What's new
What's new

Carbide feeds and speeds issues

dreammstr6

Plastic
Joined
Mar 6, 2022
Location
Henagar, Alabama
I’m looking for a little guidance. I have a tree vmc 1050 running flood coolant. I’m going through bits like candy and have tried every feed speed calculator I can find. I’m cutting 1045 steel. Nothing special. I have tried 3/8” carbide uncoated and 1/4” carbide tialn coated. I’m make a 3” pocket 1.3” deep and a bit only lasts maybe two parts if I’m lucky. I have tried a ton of speeds and feeds. One was 317fpm on the 3/8”. I have tried various depths and step overs. I’m confused why they won’t hold up. On my ez-trak they hold up better with no coolant. Any suggestions on feeds and speeds that have worked for you?
 

rklopp

Diamond
Joined
Feb 27, 2001
Location
Redwood City, CA USA
I’m looking for a little guidance. I have a tree vmc 1050 running flood coolant. I’m going through bits like candy and have tried every feed speed calculator I can find. I’m cutting 1045 steel. Nothing special. I have tried 3/8” carbide uncoated and 1/4” carbide tialn coated. I’m make a 3” pocket 1.3” deep and a bit only lasts maybe two parts if I’m lucky. I have tried a ton of speeds and feeds. One was 317fpm on the 3/8”. I have tried various depths and step overs. I’m confused why they won’t hold up. On my ez-trak they hold up better with no coolant. Any suggestions on feeds and speeds that have worked for you?
How much chatter (squeal)? I expect a lot with a 3/8 cutter going 1.3” deep. 1/4” must be even worse. What not take out most of the material with a bigger cutter and clean the corners with a smaller cutter if you have to?
 

dreammstr6

Plastic
Joined
Mar 6, 2022
Location
Henagar, Alabama
How are you clearing the chips - ..............recutting chips is one of the quickest ways to kill an EM


Clearing with 8 nozzles of flood coolant. I have tried ramping in and changing depth of cut from .125 to 0.65
 

dreammstr6

Plastic
Joined
Mar 6, 2022
Location
Henagar, Alabama
How much chatter (squeal)? I expect a lot with a 3/8 cutter going 1.3” deep. 1/4” must be even worse. What not take out most of the material with a bigger cutter and clean the corners with a smaller cutter if you have to?
I should of said final depth 1.3. I’m stepping down in at 0.125-0.65 I have tried various things. I don’t really get any squeal for the most part. I have at times playing with the feeds. And as far as the bigger cutters same issue. I can’t seem to find what this beast likes and a 1/4” or 3/8” doesn’t make me cuss as much when it goes flying around the enclosure. Starting small and get it figured out then move to bigger.
 

dreammstr6

Plastic
Joined
Mar 6, 2022
Location
Henagar, Alabama
Just thought of one thing. On the ez-trak I can run the pocket with a 3/8” but cutting at 1500rpm (spindle max 3000) and I think it was 1.5” per minute feed and was getting nice gold chips that turned blue. No coolant. But if I did do mist coolant from spray bottle the chips would be really small and silver. The tree didn’t like those settings. Right now I’m trying a 1/4 tialn bit at 3405rpm and 3.5 ipm radial cut 0.125 axial cut 0.1182.
 

eKretz

Diamond; Mod Squad
Joined
Mar 27, 2005
Location
Northwest Indiana, USA
If that's a 4-flute, your feed is way too low. Probably rubbing the cutter until it's dull. I'd expect you need to double or triple that feed at least. You're only at .0002" fpt. That's more where I'd expect to see things if the cutter was buried full depth and cutting full width. Kick that feed to 7 IPM and give it a go. I'd stick with the ⅜" if you can't run bigger. Use the biggest cutter you can get away with.
 

dreammstr6

Plastic
Joined
Mar 6, 2022
Location
Henagar, Alabama
If that's a 4-flute, your feed is way too low. Probably rubbing the cutter until it's dull. I'd expect you need to double or triple that feed at least. You're only at .0002" fpt. That's more where I'd expect to see things if the cutter was buried full depth and cutting full width. Kick that feed to 7 IPM and give it a go. I'd stick with the ⅜" if you can't run bigger. Use the biggest cutter you can get away with.
So the 1/4” you would run at around 3400rpm and 7ipm?
 

eKretz

Diamond; Mod Squad
Joined
Mar 27, 2005
Location
Northwest Indiana, USA
So the 1/4” you would run at around 3400rpm and 7ipm?

Is 3400 all you've got? What's the manufacturer recommending for SFM range? That's ~220 SFM, which is pretty low if you're able to flood it. If you give it more RPM, just increase the feed proportionately. Gotta get that feed up though.
 

dreammstr6

Plastic
Joined
Mar 6, 2022
Location
Henagar, Alabama
If that's a 4-flute, your feed is way too low. Probably rubbing the cutter until it's dull. I'd expect you need to double or triple that feed at least. You're only at .0002" fpt. That's more where I'd expect to see things if the cutter was buried full depth and cutting full width. Kick that feed to 7 IPM and give it a go. I'd stick with the ⅜" if you can't run bigger. Use the biggest cutter you can get away with.
Another question for you. How would you run the 3/8” bit it is a 4 flute uncoated carbide 1” loc what rpm,ipm, radial doc, axial doc would you recommend me trying?
 

