Material removal, pondering

I just ran a quick one-shot job off the 1100.
A dozen CRS (1020 ?) steel blocks. needed a slot taken across them in the middle. Blocks were 3" long, 1-1/2 wide and about 1" thick. The slot was across the 1-1/2 axis, 1-3/8 wide and .400 deep.
3/8 dia 4fl coated endmill, 1.25 sticking out. (what I had available, pretty much new)

Now normally I run aluminum and stainless (300 & 400 series) so it's one end of the spectrum and the other. These steel parts were an oddity so I played with Gwizard and come up with .050" DOC, 3000RPM and 5ipm feed
On the machine I ended up bringing the rpm down to 2200 and the feed to 3.6 :confused: to get a decent sounding cut. Now the first path through was full slot width and each one after was .260 width so I could have stepped it up but I just ran the pieces off.

Cycle time ended up somewhere near 18 minutes per.

Anyway, parts are done and gone and it's no big deal, just seems pretty excessive but was curious how others would have approached this
M

Depending on the finish required, I would have grabbed a 1/2 inch cobalt finishing rougher, 0.400 DOC, 2 IPM, 0.240 stepover, about 700 RPM, mist coolant with excess air to blow the chips out.

Take a look at NYCCNC's video about cutting 4140 and optimizing. My go-to starting point with CRS is 1/4" carbide 4flute with a corner radius, 1800 rpm, 6-7 ipm, 0.07 woc, and .2-.3 or more doc. You were initially slotting, so that needs some adjustment. My overall take on the video is go deeper but narrow rather than wider and shallow, and keep speed and rpm in the ballpark of 300 rpm per ipm (in steel). That has worked for me. Either speed range seems to work OK.

Saunders was doing about .25 doc, 3500 rpm, and around 0.1-.2 woc at roughly 15 ipm. NOT slotting.

https://www.youtube.com/watch?v=7kkx6JFUDFI

If I did the math right, that'd bee 14 full depth passes (1 inch/0.07 per pass) at about 15 sec/pass at full depth, or about 4 minutes, vs 4 passes (1"/.260)x 8 (.4/.05) or 32 passes at 30 sec per, which is 16 minutes. Plus the initial slotting pass in both cases. Math seems to match your actual within reason, so it may be right.

For what it's worth.

I was actually trying to get my mastercam to deal with the trochoidal or HS looping path for this slot as I programmed it but it kept creating this weird D shaped path so after playing for a few minutes I just went ahead with a zig-zag regular path to get the parts done.
I'll have to experiment more and see but I get the feeling that my old X2 version was before they really started with the HS paths.
Thanks
M

Quote:

---

Originally Posted by Mooser

I was actually trying to get my mastercam to deal with the trochoidal or HS looping path for this slot as I programmed it but it kept creating this weird D shaped path so after playing for a few minutes I just went ahead with a zig-zag regular path to get the parts done.
I'll have to experiment more and see but I get the feeling that my old X2 version was before they really started with the HS paths.
Thanks
M

---

Trochoidal paths ARE D-shaped, cutting on the curved side, doing a straight rapid back to the start of the next pass...

Regards,
Ray L.

Yes, guess I should have worded that better.
It kept trying to do it in the middle of the slot outwards, my problem but I usually struggle with open-ended slots in MC and ended up creating a closed slot, which is why I'm guessing it was trying to work from the center out. I keep meaning to figure out how to do open slots properly but then forget about it until it pops up again...
M

i like using varimills and run them at the suggested speeds and feeds. i would use 1/2 4 flute with champer corners. about 3800 rpm and feed of 38 ipm, about .3-.4 doc... works well. then i would use a new varimill for finish...

Mooser,
Your chipload seems too light. 3000rpm, 4flute, 5ipm works out to .0004 ipt.
I would slot with HSM paths at full depth, but getting that right takes a lot more work, and when you have to get the job done now isn't the time to figure it out.

For a slot that wide, just use an HSM/adaptive roughing path with a smaller cutter.

1/4" 4fl carbide (short flute: 1/2" LOC), 3600 RPM, 80 IPM, 0.012 WOC, 0.4 DOC (230 SFM, 0.0013 chip)

Should do your slot in about 3 min. I just ran the same path last night with my 770 on Titanium, Stainless, and Zirconium so it should work for 1020 no prob. Probably even kick up the SFM another 100+. I also let the cutter run in both directions so there's no D-shaped paths, the cutter stays in the cut the whole time.

--Bryan

Bryan,
Look at your numbers again. 3600rpm, 80IPM 4fl results in .0055ipt. Chip thinning with a .250dia and .012WOC results in a chip thickness of .0025
To get a chip thickness of .0013 you need .003ipt. Feedrate of 43.2ipm at 3600rpm

BTW, Great job on your FS calculator. I use it regularly.

IMT - Thanks! Glad it is helpful, I've been using it almost exclusively for a couple years.

I'm quoting numbers from a different version of the calculator, it's got new equations for HSM. Since you point it out, I'll check the math and see if I mucked something up! ;-) It uses a scale factor for chipload, as well as an equation for average-chip thickness (instead of initial chip-thickness) which works better for the extremes of the scale that you run into using HSM. The average chip thickness gives you a thinner chip under most conditions, so the calculator offers a higher feed rate, which translates into higher MRR.

Some of Widia's recommendations are quite clever, though I haven't decided to fully switch over to their model yet. Their model is nice because it works for any material if you know its hardness, no need for the magic "power constant" used by the classic model.

--Bryan

OK So now I'm curious and I'll have to try

I've got a little bracket piece to make (2 pieces) that is also 1020, looks like half circle with two flanges, where each would go together with a bolt through each flange and clamp around a 1" dia pipe
Going to contour around the outside, total depth is .7"
Material in a vise sticking out .750, holding onto .625 in the vise (material I have in hand)
I've got the same .375 4fl carbide endmill, tialn coated

Loaded HSMexpress for solidworks since I didn't have much luck with MC

Plugged in a bunch of stuff and came up with .250 DOC, 4000 RPM and 20ipm stepping over .05 each path, climb milling

With the given 3/8 EM, what would you think the WOC should be? I'm thinking I'd like to see something closer to .01, maybe with a DOC closer to .4 (two steps) or even full?

Input?

So it more or less actually worked :)
Adaptive clearing .700 DOC, .025 WOC, 4500 RPM, 20ipm (tried 30 and ended up bringing the feed override down to 65% where it sounded like a happy cut)

Finish pass contour .700 DOC, 010 WOC 4500 RPM 13 IPM with 1 spring pass leaving a nice finish and no chatter even on the inside corners (.200 Rad with the .1875 rad cutter)

I'm fairly impressed with how that worked, not very aggressive and I'll have to check my "old" way to compare times.

Now to look at open ended slots....

M