What's new
What's new

Carbide feeds and speeds issues

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...
Just finished the pocket running 250 sfm 0.0005 fpt (reduced via override) depth of 0.323 and radial of 28% the bit looks good slightly discolored at bottom 0.375 so I’m going to step up sfm and keep fpt the same. (0.0005)
 

eKretz

Diamond; Mod Squad
Joined
Mar 27, 2005
Location
Northwest Indiana, USA
Best I can get so far with my phone.

I see a LOT more edge wear on the bottom of the cutter than I'd expect. I felt like your ramp feedrate was too high, I think that confirms it. You also might try exploring another method of getting to depth rather than ramping. Perhaps plunging almost to depth straight down at one end of the pocket and dropping the cutter down in that hole at each successive path around rather than ramping would work better. Alternatively you could use a drill to make that first hole almost to full depth then switch to the endmill and use the same strategy.

Also: is there any clearance in the center of that cutter? It almost looks like there's none. That could be causing much of your trouble also. (Lay a ruler or something flat along the bottom of the cutter... Do you see air in the middle or no?) Also, how much time is on that cutter?
 

dreammstr6

Plastic
Joined
Mar 6, 2022
Location
Henagar, Alabama
I see a LOT more edge wear on the bottom of the cutter than I'd expect. I felt like your ramp feedrate was too high, I think that confirms it. You also might try exploring another method of getting to depth rather than ramping. Perhaps plunging almost to depth straight down at one end of the pocket and dropping the cutter down in that hole at each successive path around rather than ramping would work better. Alternatively you could use a drill to make that first hole almost to full depth then switch to the endmill and use the same strategy.

Also: is there any clearance in the center of that cutter? It almost looks like there's none. That could be causing much of your trouble also. (Lay a ruler or something flat along the bottom of the cutter... Do you see air in the middle or no?) Also, how much time is on that cutter?
There is clearance not much but some. That cutter was new just did the one pocket so about an hour. What is funny is here is pictures of one I killed I think was at 250sfm 0.0008 fpt 28% radial 0.325 depth. And it was ramping in also. End looks much better and more time on it.
 

Attachments

  • AC60E9F8-789B-4B38-B13C-4F90660E139F.jpeg
    AC60E9F8-789B-4B38-B13C-4F90660E139F.jpeg
    695.3 KB · Views: 4
  • 841FD661-E97C-405F-9E34-D3780444F1BE.jpeg
    841FD661-E97C-405F-9E34-D3780444F1BE.jpeg
    761 KB · Views: 4

eKretz

Diamond; Mod Squad
Joined
Mar 27, 2005
Location
Northwest Indiana, USA
That end still looks pretty bad to me. I think you are exceeding the available clearance when ramping due to excessive ramp feedrate. You ideally want to keep the endmill from cutting across the entire bottom while ramping, which is why you'll often see cutters made specifically for ramping with a lot more clearance in the center. You want to keep the cutting happening at the periphery. If you can't do that, better to plunge straight in and drop down every time you come around the path loop.
 

dreammstr6

Plastic
Joined
Mar 6, 2022
Location
Henagar, Alabama
That end still looks pretty bad to me. I think you are exceeding the available clearance when ramping due to excessive ramp feedrate. You ideally want to keep the endmill from cutting across the entire bottom while ramping, which is why you'll often see cutters made specifically for ramping with a lot more clearance in the center. You want to keep the cutting happening at the periphery. If you can't do that, better to plunge straight in and drop down every time you come around the path loop.
Good information. I swapped back to plunge. I started with plunge but thought maybe chips was getting caught and damaging the cutter on start of cut so I tried ramping and did better. Running another pocket now. Will prep some new bits and see what happens. Maybe I can get another pocket or two out of the one running. Thanks again for the suggestions
 

dreammstr6

Plastic
Joined
Mar 6, 2022
Location
Henagar, Alabama
That end still looks pretty bad to me. I think you are exceeding the available clearance when ramping due to excessive ramp feedrate. You ideally want to keep the endmill from cutting across the entire bottom while ramping, which is why you'll often see cutters made specifically for ramping with a lot more clearance in the center. You want to keep the cutting happening at the periphery. If you can't do that, better to plunge straight in and drop down every time you come around the path loop.
Here is pictures of the bit I killed on first depth cut at 300sfm earlier. Finally unloaded from carousel.
 

