End Mill Jamming in Aluminum during CNC milling Attempts 2

[DominicASP]

I just bought a Chinese 3040 230W engraving CNC machine and have recently been struggling with milling operations on aluminium as you can see on my previous forum posts. I am trying to cut through a 4.3 mm thick aluminium box with a TiN coated carbide 2 flutes 42degree end mill with the following specs:
[ul]
[li]Mill Diameter: 3/32" (2.38 mm)[/li]
[li]Shank Diameter: 1/8" (3.175 mm)[/li]
[li]Length of Cut: 1/4" (6.35 mm)[/li]
[/ul]

I am trying to cut a profile through the entire thickness of the box. To generate my gcode, I used CamBam with the following parameters:
[ul]
[li]Depth Increments: 0.5mm[/li]
[li]Target Depth: -4.5mm[/li]
[li]Cut Feedrate: 125 mm/min[/li]
[li]Plunge Feedrate: 62 mm/min[/li]
[li]Spindle Speed: 6000 rpm[/li]
[li]Tool Diameter: 2.38 mm[/li]
[li]Inside Profile Cut (Rectangular Shape)[/li]
[/ul]

I have been trying 4 times to complete the operation but every single time, at some point, I would start hearing a really harsh noise and could see that my spindle speed was gradually slowing down or even see my end mill completely jam in the aluminium. When it happened, I always tried to shut down my controller as fast as I could to prevent further damage to my machine but during my last trial, the fuse blew and had to replace it. I use WD-40 as a lubricant and compressed air to blow the chips away.

Since I was able to cut through softer 1.25 mm thick aluminum plates with the same machine, end mill and parameters, I am wondering what is causing my problems. At a first glace, do my parameters look good? Is my machine powerful enough to complete such operation? Any hints/tips would be greatly appreciated! Thanks a lot!

 

[JNieman]

Is this the machine:

http://www.alibaba.com/product-detail/Mini-Wood-Router-China-CNC-Machine_1257750803.html

?

Off the cuff math shows your feed per tooth is .0004" / .01mm

That's super low for any machine. Couple that with what is likely a rather not-rigid spindle, a tool that probably is experiencing significant runout, and a motor that isn't even advertised to cut metals... you might be rubbing more than you're cutting.

Slow your spindle speed a bit. Half it, even. See what happens. With a machine like that, there's too much going on to go "by the book" with suggestions, so the solution is basically to make intelligent experiments and see what happens. Without seeing the thing in action, I can't really say exactly what it is that's going wrong.

With metal cutting you CAN be TOO gentle.

_________________________________________
NX8.0, Solidworks 2014, AutoCAD, Enovia V5

 

[berkshire]

DominicASP
Buy yourself a mister system to blow a mixture of air and emulsified wax onto the cutter it will serve two purposes.
It will cool the tool and blow the chips away preventing this kind of cutter jam . Squirting with WD40 and using an air hose is not consistent enough to ensure the tool does not over heat.
B.E.

You are judged not by what you know, but by what you can do.

 

[imcjoek]

My experience with these little hobby-duty machines:
Effect of coolants and lubes on tooling is negligible. The damn things don't have the horsepower to really heat up the tool.
That said, a bit of kerosene or tap magic type stuff can help prevent galling in gummy-bear aluminum, but frankly if the setup is such that it crashes cutting dry, it's gonna crash lubed too.

In these little machines, crashes and jams occur 90% of the time due to lack of rigidity, poor work holding setup, or poor tool holding setup. IE: Something moved.

Do you absolutely require that tiny endmill? Can you get away with a larger diameter? 1/8"?
Make sure you are conventional milling: NOT climb milling.
Does your jam occur only as the cut gets deeper? Or will it occur on the first pass? If it only occurs deeper, can you widen out your pocket to allow some chip-space?
How well is the work held down?
Do the slides allow significant lash/wiggle?

