This video by Onsrud explains the basics of Feeds & Speed and Chip Load
Feeds & Speed and Chip Load Explained
- Rcnewcomb
- Vectric Archimage
- Posts: 6379
- Joined: Fri Nov 04, 2005 5:54 am
- Model of CNC Machine: 24x36 GCnC/WinCNC with ATC
- Location: San Jose, California, USA
- Contact:
Feeds & Speed and Chip Load Explained
- Randall Newcomb
10 fingers in, 10 fingers out, another good day in the shop
10 fingers in, 10 fingers out, another good day in the shop
- Leo
- Vectric Wizard
- Posts: 4356
- Joined: Sat Jul 14, 2007 3:02 am
- Model of CNC Machine: 1300 x 1300 x 254 Chinese Made
- Location: East Freetown, Ma.
- Contact:
Re: Feeds & Speed and Chip Load Explained
Randal that is a very good instructional video.
I like that while mentioning LMT-Onsrud cutters he was not pushing for sales.
Bravo on that.
I have been thinking about a cutting parameters video for a long time now.
Right now I am up to my eyeballs building a laundry room and making kitchen cabinets.
I am in the middle of making cool things video series - on hold
Maybe after cool things
There are a lot of things to think about with cutting parameters, some mentioned and some not in the Onsrud video.
Process
Slotting - profiling - facing - perifery - plunging - engraving - vCarving -
Material being cut
Plastic - mdf - oak - bubinga - pine - balsa - brass - aluminum
Accel - decel
Cutting 3D - cutting corners - Can the "machine" make accurate corners - lost steps
I can cut a straight line at 500 IPM - maybe not so good trying to make a square
Ability of the machine
Hand held router for spindle - Varieble speed spindle - ER11 collet size(lower torque curve)
I am sure there is more
I like that while mentioning LMT-Onsrud cutters he was not pushing for sales.
Bravo on that.
I have been thinking about a cutting parameters video for a long time now.
Right now I am up to my eyeballs building a laundry room and making kitchen cabinets.
I am in the middle of making cool things video series - on hold
Maybe after cool things
There are a lot of things to think about with cutting parameters, some mentioned and some not in the Onsrud video.
Process
Slotting - profiling - facing - perifery - plunging - engraving - vCarving -
Material being cut
Plastic - mdf - oak - bubinga - pine - balsa - brass - aluminum
Accel - decel
Cutting 3D - cutting corners - Can the "machine" make accurate corners - lost steps
I can cut a straight line at 500 IPM - maybe not so good trying to make a square
Ability of the machine
Hand held router for spindle - Varieble speed spindle - ER11 collet size(lower torque curve)
I am sure there is more
Imagine the Possibilities of a Creative mind, combined with the functionality of CNC
-
- Posts: 15
- Joined: Tue May 23, 2023 6:16 pm
- Model of CNC Machine: Onefinity
Re: Feeds & Speed and Chip Load Explained
"..There are a lot of things to think about ... some mentioned and some not...(such as)- engraving - vCarving"
When the bit has a 30 degree cutting angle and a 0.010" tip, the chip load math is merely difficult. When the cutting edge is 0.5" long, but only 0.012" is beneath the substrate surface, I don't know what the chip load calculation is doing. But when working with a material that both cuts and melts (brass) even the logical steps in those calculations become harder to trust.
Serial failures with my Amana single-flute cutters led to a consult with the engineers. They said that as the tip gets smaller, the required RPM increases and the IPM decreases. At fast IPMs, you're effectively scraping a point across the surface and breakage is more likely. Their suggestion was an impossibly fast RPM (60k) and impossibly slow IPM (2-5). The clock dials I'm making would take days to carve, and my spindle maximum is 24K. Reading other posts here, I'm also reminded of features I can't measure on my hobbyist machine (Onefinity) such as rigidity. Yes, they sell stiffer devices, but I'm not confident that paying that cost would solve these issues. Another factor concerns the variations of alloys. Concerning only one metal (brass) there are lots of Alloy 260 (which is brittle "cartridge brass") but I can't find sheets of Alloy 360 (machineable "clock brass"). Surely that also affects aluminum and various plastics.
I reached this thread via a series Leo started. That thread concerned factors to include in his project (a reference for hobbyists on feeds/speeds).
1. Brass was mentioned, but not alloy-related adjustments to the feeds/speeds.
2. If manufacturers have data on 'rigidity', then it could help to tell us what terms to use when we ask about the stiffness of the CNC we want/have. By the way, very stiff way tubes might not matter if we have a wiggly machine bed.
