just how rigid should a rh33 be?

[poster]

We have a RH33 and it is the only cnc i have ever had experiance with. It seems as though when taking cuts with any indexable tool or using endmills vibration can be felt in the spindle, on the table and all through the chip guards. Is this normal?? Its not a heavy vibration, but if i have something leaning on the chip pan, it will definetaly fall. I haven't seen other machines run, so i am not sure exactly how rigid this thing should be. It is level using a machinist level, (also has little hours so i'm sure gibs are tight) but when the installer levelled the machine he definetly didn't use the procedure outlined in the manual. Is this important? Anyway to test the rigidity to see if something is wrong?

[Brian L]

I had to go look up the model number, that's a monster of a machine... I can't imagine much vibration, but then again, you don't describe the situation very well. What size is the endmill, or indexable cutter? How deep of a cut, into what material, interrupted cut, facing, profiling... what?

There are way too many factors to consider, rigidity of the part, vise, tooling, cutters to be able to give any sort of answer.

[poster]

Well if i use a hydraulic vise with a pc of 1/2" steel flatbar on parrallels, and take a cut with a 1/2" carbide endmill .0625" deep with 50% engagement you'll feel it. Thats running it at 1200rpm and 8ipm. Face mills don't seem to be as much of a problem. If i grab a 1-1/2"ms plate say 6" wide across 2 vises 12" apart, the pc being 24" and take a .100" cut with a 4" face mill with 3" engagment it cuts fine. The vibration is still there but not as bad. I wish i could take a video. Its just I can't make a carbide endmill last or even work right for that matter(lots of chatter), and thinking it may be do to the rigidity of this thing. Like you said its so big, I'm suprised it vibrates at all

[Brian L]

Well, a 1/2" endmill in that thing shouldn't hardly make a noise. That said, with only .0625 DOC, you should be running more like 2500 rpm and .004" to .008" per tooth, you didn't say 2fl or 4fl... so if 2fl more like 20ipm, and this would be climb milling, 4fl would be twice that.

Now the plate, even though it's 1.5" thick, hanging between two vices you might get some chatter in an unsupported area. That's just the nature of the set up.

I would examine a couple things, your tool holders and method of holding the 1/2" endmill... collet, solid holder, hydraulic or shrink fit. Then look at the method of holding the part, how high it's sticking up out of the vise, that sort of thing. Then play with speeds and feeds..... too slow and you will "pound" rather than cut, too fast, you burn up the cutter.... and a slow feedrate is always going to wear and tear your endmills and cutters a whole lot worse that keeping the chip load up where it cuts rather than rubs.

[poster]

we maily use collets for the endmills (Er40s) with those speeds you mentioned i wouldn't get an inch without busting it to pcs. We are suppied with Sowa endmills their book suggests 150SFM for them, what you say is more like 300-350. Maybe these endmills are just crap?? I'll get a couple from Kennemetal and give it a shot. That or somethings wrong here and the vibration kills them. Honestly I'm down to running HSS cause they are the only thing that holds up. Its also frustrating cause were we are theres no one to ask, or watch another machine run to compare. It also seems like the spot were i can get a tool to run half decent, is so small. 5% one way it squeals, and 5% the other way it chatters or breaks.

[Brian L]

I used to own a production shop, granted this was back in the mid 90's that I shut it down.... but if anything, carbide and coatings have gotten better. We used to run 200sfpm with uncoated carbide on mild steel, and if you are using inserts with coating, most could be up in the 350-400 sfpm or more.

You mentioned .0625 depth of cut..... are you running into a "skin" on the steel and chewing up the endmills? I would think a 1/2" endmill would take more like at least .25" depth of cut. Heck, I was running 3/8" depth of cut on a carbide endmill today on my little Parnter 4, a knee mill, a stout one, but still a knee mill.

Go watch some youtube videos and pay attention to the speeds and feeds..... they will open your eyes. Most of the time too slow of rpm and feed is worse/harder on the tool than a lot faster....

[poster]

no problems with the scale. I only ran .0625" deep as i had no chance of going any deeper. I've been looking on youtube, but everyone seems to mill aluminum, or use indexable tools. Not much to see on regular endmills in steel. I have a few things to try next week, and maybe Ill get it figured out.

[Brian L]

Just a quick look turned up a few, here is one in 316 stainless steel:

Trochoidal Milling_Guhring.wmv - YouTube

and one in mild steel:

Hanita milling mild steel 3 - YouTube

[poster]

haha wow, i got some serious issues to figure out

[Brian L]

Yeah... this new trochoidal tool path stuff is pretty amazing. I see them cutting titanium at speeds we would have used on aluminum 25 years ago. I don't know how much of that will translate to you if you don't have the software to program those type of paths..... but still, you should be way above and beyond what you are getting.

With the Vertical Machining centers I used to have (Fadal, Hitachi and Leadwell) we used to kind of go by 1/2 the diameter for depth of cut (this is with endmills down to about 1/2", smaller you have to back off a bit), so a 1/2" endmill would get 1/4" depth of cut. Feed rate should be loading it at least .003" to .005" per tooth, and like I said before, mild steel I would start at 200 sfpm, and go up if I could.

A machine as big as you have there to work with should haul ass and never even whimper until you get something like 2" diameter and bigger in it.

With insert endmills and shell mills, you can go even faster. Most any brand will have books telling you the base speeds and feeds to start with on any given material. They might not be perfect, but it will give you a start.

Oh, and collets really aren't the best thing for endmills, much better off in a end mill holder, heat shrink or hydraulic chuck. I use ER collets for drills and light milling, holding reamers, that sort of thing. You will have better luck with dedicated end mill holder I suspect.