[littleCNCjohn]

I've heard the rule of thumb that I should plunge at my normal feed rate divided by the number of flutes on the end mill. So for a 2 flute cutter, I should plunge at 1/2 the normal feed, for a 4 flute, it would be 1/4. etc. But my question is if the "normal feed rate" is the feed rate that I would use for a 25% radial depth of cut (such that 25% of the end mill's width is used), or for a 100% radial depth of cut (as when slotting)? In other words, if the manufacturer recommends 10 ipm at a certain RPM and 25% cutter width, do I plunge at 10/4 ipm or 10/4/4? Thanks,

John

[109jb]

if you are at a 25% stepover why would you plunge there? Just side cut into it. Plunging is generally considered making a hole. If you can drill a smaller hole first that is preferred. If you are slotting, do a horizontal move with a Z component and the feedrate will be close to a normal side cutting feed rate. If doing a hole or counterbore that is bigger in size than the end mill, use a helical move. This is the same as a circular move, but you add a Z component. If you must plunge then the feed rates you mentioned are good, but depend on the rigidity of the machine. A large VVMC may be able to do it, but a X2 may need a much slower feed rate.

[zero_divide]

Yes if you are engaging less material you can bump up your feed accordingly.
For 2 flute endmills 1/4dia and below I don't even bother ramping.
I just plunge at 1/2 the normal slotting feed.
I don't think you should bother too much about it. Plunge is so fast you will not have time to get scared.

[littleCNCjohn]

Thanks for your replies! I usually do a helix or ramp into the part, but just to be clear - hypothetically if I was slotting I would need to reduce my feed due to having 100% of the mill tool's width engaged (say down to a quarter of the recommended feed for a 25% stepover), and then reduce it further for the number of flutes (half again for a two flute mill), right? Thanks again,
John

[109jb]

Use the speed and feed for whatever you are doing then reduce. For example, milling a full width slot, calculate the feed and speed for milling the slot (ie: full engagement) and reduce to 1/4 to 1/2 of that speed. BTW, plunging at 25% stepover is probably worse than plunging at full engagement. Plunging at anything less than full engagement means that the cutter is in and out of the cut and will buck even harder than if it had full engagement.

Like I said though, for doing a slot, I would start at one end of the slot on top and do a ramp to the bottom of the slot at the other end and then a horizontal move to finish. I find that plunging on less rigid machines produced a hole that is oversize because of the end mill walking around. Because of this a plunge and then slot winds up looking a bit like a keyhole. If your slot tolerance is not too tight this might not be a problem. If it is then use a smaller mill and clean up the sides afterward.

[littleCNCjohn]

Will do! Thanks for your help! Now if I could figure out why my workpiece has started bowing up in the middle (the same toolpaths never caused it before)... clamped on both ends and attached to a shim under it with Mighty Bite wax... Sincerely,
John

[SCzEngrgGroup]

Will do! Thanks for your help! Now if I could figure out why my workpiece has started bowing up in the middle (the same toolpaths never caused it before)... clamped on both ends and attached to a shim under it with Mighty Bite wax... Sincerely,
John

Could just be a function of the material. All metal has internal stresses due to the forming in manufacturing. When you cut away some of the material, the stresses can be relieved, and the material changes shape. With thin material, the only way to avoid this is better holding, such as using a vacuum plate instead of clamps.

Regards,
Ray L.

[littleCNCjohn]

That could be... I notticed that the plates (303 stainless) have changed recently. Now they have less scale and sharper, square edges (before the slitting operation left rounded, beveled edges and residual curvature). The plates are also harder (now ~115 HRB as opposed to ~90 HRB). Thanks again,

John