When the bit has a 30 degree cutting angle and a 0.010" tip, the chip load math is merely difficult. When the cutting edge is 0.5" long, but only 0.012" is beneath the substrate surface, I don't know what the chip load calculation is doing. But when working with a material that both cuts and melts (brass) even the logical steps in those calculations become harder to trust.
Serial failures with my Amana single-flute cutters led to a consult with the engineers. They said that as the tip gets smaller, the required RPM increases and the IPM decreases. At fast IPMs, you're effectively scraping a point across the surface and breakage is more likely. Their suggestion was an impossibly fast RPM (60k) and impossibly slow IPM (2-5). The clock dials I'm making would take days to carve, and my spindle maximum is 24K. Reading other posts here, I'm also reminded of features I can't measure on my hobbyist machine (Onefinity) such as rigidity. Yes, they sell stiffer devices, but I'm not confident that paying that cost would solve these issues. Another factor concerns the variations of alloys. Concerning only one metal (brass) there are lots of Alloy 260 (which is brittle "cartridge brass") but I can't find sheets of Alloy 360 (machineable "clock brass"). Surely that also affects aluminum and various plastics.
I reached this thread via a series Leo started. That thread concerned factors to include in his project (a reference for hobbyists on feeds/speeds).
1. Brass was mentioned, but not alloy-related adjustments to the feeds/speeds.
2. If manufacturers have data on 'rigidity', then it could help to tell us what terms to use when we ask about the stiffness of the CNC we want/have. By the way, very stiff way tubes might not matter if we have a wiggly machine bed.
- Leo
- Vectric Wizard
- Posts: 4356
- Joined: Sat Jul 14, 2007 3:02 am
- Model of CNC Machine: 1300 x 1300 x 254 Chinese Made
- Location: East Freetown, Ma.
- Contact:
Re: Feeds & Speed and Chip Load Explained
Ken - with the conditions you state here it appears that the cutting conditions are certainly not normal. In cases like that the spped and feeds and chipload are still important. There are limits though. some limits are max RPM, Max feedrate. Max limits on many router spindles can be RPM at max 25,000. High speed machining can go MUCH higher but those machine are VERY expensive and SUPER rigid. They are NOT hobby level machines.kenagyd wrote: ↑Sun Feb 02, 2025 2:47 am"..There are a lot of things to think about ... some mentioned and some not...(such as)- engraving - vCarving"
When the bit has a 30 degree cutting angle and a 0.010" tip, the chip load math is merely difficult. When the cutting edge is 0.5" long, but only 0.012" is beneath the substrate surface, I don't know what the chip load calculation is doing. But when working with a material that both cuts and melts (brass) even the logical steps in those calculations become harder to trust.
Serial failures with my Amana single-flute cutters led to a consult with the engineers. They said that as the tip gets smaller, the required RPM increases and the IPM decreases. At fast IPMs, you're effectively scraping a point across the surface and breakage is more likely. Their suggestion was an impossibly fast RPM (60k) and impossibly slow IPM (2-5). The clock dials I'm making would take days to carve, and my spindle maximum is 24K. Reading other posts here, I'm also reminded of features I can't measure on my hobbyist machine (Onefinity) such as rigidity. Yes, they sell stiffer devices, but I'm not confident that paying that cost would solve these issues. Another factor concerns the variations of alloys. Concerning only one metal (brass) there are lots of Alloy 260 (which is brittle "cartridge brass") but I can't find sheets of Alloy 360 (machineable "clock brass"). Surely that also affects aluminum and various plastics.
I reached this thread via a series Leo started. That thread concerned factors to include in his project (a reference for hobbyists on feeds/speeds).
1. Brass was mentioned, but not alloy-related adjustments to the feeds/speeds.
2. If manufacturers have data on 'rigidity', then it could help to tell us what terms to use when we ask about the stiffness of the CNC we want/have. By the way, very stiff way tubes might not matter if we have a wiggly machine bed.
I am not sure about a few things you mentioned
.010 tip
.012 DOC
brass melting ?
I am aware that you cannot always get 360 free machining brass in all forms but brass is still pretty easy to cut
Yes - a rigid machine can be defeated by a flimsy workholding. It all needs to work together.
I have done clock faces on brass with a V bit on sheet brass. No it is not easy. I have not done a lot of that work, but I will consider a TBN (tapered Ball Nose) with a .5mm ball tip. Chipload will be a challange but it will be essential. If the brass is melting, and it should not malt, that means that the RPM to feedrate ratio is off and way to much heat is being generated, hence melting the brass. Therefore, the RPM must be lowered and/or the feedrate increased to bring the chipload into a more reasonable ratio.
