[mrquacker]

This is what I am making:



I start off with 1” wide stock, the final side walls are ~0.095” thick. The slot is 1.6” deep. I have tried many different things, from drilling it out; a 5/8” drill only lasts ~100 holes.

https://www.youtube.com/watch?v=CgGnHCmjilg

To milling, plunging, ramping, pre-drilling, and more.

https://www.youtube.com/watch?v=YWMjyAoxOfE
https://www.youtube.com/watch?v=f4fjWbcCGfU

Everything took too long, and kept breaking tools.

What I am doing now that seems to be working very well is plunge roughing with a 3 flute 3/4” carbide endmill, then taking a ramping finish pass with a 3/8” EM to clean it up and get to the final wall thickness. My fogbuster is doing a great job of blowing out all the chips.



I pre-drill the center of the first plunge using a 5/16” drill from an earlier operation and fill it with lube/coolant, then plunge the first hole at 3.2 ipm 3250rpm, and the rest of the “bites” at 6 ipm. This is all done on the low speed pulley on my 770, with the load meter right at the limits of the green zone. Any faster plunge and it goes into yellow/red, or pushes the tool up into the spindle, making each hole shallower than the last. I havent even bothered testing the high speed pulley because I think regardless of the speed, it will just stall the spindle and break the tool.

https://www.youtube.com/watch?v=3G0HUVenbnQ

This works well so far. Including tool changes, and spending ~15 minutes changing belt speed twice. (the pdb gets in the way; this really sucks compared to doing it without the pdb installed)
The entire program takes just around 2 hours to finish, or about 10 minutes per finished part. ~40 minutes of that being the plunge roughing.

Now after running ~100 parts, the ~$100 endmill is starting to wear out and chip on the edges. I need to make a couple hundred more of these. Before I buy another one, I want to ask if this tool from Tormach will work as good?

Center Cut End Mill - 17mm

The tool and toolholder come out to around $150, and inserts are ~$11 each. Assuming they also last ~50 parts per side, and I can rotate them once; then this tool will pay for itself in one run. I will be saving money long term.

At 17mm 0.67” it’s thinner than the 3/4” endmill. I will probably have to take two finish passes with the 3/8” EM, or slow it down a bit and do it in one pass. Anyone else have experience plunge roughing with this tool?

[SCzEngrgGroup]

You're almost certainly killing the drill bits through heat. A FogBuster just doesn't work well for drilling, adn the deeper the hole, the worse it is. Even so, it would help a LOT to do peck drilling, with a full retract, to give the drill a chance to cool off. That alone would probably greatly extend the tool life.

On the 3/4" carbide endmill, your RPM is way to high for the very slow feed. That will generate lots of heat in the tool due to the very low chipload. Plunging is inherently very hard on an endmill, and doing so with out really good cooling and chip clearance makes it very much worse. And, carbide tools really do not like re-cutting chips - it causes rapid deterioration of the cutting edges. Used properly, those things should be lasting you weeks, not hours.

If I were doing those parts, I'd be using HSS tooling, not carbide (it's a lot cheaper, and on these machines will cut just as well, and last just as long). A good HSM toolpath will GREATLY reduce the strain on the tool. For such a simple shape, even hand-coding it would not be that bad - I would take one of two approaches:

1) Do a ramped slotting cut right down the middle, with about a 3 degree ramp, zig-zagging back and forth until you get down about 1/2". Then do very fast spiral cuts, with 1/2" DOC, 0.05" WOC. You should be able to do these spiral cuts at rapid speeds (100IPM at least) at 5-6K RPM. If you run out of power, back off on WOC, not DOC. Leave about 0.02" for finishing. Then step down another 1/2", and repeat. This would eliminate the drilling, and get the whole job down in a fraction of the time, with very low stress on the machine and the tool. Or...

2) Do a helical entry, again going down about 1/2", then do trochoidal passes to open up the pocket, at 1/2" DOC, ,0.05" WOC. This will also be very fast, but much harder to program by hand, and probably slower than #1, due to the slow-ish rapids.

I would also use a 1/2" endmill, rather than 3/8". A 3/8" tool is awfully flexible.

Using either of the above methods, I would expect each pocket to take on the order of 3-4 minutes.

What are you using for CAM?

Regards,
Ray L.

[mrquacker]

You're almost certainly killing the drill bits through heat. A FogBuster just doesn't work well for drilling, adn the deeper the hole, the worse it is. Even so, it would help a LOT to do peck drilling, with a full retract, to give the drill a chance to cool off. That alone would probably greatly extend the tool life.

Been there done that. Still only around 100 holes per drill. 5/8" dia, 1100rpm, 10ipm.

Then do very fast spiral cuts, with 1/2" DOC, 0.05" WOC. You should be able to do these spiral cuts at rapid speeds (100IPM at least) at 5-6K RPM.