dreammstr6

Plastic
Joined
Mar 6, 2022
Location
Henagar, Alabama
Is 3400 all you've got? What's the manufacturer recommending for SFM range? That's ~220 SFM, which is pretty low. If you give it more RPM, just increase the feed proportionately. Gotta get that feed up though.
I have a 6k spindle I like to keep at 5k and under but can do 6k no problem. The one speed feed calculator recommended 220sfm for the 1/4”
 

dreammstr6

Plastic
Joined
Mar 6, 2022
Location
Henagar, Alabama
If that's a 4-flute, your feed is way too low. Probably rubbing the cutter until it's dull. I'd expect you need to double or triple that feed at least. You're only at .0002" fpt. That's more where I'd expect to see things if the cutter was buried full depth and cutting full width. Kick that feed to 7 IPM and give it a go. I'd stick with the ⅜" if you can't run bigger. Use the biggest cutter you can get away with.
Kicked it up to 6 ipm with override. It lasted maybe 10 minutes at that rate and said snap. Was a brand new bit didn’t last one part.
 

eKretz

Diamond; Mod Squad
Joined
Mar 27, 2005
Location
Northwest Indiana, USA
Kicked it up to 6 ipm with override. It lasted maybe 10 minutes at that rate and said snap. Was a brand new bit didn’t last one part.

Was that the ¼"? Get away from that small cutter... In non-hardened 1045 I'd want to be starting out at 300-350 SFM and adjusting from there. Also, have you checked runout at the tool? Sounds like something weird is going on. I'll also stress again: use the largest cutter you can get away with. Stop and check your edges after a few minutes and see what the cutting edge looks like. If it's getting edge wear, drop your SFM. If you see signs of BUE, increase your SFM.
 
Last edited:

dreammstr6

Plastic
Joined
Mar 6, 2022
Location
Henagar, Alabama
Was that the ¼"? Get away from that small cutter.
That was the 1/4. Give me some suggestions on a 3/8” 4flute solid carbide uncoated end mill. Fpm, rpm, ipm, radial and axial doc and I will give it a shot. Got 12 more coming in tomorrow. I’ll be glad to try suggestions. I was cutting last with the 3/8” at 2200 rpm and I think around 3.5ipm and it lasted a couple parts. I was just playing with spindle and feed overrides until I got decent sized chips.
 

eKretz

Diamond; Mod Squad
Joined
Mar 27, 2005
Location
Northwest Indiana, USA
That was the 1/4. Give me some suggestions on a 3/8” 4flute solid carbide uncoated end mill. Fpm, rpm, ipm, radial and axial doc and I will give it a shot. Got 12 more coming in tomorrow. I’ll be glad to try suggestions. I was cutting last with the 3/8” at 2200 rpm and I think around 3.5ipm and it lasted a couple parts. I was just playing with spindle and feed overrides until I got decent sized chips.

Uncoated ⅜" I'd try starting out more like 250 SFM and maybe start out at .0008" to .001" IPT since you're having issues. I'd try 1 × D for depth on the initial cut, then maybe ⅛" stepovers at a higher feed if it will take it. You really need to inspect the edges after a little cutting, and also check runout. You may have harder material than you think or a runout issue. Runout will cause all kinds of trouble with putting any feed to the cutter since it will be cutting with pretty much only one tooth.
 

dreammstr6

Plastic
Joined
Mar 6, 2022
Location
Henagar, Alabama
Was that the ¼"? Get away from that small cutter... In non-hardened 1045 I'd want to be starting out at 300-350 SFM and adjusting from there. Also, have you checked runout at the tool? Sounds like something weird is going on. I'll also stress again: use the largest cutter you can get away with. Stop and check your edges after a few minutes and see what the cutting edge looks like. If it's getting edge wear, drop your SFM. If you see signs of BUE, increase your SFM.
Was that the ¼"? Get away from that small cutter... In non-hardened 1045 I'd want to be starting out at 300-350 SFM and adjusting from there. Also, have you checked runout at the tool? Sounds like something weird is going on. I'll also stress again: use the largest cutter you can get away with. Stop and check your edges after a few minutes and see what the cutting edge looks like. If it's getting edge wear, drop your SFM. If you see signs of BUE, increase your SFM.
I checked for runout when I got the holders. Haven’t lately. Will do that in the morning.
 

dreammstr6

Plastic
Joined
Mar 6, 2022
Location
Henagar, Alabama
Uncoated ⅜" I'd try starting out more like 250 SFM and maybe start out at .0008" to .001" IPT since you're having issues. I'd try 1 × D for depth on the initial cut, then maybe ⅛" stepovers at a higher feed if it will take it. You really need to inspect the edges after a little cutting, and also check runout. You may have harder material than you think or a runout issue. Runout will cause all kinds of trouble with putting any feed to the cutter since it will be cutting with pretty much only one tooth.
Ok just started a new file with the 3/8” bit. At 250sfm it puts my rpm 2546.4791 I set the feed per tooth to 0.0008 and plunge feed per tooth to 0.0004. Cutting feed rate is 8.1487 ipm plunge feed rate is 4.0744 ipm what depth of cut and step over you recommend? The usual 50% bit diameter?
 

eKretz

Diamond; Mod Squad
Joined
Mar 27, 2005
Location
Northwest Indiana, USA
Ok just started a new file with the 3/8” bit. At 250sfm it puts my rpm 2546.4791 I set the feed per tooth to 0.0008 and plunge feed per tooth to 0.0004. Cutting feed rate is 8.1487 ipm plunge feed rate is 4.0744 ipm what depth of cut and step over you recommend? The usual 50% bit diameter?

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.
 

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.
Thanks I will give that a try in the morning and see what happens. I appreciate your help.
 

dreammstr6

Plastic
Joined
Mar 6, 2022
Location
Henagar, Alabama
Thanks I will give that a try in the morning and see what happens. I appreciate your help.
Just starting to cut. I did find some bad 3/8” holders with runout around 0.002 but the others was good. So we shall see what happens with new program with the new speeds and feeds and depths suggested.
 








 
Top