The other thing about clock faces is holddown. Double sided tape maybe. I was also thinking of a thick plate on top of the clock face with access holes to do the machining.
Just some thoughts
BTW - what was the series that you saw?
Imagine the Possibilities of a Creative mind, combined with the functionality of CNC
-
- Posts: 15
- Joined: Tue May 23, 2023 6:16 pm
- Model of CNC Machine: Onefinity
Re: Feeds & Speed and Chip Load Explained
If I recall correctly, you started a thread in Summer 2024, inviting folks to suggest factors that matter when a hobbyist chooses feeds & speeds. (It came up when I used the search term, “brass”).
I’ll be interested to see your project unfold. My first efforts used an Amana 1- flute insert into a 1/2” diameter arbor. The tip sizes were 0.005”, and every one of them broke. I figured I must be using terrible settings, with every tip from a well-known company breaking. But I was even more surprised with the extreme settings those engineers called for. Frankly, those aren’t possible for hobbyist machines.
I next tried 2-flute cutters (Amana and Onsrud) with 30 degree included angles, 0.010” tip. Even with DOC at 0.005” per pass (0.012 final depth) the tips broke.
My first successes came with a new approach. I used a 0.030” mill to hog out material, and only asked the V-bits to reach into the corners. The maker (Bits&Bits) told me another client’s best results were at 16k RPM, 20 IPM, DOC 0.005”. They got there from trial and error, rather than calculations. The TBN that you describe has a 0.5 mm tip. That’ 0.019”, about twice the size of the bit I’ve been using.
As a newcomer, I quote others rather than claiming personal knowledge. Several have said the difficulty with brass includes its tendency to soften when we’d prefer that it cut. That, too, is said to cause more breakage.
Our Case Western University has a “Maker’s Space” where teachers of Mechanical Engineering allow non-students to work on projects. Though they actually ran the metal CNC, I learned a lot of associated ideas. I now bolt a piece of Delrin to the table. After I surface the Delrin I use plastic bolts to secure the brass to it. Though that doesn’t rule out “chatter” from problems with rigidity, it ‘s the most secure work-holding I’ve seen.
I’ll be interested to see your project unfold. My first efforts used an Amana 1- flute insert into a 1/2” diameter arbor. The tip sizes were 0.005”, and every one of them broke. I figured I must be using terrible settings, with every tip from a well-known company breaking. But I was even more surprised with the extreme settings those engineers called for. Frankly, those aren’t possible for hobbyist machines.
I next tried 2-flute cutters (Amana and Onsrud) with 30 degree included angles, 0.010” tip. Even with DOC at 0.005” per pass (0.012 final depth) the tips broke.
My first successes came with a new approach. I used a 0.030” mill to hog out material, and only asked the V-bits to reach into the corners. The maker (Bits&Bits) told me another client’s best results were at 16k RPM, 20 IPM, DOC 0.005”. They got there from trial and error, rather than calculations. The TBN that you describe has a 0.5 mm tip. That’ 0.019”, about twice the size of the bit I’ve been using.
As a newcomer, I quote others rather than claiming personal knowledge. Several have said the difficulty with brass includes its tendency to soften when we’d prefer that it cut. That, too, is said to cause more breakage.
Our Case Western University has a “Maker’s Space” where teachers of Mechanical Engineering allow non-students to work on projects. Though they actually ran the metal CNC, I learned a lot of associated ideas. I now bolt a piece of Delrin to the table. After I surface the Delrin I use plastic bolts to secure the brass to it. Though that doesn’t rule out “chatter” from problems with rigidity, it ‘s the most secure work-holding I’ve seen.
- Leo
- Vectric Wizard
- Posts: 4356
- Joined: Sat Jul 14, 2007 3:02 am
- Model of CNC Machine: 1300 x 1300 x 254 Chinese Made
- Location: East Freetown, Ma.
- Contact:
Re: Feeds & Speed and Chip Load Explained
I am a manufacturing engineer that has worked in industry over 40 years cutting a lot of different metals. That being said, I will agree that it's not always about the calculations, though the logic of the calculations still do very much apply. You still need to get a decent ratio in order for the cutter to be able to do its job.
Carbide is very brittle and breaks very easily. The tiny pointy tips of carbide V cutters break so easily that just touching the surface of the material can break the tip. Rigidity of all of the setup it super critical. Holding that sheet material from moving is super critical. The onefinity is a really nice machine, but it's just not as rigid as a Mazak or other industrial machines.