Attachments

  • 9FCEB7BE-E8FB-4D9F-AD17-E21EAAA69B5C.jpeg
    9FCEB7BE-E8FB-4D9F-AD17-E21EAAA69B5C.jpeg
    750.3 KB · Views: 7
  • B10B3A54-8A87-4C61-87FF-9F3F33228CF3.jpeg
    B10B3A54-8A87-4C61-87FF-9F3F33228CF3.jpeg
    765.4 KB · Views: 7

AARONT

Stainless
Joined
Feb 19, 2013
Location
Madison, WI
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.
Bob & Tom over there at ZPS are extremely helpful and knowledgeable. They've helped us out a bunch with just a phone call.
 

dreammstr6

Plastic
Joined
Mar 6, 2022
Location
Henagar, Alabama
That end still looks pretty bad to me. I think you are exceeding the available clearance when ramping due to excessive ramp feedrate. You ideally want to keep the endmill from cutting across the entire bottom while ramping, which is why you'll often see cutters made specifically for ramping with a lot more clearance in the center. You want to keep the cutting happening at the periphery. If you can't do that, better to plunge straight in and drop down every time you come around the path loop.
250sfm 0.0005fpt 0.325 axial 28% radial. New bit one pocket plunge lead in
 

Attachments

  • 07F3F4B9-21E3-41F7-8B42-CECAE6F03183.jpeg
    07F3F4B9-21E3-41F7-8B42-CECAE6F03183.jpeg
    707.3 KB · Views: 3
  • 566A08A2-8743-4B50-A56C-74417439D3B2.jpeg
    566A08A2-8743-4B50-A56C-74417439D3B2.jpeg
    768 KB · Views: 3

eKretz

Diamond; Mod Squad
Joined
Mar 27, 2005
Location
Northwest Indiana, USA
Hmm. Very odd that it's so inconsistent. Who makes the endmills? Have you noticed any pattern in terms of which toolholder you're using and whether one has more failures or works better? Maybe get completely away from the plumge and try pre-drilling and only dropping down into the pre-drilled hole. Gotta try to find the variable that's causing the issue.
 

dreammstr6

Plastic
Joined
Mar 6, 2022
Location
Henagar, Alabama
Hmm. Very odd that it's so inconsistent. Who makes the endmills? Have you noticed any pattern in terms of which toolholder you're using and whether one has more failures or works better? Maybe get completely away from the plumge and try pre-drilling and only dropping down into the pre-drilled hole. Gotta try to find the variable that's causing the issue.
It is very odd. I decided to run only 3 specific tool holders to limit the variables. So I run those three bits then swap out and re register length offsets. I don’t notice any patterns which is why I reached out I have tried everything I know which isn’t a lot lol. The bits are HTC 120-4375. I have good luck with their bits on other projects. Even tried a Roman cutting tools 3/8” rougher bit. It lasted maybe 4 pockets. I have about decided it is the metal that is inconsistent. Once the pockets are done I have to mill some inside circles out of 1” flat steel. Will see how everything does on it.
 

dreammstr6

Plastic
Joined
Mar 6, 2022
Location
Henagar, Alabama
Hmm. Very odd that it's so inconsistent. Who makes the endmills? Have you noticed any pattern in terms of which toolholder you're using and whether one has more failures or works better? Maybe get completely away from the plumge and try pre-drilling and only dropping down into the pre-drilled hole. Gotta try to find the variable that's causing the issue.
I bumped the sfm up to 300 and left everything else the same since that picture was a little blue. Yeah after that pocket(2nd on bit) may it rest in piece. Has more craters on the cutting edge than the interstate in Alabama does…..
 

