Let's talk about CAM

Thanks for the info. I'm really glad you posted about this.

what do you mean about avoiding sharp corners?

Let's say you are peeling away metal in 'vertical slices' of one millimeter at a time to make a square pocket. The endmill humms along nicely;a tooth enters the cut and some 40-60 degrees later it exits the cut again.

Now it enters a corner.Suddenly the endmill has to take away a millimeter from both sides of the corner, and load doubles almost instantly. This is a situation that carbide endmills don't like, Especially not in a not-ultra-stiff-homebuild-machine with a spindle that is operating close to it's low maximum torque already.

The same with plunging in the metal; standard endmills are not so good in doing that, and all drilling operations require a lot of torque. A gentle helical or ramped entry into the cut is much easier on the endmill.

Deep cuts peeling away small layers at a time work best with highspeed spindles in metal. It is not cutting speed by itself that dulls endmills, it is the combination of pressure and heat that dulls endmills. By taking small (vertical) layers away you get to the situation that the flutes are in the cut only 15% of the entire revolution and spend 85% of the time in air/coolant. In that small portion of time there is not much heat buildup in the cutting edge and not so much pressure either. This allows you to increase cutting speed, and therefore feed, a LOT. To do this with acceptable removal rates you increase the depth of the cut, which also provides the benefit of using not only the bottom few mm of your endmill but a much larger portion of the cutting length. More chips for the same money.

With an 8mm 4-flute TiAlN coated carbide endmill you can take cuts in regular construction steel of 12mm deep in one pass, 1mm wide, at 9000rpm while feeding at 2100mm/minute using only mist cooling (I use an alcohol mist; that results in completely dry chips. But mind you, while milling steel there is a potential danger since alcohol is flammable and milling steel might produce sparks). After a bucket full of chips the endmill still looks almost new.

Officially this is the territory of CAM-software that can produce constant engagement toolpaths. Unfortunately software like HSMWorks, OneCNC, SolidCAM, etc. is completely unaffordable for us hobbyists. But with some thinking and clever programming it is not hard to force CamBam to do well enough. Split a square pocket in a pocket with severely rounded corners (corner radius much larger than endmill radius) and a few operations to clear the remaining metal, for example.

Great info.
What are your recommendations for something like a pocket that requires a plunge?

What are your recommendations for something like an exhaust manifold flange where your fastest option is a single cutter width pass?
I have been running a lot of numbers this morning to figure out the limits of the machine. If I was cutting a stainless steel flange I would definitely be pushing the machine and with a 1/4" cutter may just barely be able to get it above 3000 RPM and with full radial width and small cuts like a couple mm in depth may be able to get power requirements down to .2kw. It looks like it will all be pretty near the limits.
Or would I be better stepping down to a 3/16 cutter where I can get the RPMs up a good bit more. Upsides are more power and less resistance but the downside is a smaller, weaker and more flexible cutter.
What are your thoughts for a situation like this?
Otherwise for things like pockets instead of taking a full width cut you could just do a plunge then spiral out with something like 20% of the cutter width or something like that. This still has me wondering on best techniques where you will need to plunge.

Most of my work comes from manual machining and in my experience with steel with the right feeds and speeds no lubricant or cooling should be needed. What are others thoughts on this?
It's interesting to hear you are using alcohol. Once concern I have often heard is that of water or coolant actually shocking the cutter and shortening life. At my last job even most of the CNC machining we did on steel we did dry and had very good luck with cutter life and finish. Of course this also greatly depended on the cutters as well. I know there were some brand new carbide cutters I'd throw on the mill and it would cut horribly, get hot and smoke it's self. Throw a good cutter in there and triple the feeds and speeds and it would happily cut dry all day long for weeks.

This topic has gone pretty far off topic but I would love to continue the convo.
Any way a mod can move this part into a new thread more on topic?
Not sure what the topic would be called though.

How to get by when your equipment is too small?
Using small tools in big pockets?

A word of caution upfront: I am just a hobbyist with a Chinese (BF20/G0704) mill who managed to find a set of cutting parameters that the machine likes. I am in no way an expert.

yoshimitsuspeed wrote: Great info.
What are your recommendations for something like a pocket that requires a plunge?

Helical entry with a 2 degrees angle or a ramp-in over almost the entire pocket outer edge if the pocket is large enough.

What are your recommendations for something like an exhaust manifold flange where your fastest option is a single cutter width pass?

