Would anyone share what their most common numbers are for a 1/2" roughing endmill with 4 flutes? IPM, Speeds, Ramps etc?
I seem to be struggling a bit with a bit I purchased. I am trying to cut a block of 4140 and its not cutting well.
I suppose I should ask if running this bit & 30ipm .075" DOC and .080" WOC is way to much for this machine and bit? I dont run .500 much and not in this kind of metal.
Rufus, Ive had 4140 that was a bear to cut in the past on manual machines because it had hard spots. Dont know if thats a fluke or what.
What RPM are you running? It does sound like the WOC is alot. Thats a pretty decent cut for any small machine. I know a Tormach 440 would have problems with it. What is messed up about the cut? Chatter? Also, these machines are sensitive to crappy endmills, like most are. The LS endmills are pretty good for the money.
Try going the other way. Run the IPM up and reduce the WOC. Try it at 3000, then at 3500 rpm. Basically, for testing purposes, ignore the recommended SFM at first. Once you have something that is working, increase your depth of cut until youve maxed out.
Hey Turkeyleg, thank you for the reply and you have hit the nail on the head. I think buying cheap bits on Amazon probably doesn’t help but yes I was getting massive screaming from this. I have slowed it down and sped it up and the only thing that helped was to just berry it but this machine cant get there. Right now I am down to about 2600rpm but to me that seems a bit slow. I just didn’t want to burn it up quickly. I started locking the bit up at these feed rates.
This is a pretty big job 3x6x16 chunk of beef and I was trying to get as much as I could get out of this bit but I am losing. I will try and drop down to .040" WOC tomorrow and maybe speed up as you said to see what that leads to but its pushing me into a 5hr milling job.
When you say maxed out what do you mean?
One of the other problems with this milling job is a lot of Helix transitions and I don’t think these end mills like that much.
I get a lot of my end mills from Titan bits. Not terribly expensive and seem to last a little longer than the cheap stuff from Amazon.
Are you by chance familiar with pretty good Indexable Facing mills with 1/2" shank?
Ive never had any luck with small indexable mills. Most likely though, it was because I used them on Bridgeports and they were never very high quality inserts. The high polish, sharp aluminum type APKT inserts gave me the best finishes, which were nothing to brag about, and they didnt last in steel. I havent seen a 1/2" shank indexable mill that had more than one insert, so Im sure its just IPT vs. SFM vs. IPM. You end up having to compromise on one or two of those, every time. When you use a facing mill, you get more inserts, but the deflection leaves a rotten finish.
What I meant by “maxxing” out is that you fiind a hard limit. Whether thats tool life, chatter or horsepower, youll reach a point where you cant increase anything any more.
I know that the Titans of CNC videos are usually clickbait, but they preach “more speed” and “experimentation”, and rightfully so. Im no CNC expert by any means, but Ive run coated carbide tools at way higher SFM’s than the manufacturer typically recommends and gotten good results. The first thing people notice when they use HSM strategies is that more often than not, the chip temperature doesnt climb in a linear fashion. Sometimes it even drops or stays the same.
Im a stupid ass, but i wouldnt hesitate to run the RPM up to 5000 and the IPM to 80, with a .030 WOC to see what happens. Im not saying it will definitely work, im just saying it will give you a baseline at a higher speed that will tell you if there is another way to approach the problem. Hell, i would go even higher if it smooths out a little.
You may also try reversing the cut direction. Climb milling with cheap end mills can cause a bunch of chatter and you may not be able to load it enough to overcome that. Switching to conventional milling may help.
I’ve run a few different steels and stainless on my mill and generally have to go with a smaller step over and crank the rpm and feed up. My build just doesnt seem to be rigid enough to really load up the mills in a full cut.
1 Like
Thanks guys for the input. I will try to flip direction first thing. I have dropped to a 3/8 and it has made a bit of a difference. I have some brand new bits coming tomorrow and may try to jump back to 1/2".
[quote=“TurkeyLeg, post:4, topic:37927”]
i wouldnt hesitate to run the RPM up to 5000 and the IPM to 80, with a .030 WOC to see what happens
[/quote] I will be trying that tomorrow as well when the bits get in.
One question I am boggled by, I am pre-drilling the leads and I am pilot drilling with a 1/4" drill getting great chips then jump to a 7/16. I am running aprox 400-500 rpm at 1-2ipm and I am struggling terribly. If I drop rpm (which I should) to say 300ish I start getting great chips but there is not enough torque and the spindle locks. I jump back up to the 4-500 range and it chatters pretty bad and loose my chip. This is a brand new bit from Mcmaster. Anything I might be missing on this? Seems I have always had issues drilling with this thing.
The lack of torque has been a limiting factor on a few things I’ve made as well. Once I get larger than a 3/8 drill in steel I go to a peck drill cycle @ about 0.050" pecks to break up the load on the spindle and keep it from bogging down in the cut. May have to play with the peck depth to find the sweet spot.