I don't care much for the Amana single insert V cutter. I have one that I bought just to try it out. I also have several other Amana insert cutters that I bought to try. Also, I don't like Amana Feeds and Speeds at all.
I prefer the brazed V cutters. By brazed I mean that the carbide is brazed onto a steel substrate than sharpened. Brazed is more rigid than inserts. Even so - the tiny tips still break.
I mentioned the TBN because the tip is not a tiny sharp point that is easily broken. In industry we used a 1/32 ball nose end mill (not TBN) to engrave product information onto 17-4PH surgical stainless steel. That 17-4PH is hard to machine. We used industrial Matsuura machining centers. Pointy cutters just did not work. RPM 16,000 Feedrate 5 IMP Worked like a charm
Another choice is to use HSS rather than carbide. HSS is a lot tougher than carbide. Tougher is a specific term used in metals not just my choice of words. HSS can also be sharper. HSS is not as brittle at carbide. RPM requirements will be lower.
I have not done a lot of experimenting with the kind of cutting you are doing on sheet brass but I can see the value in working out that process. I do have some sheet brass. Unfortunately, I cannot get to experimenting for some time as I am very busy in my shop.
I don't know what you are trying to do, but considering a .5mm TBN may be a good choice, Yes the .5mm (.019") is bigger, but that is at a depth of .019" deep. At a depth of .012 deep it will be a little less. The plus is that the cutter is a lot stronger. EBAY "drillman1" sells the cutters a LOT less expensive than Amana or bits and bits and they perform well, I have used them on brass - not sure of the alloy as some of stock is scrap brass left over from manufacturing.
I am not sure but maybe a google search of .25mm TBN may show some results.
Carbide is very brittle and breaks very easily. The tiny pointy tips of carbide V cutters break so easily that just touching the surface of the material can break the tip. Rigidity of all of the setup it super critical. Holding that sheet material from moving is super critical. The onefinity is a really nice machine, but it's just not as rigid as a Mazak or other industrial machines.
I don't care much for the Amana single insert V cutter. I have one that I bought just to try it out. I also have several other Amana insert cutters that I bought to try. Also, I don't like Amana Feeds and Speeds at all.
I prefer the brazed V cutters. By brazed I mean that the carbide is brazed onto a steel substrate than sharpened. Brazed is more rigid than inserts. Even so - the tiny tips still break.
I mentioned the TBN because the tip is not a tiny sharp point that is easily broken. In industry we used a 1/32 ball nose end mill (not TBN) to engrave product information onto 17-4PH surgical stainless steel. That 17-4PH is hard to machine. We used industrial Matsuura machining centers. Pointy cutters just did not work. RPM 16,000 Feedrate 5 IMP Worked like a charm
Another choice is to use HSS rather than carbide. HSS is a lot tougher than carbide. Tougher is a specific term used in metals not just my choice of words. HSS can also be sharper. HSS is not as brittle at carbide. RPM requirements will be lower.
I have not done a lot of experimenting with the kind of cutting you are doing on sheet brass but I can see the value in working out that process. I do have some sheet brass. Unfortunately, I cannot get to experimenting for some time as I am very busy in my shop.
I don't know what you are trying to do, but considering a .5mm TBN may be a good choice, Yes the .5mm (.019") is bigger, but that is at a depth of .019" deep. At a depth of .012 deep it will be a little less. The plus is that the cutter is a lot stronger. EBAY "drillman1" sells the cutters a LOT less expensive than Amana or bits and bits and they perform well, I have used them on brass - not sure of the alloy as some of stock is scrap brass left over from manufacturing.
I am not sure but maybe a google search of .25mm TBN may show some results.
Imagine the Possibilities of a Creative mind, combined with the functionality of CNC
- Phil
- Vectric Wizard
- Posts: 3169
- Joined: Thu Nov 17, 2005 10:56 pm
- Location: Pittsfield, MA
Re: Feeds & Speed and Chip Load Explained
I have tried to find a source for HSS router bits. I have not been able to find one. Do you know of a source?
Phil
Phil
- Rcnewcomb
- Vectric Archimage
- Posts: 6379
- Joined: Fri Nov 04, 2005 5:54 am
- Model of CNC Machine: 24x36 GCnC/WinCNC with ATC
- Location: San Jose, California, USA
- Contact:
Re: Feeds & Speed and Chip Load Explained
- Randall Newcomb
10 fingers in, 10 fingers out, another good day in the shop
10 fingers in, 10 fingers out, another good day in the shop