eKretz

Diamond; Mod Squad
Joined
Mar 27, 2005
Location
Northwest Indiana, USA
It is very odd. I decided to run only 3 specific tool holders to limit the variables. So I run those three bits then swap out and re register length offsets. I don’t notice any patterns which is why I reached out I have tried everything I know which isn’t a lot lol. The bits are HTC 120-4375. I have good luck with their bits on other projects. Even tried a Roman cutting tools 3/8” rougher bit. It lasted maybe 4 pockets. I have about decided it is the metal that is inconsistent. Once the pockets are done I have to mill some inside circles out of 1” flat steel. Will see how everything does on it.

Hmm, I'm not familiar with that brand so did a little Google sleuthing and found this:

I used the "Hot Mill" in the past, but you won't see them in this shop anymore. Initially we had pretty good success with them. Bought a fair amount. Then we started breaking tools left & right, running the same programs that they used to. After talking to a few reps around the country, we very strongly suspected that they went to a cheaper carbide blank, likely China sourced. Whatever the reason, having 2 "identical" but inconsistent tools costs more than having one good one.

The "Hot Mill" according to that guy was apparently a "premium" HTC brand offering. I think if I were you I might try an endmill or three from a more established brand.
 

dreammstr6

Plastic
Joined
Mar 6, 2022
Location
Henagar, Alabama
Hmm, I'm not familiar with that brand so did a little Google sleuthing and found this:



The "Hot Mill" according to that guy was apparently a "premium" HTC brand offering. I think if I were you I might try an endmill or three from a more established brand.
I thought about that but I have a pile of other brands also including some that was tialn coated I was tired of crying. I did order a few more from McMaster to test. Fast and not to horrible price.
 

dreammstr6

Plastic
Joined
Mar 6, 2022
Location
Henagar, Alabama
Hmm, I'm not familiar with that brand so did a little Google sleuthing and found this:



The "Hot Mill" according to that guy was apparently a "premium" HTC brand offering. I think if I were you I might try an endmill or three from a more established brand.
I’m thinking chips or debris caused this damage. What is your opinion ? The tip is very sharp and the edges are sharp right to the damage. I was running it at over 10ipm and did well on a few pockets then I saw this damage.
 

Attachments

  • 08661CF2-B77C-4948-B8E8-F7115FD012C1.jpeg
    08661CF2-B77C-4948-B8E8-F7115FD012C1.jpeg
    868.4 KB · Views: 4
Last edited:

eKretz

Diamond; Mod Squad
Joined
Mar 27, 2005
Location
Northwest Indiana, USA
I’m thinking chips or debris caused this damage. What is your opinion ? The tip is very sharp and the edges are sharp right to the damage. I was running it at over 10ipm and did well on a few pockets then I saw this damage.

Very possible. I thought you had mentioned blasting them out with quite a few coolant nozzles though. Are you seeing much evidence of chips in the pocket when you've finished one?
 

dreammstr6

Plastic
Joined
Mar 6, 2022
Location
Henagar, Alabama
Very possible. I thought you had mentioned blasting them out with quite a few coolant nozzles though. Are you seeing much evidence of chips in the pocket when you've finished one?
I have 8 nozzles blasting away. I haven’t seen much if any chips when done. Maybe one or two. But that’s the only thing I can come up with for the damage. Because it is still sharp enough to cut skin on the tip. Maybe at some point in the cut the nozzles aren’t enough and I just don’t see/notice it.
 

eKretz

Diamond; Mod Squad
Joined
Mar 27, 2005
Location
Northwest Indiana, USA
I have 8 nozzles blasting away. I haven’t seen much if any chips when done. Maybe one or two. But that’s the only thing I can come up with for the damage. Because it is still sharp enough to cut skin on the tip.

Is this still the HTC endmill? I would strongly suggest trying something from a more established brand. That sort of failure pattern is too similar to what that other guy was describing. You might try using an air blast rather than coolant for a part or two also so you can see what is going on better.
 








 
Top