Ramping into slots

[traceflair]

Not a HAAS specific post, but I thought I'd post here since I work mainly on a VF-4. I've been getting the hang of ramping, and I've found an issue which has me curious. Specific slot today was 3/8" wide, 2" long, and 3/8" deep being a through slot.

Since I didn't ramp down to the full depth in one pass, I wondered about the proper way to complete the ramp. The first pass was, say, G1 G91 X2. Z-.04 (pretty shallow ramp, like 1.5 degrees). Now if I ramp down .04" on the X-2. cut back, then my endmill will actually approach a .08" depth of cut as it makes its way back across the slot, correct? Seems like that could run into some tool stress problems with longer ramps.

On the other hand, if I cut back to the beginning without another ramp -- G1 G91 X2. Z-.04; X-2.; -- then I have a lot of wasted run time, I think, by cutting passes that don't ramp down. What's the general practice for slot ramping?

Also, since I found out the hard way today that this practice is a pretty bad choice in 304 stainless, is the traditional slotting practice of drilling a lead hole, roughing, then finishing still necessary in this abomination of a metal?

Thanks for any advice and for all of the helpful information on this forum.

[christinandavid]

One approach you could consider is to use a smaller cutter, say 1/4" to 5/16", and helically mill hole at one end of the slot. Essentially a circular ramp.

Then mill the slot full depth to the other end trochoidally (incrementing circular motions). Your cutter will thank you for it.

DP

[traceflair]

Thanks for the advice. How does helical interpolation work on 304 stainless? Seems like it's still quite a bit of surface time on the bottom of the tool, which is what wore out my carbides (uncoated) when I tried to ramp the slots. Just hard to feel comfortable with the bottom of the tool in contact with the stainless for that length of time.

As for the trachoidal path. I don't have any CAM software, but I did once manually program a loop which did a G3 arc with .015" radial engagement and a .015" stepover to trachoidal mill a different slot in some 304. It was quite quick and impressive, but I did get a chipped flute after a few slots. Though, that was also an uncoated carbide and a first attempt at manually programing the closest thing to trachoidal milling.

I'm quite partial to this approach if I can get it dialed in.

[christinandavid]

I wouldn't think helical ramp or even a pecking cycle would be any more trouble than linear ramp - the advantage you have is that the slot is thru - you can use the bottom part of the cutter for the pilot hole then move down to the fresh part of the cutter for the sideways motion. If you are still getting chipping try less engagement per pass with higher feed rates. Even try running dry versus running with coolant, see if there is a difference in tool wear.

It will be more work programming-wise doing it this way - but it is a good opportunity to see how material/cutter behaves when you alter the conditions.

If it works well and you will be doing a lot of similar work, consider writing a macro program (this, of course, assumes you have the option). The one I wrote uses linear increments and 'oscillates' the feedrate in sync with the cutter engagement. I probably have too much time on my hands...

DP

[traceflair]

I have been dying to do some macro programming, but alas my two HAAS VFs aren't equipped with the option. The sad part is my 1998 Fadal VMC has all sorts of fun options like parametric programming and modal subroutines, but its spindle acts funny over 2k RPM, and I haven't had the time to fix it.

I have quite a few 304 stainless plates to cut numerous slots in tomorrow, so I'll hopefully get it dialed in.