I consider the mill as just another tool, not as the 'one solution to solve all problems'. Thus, If I need only one or a few, I would drill the flange bolt circle holes using the mill so you have a reference, use the bandsaw or angle grinder to roughly shape the flange contour, then clean up on the mill using the previously drilled holes to hold the workpiece and align the mill. Cutting off chunks of metal is a lot faster than converting them into chips on the mill anyway and I can prepare flange #2 while #1 is cutting on the mill.
The large inner hole is something I would mill away completely, starting from a hole I drilled before and spiralling outwards. My drill press with it's 3/4hp motor makes a 16mm hole in steel sheet metal a lot quicker than my Chinese 24k rpm spindle does.

Using the bolt circle holes to screw down the flange makes it possible to clamp down the work tightly so it won't vibrate, and you don't need holding tabs.

If I cannot do that (or if am too lazy) and the contour cut is deep, I take small depth steps and mill a contour ~1.4x as wide as the cutter diameter so chips can get away.

But maybe your machine can handle deep slots with endmill diameter just fine. All those machines seem to be happy with different cutting parameters.
My Chinese mill definitely doesn't like plunging and slotting in steel, so I work around it.

I have been running a lot of numbers this morning to figure out the limits of the machine. If I was cutting a stainless steel flange I would definitely be pushing the machine and with a 1/4" cutter may just barely be able to get it above 3000 RPM and with full radial width and small cuts like a couple mm in depth may be able to get power requirements down to .2kw. It looks like it will all be pretty near the limits.

Stainless is one of the materials I am not very happy with. I did a motorcycle brake caliper adapter in 316 stainless for a friend using a 6mm 4-flute TiAlN coated endmill, but it was slow and it did cost me an endmill.

Or would I be better stepping down to a 3/16 cutter where I can get the RPMs up a good bit more. Upsides are more power and less resistance but the downside is a smaller, weaker and more flexible cutter.
What are your thoughts for a situation like this?

I would use the smaller cutter; 3000rpm is borderline on those spindles. They really are made for 6000+ rpm and although they can do lower RPM's (the watercooled ones at least) it is not their strength.
Maybe with a better VFD this changes, I don't know.

Otherwise for things like pockets instead of taking a full width cut you could just do a plunge then spiral out with something like 20% of the cutter width or something like that. This still has me wondering on best techniques where you will need to plunge.

Just spiral in too. CamBam gives you that option in the 'lead in/out' section of the machining operation parameters.
Spiralling out is a good thing. Use 1/10th to 1/6th of the cutter diameter, go full depth, forget the cutting speed you got from that 1950's era book. As a guideline, use 60-70% of the cutting speed the manufacturer provides for low angle of engagement cuts (they are often very agressive, great in production, not so great if you have to pay for the cutters yourself), and increase RPM and feed. Modern coated carbide endmills are definitely way ahead of HSS endmills (although I do like the toughness of HSS/HSSCo8 cutters)

Most of my work comes from manual machining and in my experience with steel with the right feeds and speeds no lubricant or cooling should be needed. What are others thoughts on this?

I do mill steel without cooling or lubrication if I can keep the feedrate up.

It's interesting to hear you are using alcohol. Once concern I have often heard is that of water or coolant actually shocking the cutter and shortening life. At my last job even most of the CNC machining we did on steel we did dry and had very good luck with cutter life and finish. Of course this also greatly depended on the cutters as well.

Alcohol has the tendency to flow into tight spaces much better and quicker than water does, the droplets in the mist are very small, and I like a blast of compressed air to get rid of the chips in the cutting zone anyway so adding a little alcohol is easy.
I do mill steel dry, but the finish pass is often close to 'rubbing away the metal' due to the limited stiffness of my machine. And if you cannot make chips that are thick enough to carry away the heat, you need something else.

I know there were some brand new carbide cutters I'd throw on the mill and it would cut horribly, get hot and smoke it's self. Throw a good cutter in there and triple the feeds and speeds and it would happily cut dry all day long for weeks.

I am done with Ebayed Chinese carbide cutters too. What they use for PCB production is good value for money, but the rest?
They cost only 20% of a decent one, but you need 10 of them to do the same amount of work.

It's been a long time since I visited this thread, and a while since anyone posted anything.

It's a little late to suggest a system but I thought in the event you looked here again it may be helpful to share a
CAD/CAM program that may help.
Go to webersys.com and check out Synergy.

I have enjoyed working with it\ and it's well priced.

Can you give a rough idea of price. I really hate it when companies make you contact them for pricing. I believe I found them at one point and I am pretty sure that's why I ignored them.