LinkBack URL
About LinkBacks
Why don't you look at the code? You are running at F250.
You may also have poor chip clearing technique.
I notice that you didn't mention anything about air blast or coolant.
Look at the broken endmill for hints.
Hi Guys,
Went though 3 end mills trying to mill this path and I'm totally stumped.
I'm running a 2mm center cutting carbide end mill from Accupro with a 8mm LOC. I have the bit in a ER-16 collet with about 15mm sticking out. I ran though the G-wizard calculator and given the bit size they are suggesting a
0.5mm Depth of Cut, 5100 RPM, 160 Feed (mm), and I keep breaking bits.
I though I had it all figured out running the program at 1/2 speed but I just broke my last endmill. Now I need to order more.
What am I doing wrong?
Why don't you look at the code? You are running at F250.
You may also have poor chip clearing technique.
I notice that you didn't mention anything about air blast or coolant.
Look at the broken endmill for hints.
Hey thanks for the replies.
When it breaks, the bit almost appears to get stuck and breaks away when making a pass with full width engagement. There are a few narrow areas where the bit has full width engagement and it feels like the metal is binding or grabbing the bit as it tries to back out of the slot.
I am cutting dry, but there isn't any build up or debris so I think I have that covered.
Also on the F250, let me clarify, I was scaling down the speed in mach3 in order to test out different cutting speeds.
To clarify a few points:
- I am cutting 6061 Aluminium.
- The end mill is a 4 flute carbide endmill.
- I have a cold air gun running on the head as well as manually misting it now and then.
You use 2 flutes in aluminum. Look at the piece that broke off. Are the flutes clogged, or is only 1 flute clogged? (excessive runout)Originally Posted by mooreaa
Let me ask these two specific questions:
1) Are there any issues that may be caused by maxing out the spindle speed? IE maybe more friction?
2) Are there any issues that may be caused by "slowing down" the feed rate using mach3?
I see S1500 in the code. I don't see S5100.
Phil
In G-Wizard, make sure you are in Advanced mode. Look at tool deflection. If it's in orange, don't run it. I wouldn't run this bit with more than 0.0004 inch deflection. My gut says that would be about 0.050 inch depth of cut.
You do want to run at max spindle speed for that small carbide. But you have to be very, very ginger with the feed rates.
I've never had any issues with slowing down the speed override in Mach3.
Personally I would NOT try to run a four flute that small in 6061. I would use a three flute or two flute. If I did my metric conversions right you are only .019 or so DOC and feeding at around 6 IPM. I would most likely try to run this at say .015" doc with the spindle maxed out at 5100 and feed at like 10 IPM with a three flute cutter leaving a stickout of around 5/16". Personally I think you really are gonna have a tough time running dry with that cutter in that material. I would at least hit it with a compressed air blast to really clear the chips or use a mister or something. That cutter is pretty small so optimizing your runout WILL be crucial. If you cannot get it down real tight you will break a cutter often. I have had really good results from using the Maritool 3 flute cutters in aluminum. They are pretty stout cutters and last awhile. The three flute design also seems to run smoother and the finish I get is the best I have been able to find without spending a LOT more cash on cutters. This is the cutter I would use and understand I have NO vested interest in Maritool, I just receive good tooling from them for a good price. For instance I recently ran a LOT of 6061 plate in a paying job with a 3 flute 1/8 inch maritool cutter running .050" deep at 15 IPM with a 7k spindle RPM. This cutter kicked butt in that project and made a whole pile of chips. There was a spot in the code where I ACCIDENTALLY ran the cutter thru a .250" tall wall at 15IPM for maybe .030 or so of full slot distance and the cutter just plowed thru. I was kinda shocked so that may give you an idea how tuff these cutters can be as I thought it would surely snap off. Chip evacuation in 6061 is absolutely crucial in smaller cutters In my experience. Good luck and Peace
1/16 3 Flute Carbide End Mill SE 38 Deg Helix .125 LOC MariTool
Pete
Whenever I use a small cutter (less than 3/32" or so) I am always super conservative as far as depth of cut goes, mainly because I only have 3200rpm spindle, I'm usually doing only a part or two, the time lost due to tool breakage is usually far greater than time saved cutting more aggressively, and breaking a tool is frustrating. It's usually better to reduce DOC than the feedrate if you are trying to reduce tool breakage for 2 reasons- 1. For all endmills the runout needs to be substantially less than the chip load, or else the cutter won't be cutting uniformly. If you can't realistically reduce the runout any more, you can get the same MRR by reducing the DOC and using a faster feedrate. This makes the the combined chipload per tooth (chipload+runout) more uniform. 2. If your chipload is too small, you get rubbing, which dulls the tool and exacerbates tool breakage. You probably don't have to worry about that with your current feeds, but it would start to be a concern if you reduced them to 20% or so.
The vast majority of the times I've broken a bit cutting aluminum is when the flutes get clogged, so I would definitely switch to 2 or 3 flute cutters as others have suggested (the flutes on a similarly sized 3 flute are substantially larger than a similarly sized 4 flute) I've also found, at least for similarly sized drills, is that a TiN coating (or similar) really helps reduce the aluminum clogging the tool. Plenty of coolant (generous mist with air blast, flood, etc) will obviously also help.
Hope this helps,
-Matt
I agree that the four-flute end mill is likely a big part of the problem.
I think Phil nailed it.
Thanks everyone!
Phil: Wow, now I am embarassed. That must be what killed my last bit. Thank you.
With that said, I was still breaking bits running at 160 and 5100 rpm earlier, but managed to finish a pass running at 80 MMPM feedrate.
Pete: Already ordered replacements from MSC but I will have to take a look at Maritool end mills next.
Regarding your recommendation on tooling doesn't less flutes generally mean reduced cut speeds? I will add a three flute on my next order to try it out.
For chip evac, I have an Exair 5215 Cold Air gun blasting the tool/part. Its getting rid of the chips pretty well, but I think I need to get a longer nozzle to get it closer to the smaller bits.
Posting Permissions