 

[DominicASP]

Concerning the machine, it is indeed the

http://www.alibaba.com/product-detail/Mini-Wood-Router-China-CNC-Machine_1257750803.html.

So I tried another milling operation with 4500 rpm. The damn thing stop and the fuse blew after about 3 seconds.
During my first two attempts, I did get pretty far, at about 4-5 cuts deep and then it started having a really rough time and I manually stopped the machine. Problems occurred for my last two attempts during the first cut layer after less than 10 seconds and both time, the fuse blew. Frustration is rising as I have to go buy extra fuses and continue to work with the machine. Could the controller be in cause?

The work piece is held down using a low profile drill press vise attached with screw to the working surface of the router. The whole setup looks pretty solid.

The machine is advertised as suitable for soft metal like aluminum, copper and silver but is 230W enough for the type of milling operation I'm looking to accomplish?

I have to say that for the 1.25 mm thick aluminium plates, I enjoyed better results while milling directly through the plate, i.e. using only 1 pass.

 

[imcjoek]

The machine is advertised as suitable for soft metal like aluminum, copper and silver but is 230W enough for the type of milling operation I'm looking to accomplish?

As a point of reference, I've done a lot of work with a Sherline mill/lathe combo. I have a 1/4hp (186W) DC brushed motor with a 3:1 belt reduction. It will happily swing a 1/2" endmill or small boring head and will cut steel.
It sounds like the 230W rating on your spindle is... optimistic. Or the stepper just doesn't have the right torque curve & gearing for the job.

Usually I see small endmills like 3/32" run at high RPMs. Like 10,000+.

Make sure the endmill is not pulling itself out of the collet. The spiral exerts a downward pull and these small machines don't do a good job of holding onto the tool. It'll drive itself right into the work and jam up.

Are you pilot drilling the corners of your pockets or trying to plunge cut? I recommend against the latter.

 

[JNieman]

It's advertised as being able to /engrave/ metals.

The only other capability claim I see is: "Large 3D engraving in soft wood,MDF board,native wood,PVC,Acrylic we suggest use one or two spiral flute ball bits." in which metal makes no appearance. What you are doing is much more demanding than standard engraving or even "3d engraving".

What is your drill press vice? Typically a drill press vice is rather sloppy, if it's marketed/sold as a "drill press vice" and not a machinist vice (even then, some of those suck)

You likely WOULD have better results doing the 1.25mm or even 4.00mm metal in one pass. Your current cutting strategy uses the most vulnerable part of the end mill whereas using the sides of the flutes instead of the tips would be much safer. You also end up with much better chip evacuation.

_________________________________________
NX8.0, Solidworks 2014, AutoCAD, Enovia V5

 

[Ebug]

DominicASP
Almost every prefabbed aluminum box I have had the pleasure of machining is made of really soft material. Soft equates to gummy. I was not able to tell from your post but is the tool getting gummed up with aluminum? If yes...try switching to a non Tin coated tool. Tin coated tools typically have problems with chip welding in aluminum. It is really a problem in soft aluminum.

While it has been many years since I have machined a soft aluminum project I seem to remember having success with peck plunging through and taking the whole depth in one cut. Pre-drilling an entry hole will eliminate any problems you might incur with peck plunging. WD40 is good. Another alternative is Automatic Transmission fluid. I have even heard of using isopropyl alcohol, but that sounds dangerous.

Like suggested above, move to a larger end mill if possible and make a finish pass with the smaller end mill using the sides of the flutes to achieve a really tight corner radius if required.

Really soft aluminum is a bear to machine. When you get done you will vow to never do it again.

You might check in over at cnczone.com. That is a very good forum with many users with the exact equipment you have. I am sure someone over there has recent hands on experience with what you are doing.

I wish you much luck my friend.

Rob

 

[ornerynorsk]

6000 rpm is very slow for a 3/32 carbide endmill in aluminum. If you are limited to 6000 rpm, slow down your feedrate (seriously!