That recipe would stall my spindle and snap the $50 endmill in seconds. Or cause it to pullout, then snap.

I knew this post would be distracting because I included all the info of what I've already tried... I've been making this part for a couple years now.

I'm not asking how you would do it, or how you think I should do it. I've already tried everything Sprutcam7 will let me try on this, and I'm not happy with any of it.

I finally found something that works for me, now all I'm asking if this tool will work for plunging.
Center Cut End Mill - 17mm
The same or better as what I am doing now :

https://www.youtube.com/watch?v=3G0HUVenbnQ

The fogbuster is doing a very good job of blowing out the chips that are made by the plunging. You can see them fly out of the slot in the above video. The tool itself is not even warm to the touch when it's done, while the flying chips burn skin. If anything is getting recut, it's by the flutes higher up the body, not at the bottom. Parts of the tool I don't care about, because I will never use anyways. I'm paying for 1.5" worth of flutes, and only using the bottom 1/8". Partly why I think going indexable will be better.

Using either of the above methods, I would expect each pocket to take on the order of 3-4 minutes.

At 40 minutes for 12 parts, I'm already there.

[popspipes]

I would have the 100 dollar endmill resharpened, that is much cheaper than a new one.


Maybe up the coolant in the fogbuster to see if it helps, the tool can be cool but the actual cutting edge can get really hot, then the shock of the cold coolant may cause the chipping??


If thats the insert mill that screws onto an arbor I would be a bit leary of that one as the screw joint wont be as rigid as a solid shank model.

I would call Tormach on the plunge capability.

[SCzEngrgGroup]

"Been there done that. Still only around 100 holes per drill. 5/8" dia, 1100rpm, 10ipm." - Well, something ain't right there. I've got drills that are 10 years old, have done many hundreds of holes, and still cut fine, even little tiny ones. A good drill is pretty hard to kill.

"That recipe would stall my spindle and snap the $50 endmill in seconds. Or cause it to pullout, then snap." - I can see how it might seem that way, buy I do those cuts all day long, well over 100 IPM, and up to an inch deep, and I can use the same $12 1/2" HSS endmill for weeks, and hundreds of parts. A $100 carbide should last almost forever. A light radial cut at high speed has the same chipload as a wide cut at far lower speed, due too chip tinning, but it is far easier on the tool and the machine.

Pullout is a function of drawbar tension, so I can't speak to how your machine behaves in that respect. I've used TTS exclusively for many years, and I've never, ever had pullout. Not even once, even doing cuts more aggressive than what I suggested. And the only time I break an endmill is when I do something stupid. Can't even remember the last time I broke, or even chipped, one doing HSM toolpaths.

Best to ask Tormach about how to get best results with their insert endmill. But, in general, many/most insert endmills don't much like doing plunges, center-cutting or not. They much prefer a ramp or helical entry to give the chips a better exit path. It should give you comparable result at a lower cost than the solid carbide. Even if the inserts wear out faster, you can replace them 4-5 times for the cost of one of those $100 carbide tools. HSS tooling would probably be cheaper still, even if they wear out a bit faster, which they shouldn't if used properly, as each one would likely cost only a little more than a single insert.

Regards,
Ray L.

[treyjugson]

Hang in there quacker, a Tomacheer will shed some light to help with your machine.

[Steve Seebold]

This is what I am making:



I start off with 1” wide stock, the final side walls are ~0.095” thick. The slot is 1.6” deep. I have tried many different things, from drilling it out; a 5/8” drill only lasts ~100 holes.

https://www.youtube.com/watch?v=CgGnHCmjilg

To milling, plunging, ramping, pre-drilling, and more.

https://www.youtube.com/watch?v=YWMjyAoxOfE
https://www.youtube.com/watch?v=f4fjWbcCGfU

Everything took too long, and kept breaking tools.

What I am doing now that seems to be working very well is plunge roughing with a 3 flute 3/4” carbide endmill, then taking a ramping finish pass with a 3/8” EM to clean it up and get to the final wall thickness. My fogbuster is doing a great job of blowing out all the chips.



I pre-drill the center of the first plunge using a 5/16” drill from an earlier operation and fill it with lube/coolant, then plunge the first hole at 3.2 ipm 3250rpm, and the rest of the “bites” at 6 ipm. This is all done on the low speed pulley on my 770, with the load meter right at the limits of the green zone. Any faster plunge and it goes into yellow/red, or pushes the tool up into the spindle, making each hole shallower than the last. I havent even bothered testing the high speed pulley because I think regardless of the speed, it will just stall the spindle and break the tool.

https://www.youtube.com/watch?v=3G0HUVenbnQ

This works well so far. Including tool changes, and spending ~15 minutes changing belt speed twice. (the pdb gets in the way; this really sucks compared to doing it without the pdb installed)
The entire program takes just around 2 hours to finish, or about 10 minutes per finished part. ~40 minutes of that being the plunge roughing.

