical head and keep the Bridgeport types for the lighter tool making type work.
Ian.