What grade of aluminum are you cutting? Liquid coolant application at the point of cutting is absolutely critical in aluminum. Plunging causes most heating and chip-welding problems, in my experience. Ramp the plunge if you have room to do it, feeding in the x or y at a ratio of about 10:1 per z depth. Manufacturers like to boast about the end cutting ability of end mills, when in reality, end mills perform very poorly plunge cutting in very soft materials.

Good luck!



It is better to have enough ideas for some of them to be wrong, than to be always right by having no ideas at all.

 

[JNieman]

Slowing your feed rate with a current chip load of .0004" is going to exacerbate issues, imo. I believe the result of slower feed with that RPM is going to be a new 6061-aluminum-coated end mill.

One thing you didn't mention, DominicASP, is how much tool is hanging out of the toolholder/collet ? If your total DOC is 5mm, hang that tool out 5.5mm and cut the path in one pass, full depth. Ramp or helix into the cuts if your software allows for it (or write it by hand) or simply drill (with an actual drill) corner relief holes as someone mentioned before, then feed down there and side-cut the connecting geometry.

_________________________________________
NX8.0, Solidworks 2014, AutoCAD, Enovia V5

 

[DominicASP]

So here how it looks like:

There is 17.5mm between the end of the tool and the toolholder.

I have noticed when my end mill was totally jammed inside my workpiece that it was no longer tight and fixed inside the collet. I could lift my Z axis and the end mill would not follow.

 

[ornerynorsk]

Feedrate is relative to the robustness of the cutting tool and the setup, neither of which are optimal in this case. 0.0004 is a healthy enough bite for a 3/32 endmill. The real issue is lubrication/coolant, and what alloy it is. Also, 17.5 mm is excessive tool protrusion on that small of an endmill, unless absolutely necessary to perform the cut. I've been in the shop for about 35 years, and the first thing that one figures out is that all of the speeds and feeds that the tooling manufacturers provide are highly optimistic, and may work only under the absolutely ideal conditions, which the OP does not have.

JNieman is correct in that you should take full depth of cut if you are able to side mill through the sheet. Far less heat will be generated, and you then have room for your chips to evacuate.

It is better to have enough ideas for some of them to be wrong, than to be always right by having no ideas at all.

 

[JNieman]

Fair point - I may be aggressive in my assessment of the chip load, but before seeing that photo, I'd have still encouraged a more aggressive rate.

However, now that I see you're hanging that tool so far out (think in terms of length-to-diameter ratio) you need to suck that thing back up in the collet. If you're going to cut full depth, your chips can evacuate down, so you can have that tool holder running with minimal clearance over the plate and be fine (probably). Less tool protrusion, more rigidity. You don't have much rigidity to start with so take it wherever you can.

If the tool is pulling out, your collet isn't holding it too well, or your tool is really bound in the part and your motor is just strong enough to let the tool pull out. Do you have any other means of holding tools aside from that ER-looking collet?



_________________________________________
NX8.0, Solidworks 2014, AutoCAD, Enovia V5

 

[sbkenn]

How big is your wprk ? Is the tool lifting the plate rather than slipping down in the collet ? A friend used to have a lot of trouble, even with a vacuum bed, with the work lifting.

 

[GClegg]

Hi Dominic
You have got an engraving machine with a low RPM motor

If you consider 200 m/min for Ali the calculations show you should be running 26,600 RPM

Switch to HSS 8% cobalt uncoated
carbide is not required

 

[silveringchap]

Have you tried TiCn slot drill instead? Try using parrafin too.

 

[dicer]

If the material is gumming up the flutes going faster does no good. You will need some coolant, even cutting oil is better than nothing. I started machining in the late 60's, believe me there are sometimes when you have to cut aluminum like it is Inconel or 321 stainless, it depends on the set up and the material and design, and the cutter, as well as the machine there are times when you can't set feeds and speeds to the book. You do what it takes to get the job done.