Does climb or conventional milling only apply to edges of the work piece?

[Pcmaker]

Does climb and conventional milling only apply when you're milling at the edge?

What if you're milling straight into the middle of a steel block?

I get very bad chatter/vibration if I climb mill, even in very small width of cuts, hence why I just don't do it.

I'm also getting chatter and vibration when I'm sometimes cutting my endmill right in the middle of a work piece even after messing with the speeds and slow feeding. Using 3/8 carbide mostly on steel with all the axis locked tightly, with the axis I'm using the only one that's not locked. Not sure what I'm doing wrong.

I'll take a video of it later on. I have a PM25mv mill

 

[Cadillac]

It applies to everything not just side milling. One reason for chatter is when cutting a pocket the first cuts are using the sides and bottom of cutter. So the ratio of the cut is overloaded. I usually use the 50% modo. Using a .500 cutter I would only take .250 per pass maximum on a side mill operation. Doing a plunge cut I would raise the table as I’m traversing to easy the plunge. I only climb mill maybe for a finish cut if improves finish.

 

[macardoso]

It doesn't apply to slotting cuts since the pulling/pushing forces on either side of the endmill tend to cancel out (more or less). Be aware however that cuts which have between 50-100% engagement (more than half the cutter diameter, but less than slotting) will still experience lateral forces due to climb or conventional cutting. The lateral forces are highest at 50% engagement and tend to diminish as you approach 0% or 100%.

If you get bad chatter when climb cutting, you might want to look at tightening up your backlash adjustment on your leadscrew. It is happening because your work is being pulled into the cutter.

Also (from a G0704 owner), the PM25MV is not a big machine. If you are trying to slot in steel with a 3/8" endmill, you're really pushing what this machine is comfortable doing.

Couple of tips:

• Use a smaller endmill. I find I can push a 1/4" endmill happily in its operating limits, but don't have enough umph to drive the 3/8" (especially in steel)
• Not sure if manual or cnc (assuming manual), but change your approach to removing material. If you need to hog out a ton of metal, drill it out first, then finish with an endmill.
• The BLDC motor has low torque at low speeds. Use the backgear to get the motor running faster.
• Use roughing endmills whenever possible. Their wavy flutes significantly reduce chatter and required horsepower.
• Use of cutting fluids can aid in minor chatter problems
• Make sure you are feeding hard enough. If your cutter rubs on the work, you will get chatter.

 

[Pcmaker]

• Make sure you are feeding hard enough. If your cutter rubs on the work, you will get chatter.

When I get chatter, I feed much slower. I guess I've been doing the opposite of what I've been supposed to be doing which is feeding even faster

I guess I should start stocking up on 1/4" end mills also

 

[macardoso]

When I get chatter, I feed much slower. I guess I've been doing the opposite of what I've been supposed to be doing which is feeding even faster

Without seeing/hearing the cut it is difficult to tell you 100% what is going on. When you are cutting, you want each tooth of your endmill to form a full chip. If you get dust or little needles, then you're cutting too lightly. The edge of each flute is not as sharp as you think it is. On a microscopic level, the edge is very blunt and you need to give it enough pressure to dig the edge into the material. If you don't, it will rub across the surface without cutting, creating heat, chatter, and tool wear. You may find that pushing a 3/8" cutting this hard will start to stall your spindle.

Also remember that these cutting forces can be on the order of thousands of pounds of force. Sometimes the machine won't be rigid enough for the cut you're trying to take no matter what you try. This is the point when you want to reevaluate your process.

 

[Pcmaker]

Yeah' I've been getting little needles when I'm milling

 

[Mitch Alsup]

When I mill a block of 6061 or mild steel, I arrange the cut such that the cutting edge is going into the surface being cut. This minimizes the bur created by the cutting, and makes post milling edge cleanup easier.

With the cutter turning CW, as seen from above, the side facing the operator is traversed from R->L and the side facing the machine is traversed from L->R. This is a climb cut, Like you I tend to go slow (table movements) and cut slow (slow rotation speed). The slow table speed gives a very nice surface finish, and my cutters tend to last a very long time.

 

[ThinWoodsman]

This is a climb cut, Like you I tend to go slow (table movements) and cut slow (slow rotation speed). The slow table speed gives a very nice surface finish, and my cutters tend to last a very long time.

What sort of RPM are we talking? For a half-inch cutter, are you doing 500 RPM or more like 300?
I prefer cutting slow and feeding slow (J-head BP in backgear), but when I do this with conventional milling I end up chipping cutters. Well, chipping the big cutters and breaking the small (1/4 and less) ones when they catch.

 

[T Bredehoft]

When slotting, use a two flute end mill. Otherwise one flute is cutting across the face, one is cutting into the side at the same time due to flex of the cutter.

 

[macardoso]

Pcmaker mentioned a 3/8" carbide endmill. Lets look at values which "properly" engage the cutter and then lets try to boil that down to something a manual machinist might be able to use.

Since they post good cutting data for their tools, I will use a GARR Tool EDP# 13230 3/8" 4F uncoated carbide endmill used in 1000 series mild steel.
Surface Speed (SFM): 175
Chipload per flute: .0027"
Spindle Speed: ~1800
Slotting cut @ 0.375" depth
Feedrate: ~20in/min
Power required for cut: 2.75HP

Whoa! That's a lot of power needed

Let's reduce those parameters that down and try to get something around 600-700W (using the full capacity of the PM25MV)

Surface Speed (SFM): 80
Chipload per flute: .0015"
Spindle Speed: ~830
Slotting cut @ 0.375" depth
Feedrate: ~5in/min
Power required for cut: 0.70HP

So there is something you can actually do on this machine (this is full slotting in steel, 1xD depth of cut). At 1.5 thou chipload, you'll be getting real chips. I would be concerned that the cutting forces on this cut may be too much for the machine. A smaller tool would save you money on carbide and you can remove just as much material with it. Lower forces too.

So I threw out a lot of numbers, what does it all mean? If you need to make a slot through 2 inches of material, you would dial in around 830 rpm on the spindle and start feeding so that you finish the cut in around 25 seconds. Feed firmly and consistently and listen to the sound. A good cut should sound something like a hiss, no squeaking or screaming. If your machine can't do that with this cutter, try a smaller tool or a roughing endmill.