Now after running ~100 parts, the ~$100 endmill is starting to wear out and chip on the edges. I need to make a couple hundred more of these. Before I buy another one, I want to ask if this tool from Tormach will work as good?

Center Cut End Mill - 17mm

The tool and toolholder come out to around $150, and inserts are ~$11 each. Assuming they also last ~50 parts per side, and I can rotate them once; then this tool will pay for itself in one run. I will be saving money long term.

At 17mm 0.67” it’s thinner than the 3/4” endmill. I will probably have to take two finish passes with the 3/8” EM, or slow it down a bit and do it in one pass. Anyone else have experience plunge roughing with this tool?

I do a lot of jobs on my 1100, and I will plunge ruff when ever I can. The first thing I do when I plunge ruff is to DRILL out most of the material using a screw machine length drill (the biggest one I can get in there. Then I'll plunge ruff the the rest of it leaving .015 to .025 on the floor and walls for finish. Then I'll do a semi finish pass leaving .005, then the finish pass with 2 spring passed. I ALWAYS have excellent results with this method.

BTW, IMHO when you conventional mill like in your video, you're not actually cutting material, you're just pushing it out of the way.

[pickled]

FYI that 17 mm insert mill isn't the best for plunging into materials. It can be used like a normal center cutting EM, but it is hardly made to be purposed for a life of plunging. It works very well for roughing and ramping, but bogs down quite a bit in the plunge (even at low feed rates) and chip welding hits quick. If you were to first start your roughing path out with punching at least an equivalent 90% diameter hole with another tool first then you could start a ramp with the 17 mm and do well. FYI I don't buy replacement inserts from Tormach anymore. If you plan on actually going through a number of them just search around. I recently bought 10 Mitsubishi inserts for $62 delivered to my door.

[Steve Seebold]

This is what I am making:



I start off with 1” wide stock, the final side walls are ~0.095” thick. The slot is 1.6” deep. I have tried many different things, from drilling it out; a 5/8” drill only lasts ~100 holes.

https://www.youtube.com/watch?v=CgGnHCmjilg

To milling, plunging, ramping, pre-drilling, and more.

https://www.youtube.com/watch?v=YWMjyAoxOfE
https://www.youtube.com/watch?v=f4fjWbcCGfU

Everything took too long, and kept breaking tools.

What I am doing now that seems to be working very well is plunge roughing with a 3 flute 3/4” carbide endmill, then taking a ramping finish pass with a 3/8” EM to clean it up and get to the final wall thickness. My fogbuster is doing a great job of blowing out all the chips.



I pre-drill the center of the first plunge using a 5/16” drill from an earlier operation and fill it with lube/coolant, then plunge the first hole at 3.2 ipm 3250rpm, and the rest of the “bites” at 6 ipm. This is all done on the low speed pulley on my 770, with the load meter right at the limits of the green zone. Any faster plunge and it goes into yellow/red, or pushes the tool up into the spindle, making each hole shallower than the last. I havent even bothered testing the high speed pulley because I think regardless of the speed, it will just stall the spindle and break the tool.

https://www.youtube.com/watch?v=3G0HUVenbnQ

This works well so far. Including tool changes, and spending ~15 minutes changing belt speed twice. (the pdb gets in the way; this really sucks compared to doing it without the pdb installed)
The entire program takes just around 2 hours to finish, or about 10 minutes per finished part. ~40 minutes of that being the plunge roughing.

Now after running ~100 parts, the ~$100 endmill is starting to wear out and chip on the edges. I need to make a couple hundred more of these. Before I buy another one, I want to ask if this tool from Tormach will work as good?

Center Cut End Mill - 17mm

The tool and toolholder come out to around $150, and inserts are ~$11 each. Assuming they also last ~50 parts per side, and I can rotate them once; then this tool will pay for itself in one run. I will be saving money long term.

At 17mm 0.67” it’s thinner than the 3/4” endmill. I will probably have to take two finish passes with the 3/8” EM, or slow it down a bit and do it in one pass. Anyone else have experience plunge roughing with this tool?

Part if the reason your cutter is beginning to wear out could be that your Fog Buster coolant system doesn't have enough air pressure to blow chips away and recutting chips as you get deeper into your parts. Dn't get me wrong, the Fog Buster is a great tool. I have been using them since about 2004. I have a dual nozzle Fog Buster on my PCNC 1100 and I love it, but when I do deep pockets like you are doing, I will use flood coolant and stay at the machine to blow chips out. I have never had success pocketing with the Fog Buster.

Parts for the Fog Buster are easy to get though. Fog Buster is made less than 3 miles from my shop.