After working on the CnC for quite a while now, I have been feeling that I can push the limits a bit now. I am going to do a carve in solid Cherry which I have used many times before. The size is 25" Long 11.5" wide and 1.75" thick. I will be using a 3-flute 1/4" endmill and a 1/4" shank tapered ball nose with 1/16" Diameter tip. Nice and strong. I have usually used a feed of about 118" per min (3000mm) for the end mill and 130" /min for the tapered ball nose. Works great but takes a while. After watching some videos many are pushing the feed to 200" /min for the endmill and 250"/ min for the taper. Some have said this is about as fast as they normally go. Of course all manufactureās recommendations seem to be extremally conservative. If I do push it, it would take me three hours for the full carve vs seven hours normally. Does anyone here go faster?
Usual preface, Iām with PreciseBits. So while I try to only post general information take everything I say with the understanding that I have a bias.
Itās hard to say anything about those as what really matters is chipload not feed. For chipload you also need to know RPM and the number of flute.
That being said letās assume 800 SFM (~12,000 RPM) and that both are a 3 flute. For 200 IPM what that would work out to is a chipload of 0.0056". Thatās not even close to the limit of any decent tool in those sizes. We regularly push tooling of that type well over double that. The other catch to it though is that part of that will depend on the tool geometry (rake, helix, edge radius, relief). If itās not a good match for the material (e.g. a metal cutter), than you will run into an issue where the tool actually want to run faster but the material will fail at the higher cutting forces (chipload/feed).
Another thing to consider in this is that in most cases people using tapered ball-nose tooling are doing 3d relief work. The max stepover for a smooth finish in that is 10%. Although you are better off at 8% to account for errors. The issue there is something called chip thinning. Basically it means that you are not cutting as fast as you think you are if your stepover is less than 50%:
So for a 10% stepover you have to cut ~1.67x normal feed to hit the chipload. For an 8% stepover you have to cut ~1.84x . Or another way of putting this is if you were to cut with an 8% stepover, at 250 IPM, you would functionally be cutting at 136 IPM.
Hope thatās useful. If you want more specifics let me know the other parameters (RPM, flute count for tapered tool) and specific cutters you are using and Iāll do my best. Or if you want something above explained on, also let me know.
This is a great response thank you. One thing I havenāt considered was this calculation while looking at other peoples videos. They rarely talk about their stepover just their IPM. I kind of felt the hardness of the material itself was more important (ex. Pine vs Oak). But chipload is a great core starting point. I will be running a serious test today or tomorrow at 10% stepover for the 2 flute taper at 250 IPM and see if the taper breaks or if there will be even more room to increase. But your comment will help me to gain more precision in regards to dialing in my max speed. Kudos
No problem.
This will make a difference in the cutting forces produced. However, there more there than just the hardness. As an example pine can range from the mid 300s to as high as over 1200 lbf depending on the species (Janka hardness). If we use something like loblolly pine itās 760 lbf. But it wonāt cut as well as say basswood with only 410 lbf. The reason for this is the grain structure of the wood. You can basically think of it as the difference in how hard it is to separate and shear the grain vs compressing the grain. You also have things like rosewood where the tree integrates silica into the wood. That makes it much harder to cut than the pure hardness would indicate.
In this same vein keep in mind that cutting forces are produced by the cubic material removed per flute per rotation (per flute MRR). So the best thing to do testing wise is to test with a very low pass depth to determine what the tool and material combination can cut. Then start using the good cutting section in another test where you increase the pass depth. That will then tell you where you reach a limit of deflection (bending) in either the tool or machine.
With the above you do run into another variable which is the engagement time of the flute or multiple flute engagements. Those are typically not as critical though other than that slotting (100% stepover) is by far the worst as you are effected by both sides of the cut (climb and conventional) at the same time.
If possible measure the moisture content of the wood. More moisture makes the wood āstickyā. It changes the ideal surface speed/chipload (feed) and will not cut as well.
One other thing. Watch your RPM. A lot of what you can run a given tool with a good cut at depends on the geometry and thatās a whole other rabbit hole. However, itās much more subtle when you are exceeding the surface speed (SFM) in wood. It WILL effect the cut quality and tool life though. I talk some about it here:
Thatās in metal but the same applies. Without knowing the tool you are probably okay with 800 SFM for all but straight metal cutters. 1200+ for mix geometry and WAY higher for application specific depending on what they are targeting. To get a RPM from SFM (3.82 * SFM) / Diameter. So for 800 SFM on a 1/4" tool (3.82 * 800) / 0.25 or 12,224 RPM. You should also bias this by the wood hardness with softer woods being able to take higher surface speedsā¦ Assuming at least similar grain structure and mineral integration.
Iām just putting this here in case anyone else was confused about SFM. Iāve seen tons of feed rate stuff but hadnāt heard much about SFM until recently. Square Feet Minute was what popped in my head but that didnāt seem right!?!
What is SFM in Machining
SFM (Surface Feet per Minute) is the key parameter measuring cutting tool speed in CNC operations. It represents the linear distance (in feet) a toolās cutting edge travels across the workpiece surface per minute. Unlike RPM, SFM accounts for both spindle speed and tool diameter, making it the true indicator of cutting action intensity.
That was new to me too. But @TDA did make good sense of it. Loving this thread and thank you @_Michael .
Sorry, probably both my fault. Surface speed is the universal term for it. Itās more or less how quickly the edge is moving across the material. Some like to think of it this way. Although, not completely accurate it demonstrates the point:
- If you imagine that you have a block of wood in front of you and a flat blade the distance you move that blade across the surface of the wood in a minute is the surface speed. So if you were to just rub that blade across the surface without cutting any material that would be like spinning a tool in the material without any feed. If you add chipload (feed), that would be like pushing that flat blade into the material as deep as your chipload and then dragging it across the surface at that same rate (for the same surface speed).
You obviously have other things (like you are not taking one continuous chip) and that example doesnāt perfectly represent whatās happening in milling. But it gives a decent idea of things like depending on what the material that blade is against how much friction itās going to produce. Or even at a given depth, that thereās a big difference in how the material or edge will react to the speed. e.g. you can cut by hand a material with a very thin blade slowly but break it if you try to cut it too fast. Or with a very strong thick blade you can carefully remove some soft material. But if you go too fast that will splinter or deform the material.
Maybe that helps some?
No problems, I also ran across SFM when I went looking for info on steel in a recent thread. They also gave the formula you mentioned to convert to RPM. It was after thinking about the numbers a bit that I realized it couldnāt be square feet. The numbers were too large for that so I went searching.
I appreciate the detail that you put into your posts. I can look up the stuff I know I donāt know but it takes someone with deeper knowledge of a subject than me to discover the things I didnāt know I didnāt know! If that makes sense.