What's new
What's new

Carbide feeds and speeds issues

dreammstr6

Plastic
Joined
Mar 6, 2022
Location
Henagar, Alabama
Try 30% and see how it goes. I'd start at 1×D for depth. Start a little conservatively since you're having issues. If it works out kick the feed up higher. You can run some crazy high feeds (SFM too) if you cut that stepover down.
Your suggestions worked perfectly. Made a part with no signs of wear on the bit running at full commanded speeds. Would you step the Sam up any or adjust anything else for more speed or leave well enough alone lol.
 

eKretz

Diamond; Mod Squad
Joined
Mar 27, 2005
Location
Northwest Indiana, USA
Well, the starting points are just that. If you only have a few parts, you might want to leave things alone. If you have a large number of parts I'd definitely make some tweaks. I don't know your specific machine well, and some of it will depend on its rigidity and condition, but you could probably start by increasing axial depth to ½" - if that goes well you might want to cut your radial DOC and start cranking the feed.
 

dreammstr6

Plastic
Joined
Mar 6, 2022
Location
Henagar, Alabama
Thanks for the advice. My machine is a rigid beast. 16,000 pounds. All in all machine is in pretty good shape. Was bought from Siemens Westinghouse. The never pushed it fast.
I have a decent bit of parts to make so I will play with it. Thanks again for the help
 

eKretz

Diamond; Mod Squad
Joined
Mar 27, 2005
Location
Northwest Indiana, USA
You're welcome, glad it helped a little. Just play it by ear, keep an eye on your cutting edges now and again and you should be able to get it dialed in pretty good. After you get that feed cranked up some, add back radial DOC until it protests (squeal, etc.) and you should be about as good as you're going to get.
 

dreammstr6

Plastic
Joined
Mar 6, 2022
Location
Henagar, Alabama
You're welcome, glad it helped a little. Just play it by ear, keep an eye on your cutting edges now and again and you should be able to get it dialed in pretty good. After you get that feed cranked up some, add back radial DOC until it protests (squeal, etc.) and you should be about as good as you're going to get.
Let me sure I’m understanding correctly. When you say crank the feed up you are referring to sfm correct?
 

eKretz

Diamond; Mod Squad
Joined
Mar 27, 2005
Location
Northwest Indiana, USA
Let me sure I’m understanding correctly. When you say crank the feed up you are referring to sfm correct?

Nope, feed per tooth. SFM you need to keep in a range where your endmill isn't getting edge wear (too fast) but also isn't getting built up edge (too slow). If you drop that stepover %age down you can massively increase your feed and probably SFM too. You kind of need to find the sweet spot - that's determined by the individual machine's characteristics (and of course, the part and workholding play a factor as well). The tricky bit is that those former two play off each other. Increasing depth of cut means you need to decrease feed - and vice versa. What you're actually effectively doing by fine tuning with those changes is attempting to optimize the heat at the cutting edge.
 
Last edited:

dreammstr6

Plastic
Joined
Mar 6, 2022
Location
Henagar, Alabama
Nope, feed per tooth. SFM you need to keep in a range where your endmill isn't getting edge wear (too fast) but also isn't getting built up edge (too slow). If you drop that stepover %age down you can massively increase your feed and probably SFM too. You kind of need to find the sweet spot - that's determined by the individual machine's characteristics (and of course, the part and workholding play a factor as well). The tricky bit is that those former two play off each other. Increasing depth of cut means you need to decrease feed - and vice versa. What you're actually effectively doing by fine tuning with those charges is attempting to optimize the heat at the cutting edge.
Got ya. Thanks
 

Overland

Hot Rolled
Joined
Nov 19, 2017
Location
Greenville, SC
I'm surprised nobody has suggested drilling out the bulk of the material, and then milling to clean out the pocket. I always thought drilling was a more efficient method of metal removal.
Bob
 

eKretz

Diamond; Mod Squad
Joined
Mar 27, 2005
Location
Northwest Indiana, USA
I'm surprised nobody has suggested drilling out the bulk of the material, and then milling to clean out the pocket. I always thought drilling was a more efficient method of metal removal.
Bob

We don't really know much about the actual size of the pocket. You've got to be careful with that too. Leaving small projections that can break loose and jam up the tool can get expensive quick. Sometimes it is a good idea, sometimes not.
 

dreammstr6

Plastic
Joined
Mar 6, 2022
Location
Henagar, Alabama
Why? It's rated for 6k, use it.
Because they actually rate the machine at 8k but if ran at 8k for long periods the spindle over heats. My machine is around 30 years old and I’m not sure if the spindle has been rebuilt. The USA guys that service these machines say to limit to 6k for long runs. And since a spindle cartridge is 10k plus putting it in. I’m going to keep it 5k and under if I can until I’m sure the spindle bearings don’t heat up. Machine been sitting a few years. Might be over cautious but right now I need it running.
 

dreammstr6

Plastic
Joined
Mar 6, 2022
Location
Henagar, Alabama
We don't really know much about the actual size of the pocket. You've got to be careful with that too. Leaving small projections that can break loose and jam up the tool can get expensive quick. Sometimes it is a good idea, sometimes not.
You're welcome, glad it helped a little. Just play it by ear, keep an eye on your cutting edges now and again and you should be able to get it dialed in pretty good. After you get that feed cranked up some, add back radial DOC until it protests (squeal, etc.) and you should be about as good as you're going to get.
Well I’m wondering if the metal I’m running is of varying hardness. Same holding method on each piece which is a 4 jaw chuck bolted to the table. Some pieces I can run the 250sfm 0.375axial doc 0.0008 fpt 30% radial and cutters come out looking brand new. But others will take a brand new bit and chip the edges of the cutter badly. Same holders and checked for runout.
 

eKretz

Diamond; Mod Squad
Joined
Mar 27, 2005
Location
Northwest Indiana, USA
Well I’m wondering if the metal I’m running is of varying hardness. Same holding method on each piece which is a 4 jaw chuck bolted to the table. Some pieces I can run the 250sfm 0.375axial doc 0.0008 fpt 30% radial and cutters come out looking brand new. But others will take a brand new bit and chip the edges of the cutter badly. Same holders and checked for runout.