1 Like
Thanks for that. That’s just crazy that drops that far that quick. I was down to .03 and just struggled.
I’ve drilled hundreds of 1/2 inch holes in steel on these machines- I’ve found following the exact parameters in the cut chart published on our website always yields perfect results (quiet cutting, no chatter, etc).
2 Likes
I often drill at higher than suggested (by FSWizard, my normal tool) RPMs with lower feed rates on my MR-1 to get good torque. I’m using a spindle with less low-end torque than the stock one, so I have to do this earlier than you would on a stock MR-1.
Looking at Langmuir’s recommended speeds and feeds for HSS it looks like they are using a similar strategy. Where FSWizard is running about 3-4 thou per revolution of cutting with drills Langmuir’s chart is recommending more like 1 thou – with higher spindle speeds and lower feed rates.
For my most common size holes I always use cobalt (better) or carbide (best) drill bits to get into higher RPM ranges. Haas often has sales on tooling that make 10 packs of cobalt bits pretty reasonable, and there are a handful of sizes that I use a lot of, since most of my work has M4, M5, M6 or 1/4-20 holes and threads.
2 Likes
Thanks Alex. My problem is around 500ish I start to vibrate real bad so I try to get that small chip left behind from the peck before and then slow it down. Its an absolute nightmare. This wouldn’t be such a huge problem except when the motor locks you have to reset everything and then power everything down and then re home the darn machine because the motor will no longer turn on. It literally takes 2hrs to drill 7 holes 1.5" deep with a Cobalt 3/8" bit (brand new) at the exact numbers on their chart or slower and it sucks. This is very frustrating.
Alex what program do you use for yours? Do you run Mach?
Are you attempting to step drill? That’s going to be much harder to do than drilling from blank. The machine will easily drill up to 1/2” holes in steel if you follow the cut chart. I’d recommend drilling one on a scrap piece and taking a video and posting here so we can take a look. If it can’t do that then there’s a problem somewhere. FYI- torque overload when drilling is almost always caused by z alignment and tram error so that’s got to be good when drilling holes.
1 Like
I have to flip this part in a few days and will video it.
Sounds good, what kind of drill are you using? Make sure its nice and sharp.
I fully agree with requiring sharp drills.
I don’t use my general purpose drills on the MR-1 because it’s too hard to keep track of condition if they were used on metal with a hand drill. My MR-1 gets dedicated drill bits that are always run with tested speeds and feeds. If I need an unusual (for me) size then I predrill close to target size and interpolate (bore) the final size with an endmill.
@Rufus My MR-1 is running on LinuxCNC and I replaced the spindle with a CNCDepot FM30F that has a pneumatic drawbar. The conversion to Mach would be similar, but I don’t have any personal experience with Mach. The MR-1 isn’t hard to convert if you are comfortable working with software at that level and I’ve posted threads here with all of the details of my conversion. A few others have since followed with conversions to other platforms as well (Acorn, CNC-PC are two that I remember).
1 Like
Just coming back to this, do you meant that below or above 500rpm you get bad vibrations? That is a very low spindle speed for this machine. What parameters are you using for the drilling operation (spindle speed, feed rate, and peck depth)?
The stock spindle was smooth for me through it’s full speed range. Are your spindle bearings okay? Is the belt properly tensioned?
1 Like
Sorry Alex I had something come up I was having issues with and had to resolve. I will be drilling hopefully tomorrow and will get back to you.
I do know that the bit I was using wasn’t an amazon cheapy and it had never been used but I will definitely check tomorrow. Thanks’ for your input very appreciated !
OK guys I am at the following.
1/2" bit only used a few times very sharp.
4-500@1.5IPM - .020"peck it locks up
600-640 @.75ishIIPM (0 on screen) .010"peck and it works but it takes 2yrs to drill 3 holes 1.3" deep.
I jumped the above up to 680rpm and jumped up to around 1-1.25IPM .010" peck and it locks up then again if I don’t catch it quick enough then the motor no longer turns on and I have to reboot the entire system.
Is this what I should expect?
I will note that in the above posts I did predrill 1/4" bit and then drilled out to .400" at about 500-550rpm with a brand-new bit and I was getting that vibration. If I dropped the RPM to around 350ish that vibration would start to go away but then when it grabbed the chip like expected the motor would lock up with no torque. This is at 025" peck
When it locks up try just power cycling the spindle drive (220V switch). It sounds like your servo spindle motor is going into alarm mode from not keeping up with it’s intended speed – which means it’s being pushed too hard.
0.01" peck seems really small. Pecking is really about chip clearing from the flutes, and the flutes should be able to hold and still clear more depth than that. When you peck does the drill retract and re-enter at high speed? It should only have the low feed rate when it is cutting metal.
I don’t have the original spindle, so I can’t easily test and compare on my own machine.
2 Likes
One more thought: Have you compared this to doing a ramped bore using a 1/4" endmill?
Also, do you have the spindle running off of 220V or 120V? The 120V conversion drops the maximum torque by quite a lot.
2 Likes