Try increasing your RPM. Bump it to 300 SFM and see how that goes. Keep the same FPT for now. And the variable material is possible - especially if it came from... Umm... Offshore.
 

dreammstr6

Plastic
Joined
Mar 6, 2022
Location
Henagar, Alabama
Try increasing your RPM. Bump it to 300 SFM and see how that goes. Keep the same FPT for now. And the variable material is possible - especially if it came from... Umm... Offshore.
Thanks for the suggestion. I’ll try that in the morning. I haven’t tried a higher sfm. I have been playing with lower sfm and varying the feed rate using the override. And as far as offshore could be. I’m sure it was the cheapest they could find. Was a 12’ piece of 4” solid round they sawed up. But it is horrible. Was hoping I could set the origin once then just swap parts. That didn’t work. Had a huge difference between parts. One piece isn’t even round. When mounted and touching off. Ended up with part measuring 3.9996 on y axis and 3.9542 on x axis. My eyes could be playing tricks but using a machinist square on the part to the 4 jaw chuck there is gaps and from one side to the opposite you would swear there is no way it can be right. I’m pretty sure the metal is what my issue is. But hey I’m learning more. I have cut a bunch of metal I bought with the mill and followed the speed and feed calculator I have and had no problem. Probably not optimum but nothing like this. But thanks to your wisdom I’m making better progress at decent speeds and not as many bits. Thanks again. Only been playing with this beast about 7 months off and on. Flood coolant is definitely different. The Bridgeport was a lot easier to figure out what the bit liked.
 

eKretz

Diamond; Mod Squad
Joined
Mar 27, 2005
Location
Northwest Indiana, USA
Try increasing your RPM. Bump it to 300 SFM and see how that goes.
300sfm 0.0008 fpt trashed the bit in the first depth of cut.

I wouldn't have expected that by your description of the edge. Try the other direction maybe. 225 SFM. And try dropping your plunge feedrate a bit, maybe take that to .0002" FPT. This would be a lot easier in person...
 

dreammstr6

Plastic
Joined
Mar 6, 2022
Location
Henagar, Alabama
I wouldn't have expected that by your description of the edge. Try the other direction maybe. 225 SFM. And try dropping your plunge feedrate a bit, maybe take that to .0002" FPT. This would be a lot easier in person...
Will do. Yeah would definitely be easier. 19 more pockets to go lol. I have tried down to 200 sfm at 0.0008 fpt. Best results across multiple parts was to slow the override down to 56% on feed which would be 0.0005 fpt. One thing I forgot to mention is I’m doing a ramp down into the part to make sure chips wasn’t my issue. I have done the pocket in zigzag and spiral. Spiral seems to help with tool life. It’s just strange. I have ran aluminum and 416 stainless on this machine with 1/4” and 1/8” bits with decent tool life.(feature required the small bits) The machine spent most of it’s life cutting copper and did wonderful. So I know it’s either me or the metal. My cam software has done great on the ez-traks. (Bobcad). I loaded a new bit and running 250sfm fpt is reduced to 0.0005 by override. Depth of cut is 0.323 or so since it did even depths. Will see how the bit looks after running one part then another and go from there.
 

dreammstr6

Plastic
Joined
Mar 6, 2022
Location
Henagar, Alabama
I wouldn't have expected that by your description of the edge. Try the other direction maybe. 225 SFM. And try dropping your plunge feedrate a bit, maybe take that to .0002" FPT. This would be a lot easier in person...
I just noticed something that might click for you. I had to run some of the pockets on the ez-trak due to the vmc being down. (Bad cable) when I was running the ez-trak I was running 1600rpm with a feed of 3.5 ipm and a axial doc of 0.65” and radial was 50%. The chips coming off were gold and turned blue when they landed. (No coolant) that machine is definitely not as rigid. I was using same work holding. (Transferred same 4 jaw to Bridgeport) according to the speed and feed calculator I plugged that data in I was running a fpt of 0.0005 which is where I’m getting best life out of bit on vmc. I should be able to achieve a higher fpt but it strange that 0.0005 seems to work for both machines.
 

AARONT

Stainless
Joined
Feb 19, 2013
Location
Madison, WI
Because they actually rate the machine at 8k but if ran at 8k for long periods the spindle over heats. My machine is around 30 years old and I’m not sure if the spindle has been rebuilt. The USA guys that service these machines say to limit to 6k for long runs. And since a spindle cartridge is 10k plus putting it in. I’m going to keep it 5k and under if I can until I’m sure the spindle bearings don’t heat up. Machine been sitting a few years. Might be over cautious but right now I need it running.
We have a Tree 1060 and only run over 6k if it's for engraving or a quick edge break. 6k and under we can run all day.
 

dreammstr6

Plastic
Joined
Mar 6, 2022
Location
Henagar, Alabama
We have a Tree 1060 and only run over 6k if it's for engraving or a quick edge break. 6k and under we can run all day.
Good to know. I was talking to Tom at ZPS about a 1060 they had. At least some of those had spindle cooling. And could run the 8k long periods. The one they had on the floor did. Been considering get a 1060 or another 1050.
 








 
Top