Feeds & Speeds - Baltic Birch 3/4"

#1

Hi Everyone,

I’d like to get a sense of the capabilities of the Longmill for cutting 3/4" Baltic Birch, which is often used for shop projects, jigs and furniture making.

There are some Sienci published feeds and speeds available for wood here as a general starting reference: https://sienci.com/docs/longmill-benchtop-cnc/common-materials/wood/

General plywood is listed at 1200mm/min (~47 ipm), with a 250mm/min (~9.5 ipm) plunge rate, and a 3mm step down. These seem quite conservative to me (which makes sense), but are they?

FEED RATE

The loaded cutting speed I can’t really comment on as I haven’t used the machine yet, but I am hopeful it can go to at least twice that speed? 47 is on the slow side for sure. I saw the reference to the lead screws being a drag on overall speed due to the reduction factor they have, but I’m hopeful there is more juice available?

There are some interesting tid-bits in this older Wired article: https://www.wired.com/2012/10/you-suck-at-using-a-cnc-router/ But like all information on CNC feeds and speeds, I detect some comments that I’ve already experienced are incorrect. 80 ipm for Plywood can be far too slow on larger machines. I turn up my recent cut to 180 ipm before the chip load and sound was ideal. I have a feeling 80 might be more in line with what the Longmill could do and more appropriate for it’s design, but given that it’s almost double the listed speed (acknowledged as a conservative place to start), I’m curious if 80 ipm (2032mm/min) is possible on the Longmill?

STEP DOWN

The step down of 1/8" seems too shallow to me. I’m hopeful 3/8" would be feasible, and of course it have a dramatic affect on overall cut time. Why such a shallow step down? If doing carving or detailed 3D work I can see it, but for profile and pocketing or larger items it seems very shallow?

PLUNGE RATE

The plunge rate also seems a bit too conservative to me. That’s only .15 inches/second, which is far slower than I believe I plunge by hand without any issues. That’s just slightly more than 1/8"/second. Does that seem right given the rigidity of the Z-axis on the Longmill? Is it an issue of avoiding any flex and deflection?

-Jeff

#2

Hi @jwoody18 you’re spot on with your observations. When I was running the LongMill through baltic birch my speeds and depth were greater, however I don’t recall the settings I used; I’ll have to get back to you on that.

Our LongMill resources are still under construction, so those values have been copied over from the recommended speeds for an 1/8" end mill from our previous machine: the Mill One. We’re quite a small team with a lot of the focus on manufacturing and packing right now, but my priority in the next week and a half will be to bring a lot of new resources in and give y’all some more information to prepare for when the LongMills start to arrive.

If you have any feedback on other information you’d like to see coming from up, then let me know or shoot me a message :+1:

#3

That would be great. I think a 1/4" downcut or compression bit, doing profile cuts in 3/4" / 19mm (18mm I guess these days) baltic birch is a pretty good general use case for getting a handle on performance. I’ve not used a 3/8" bit in my Makita but it did come with that collet as well although I rarely see people mention it. Not sure how that might figure in to things, just mentioning it for posterity.

Understood, and please do prioritize the order fulfillment. I know people are anxious to get their machines.

Getting a sense of what your final rapids and plywood cutting speeds look like with a 1/4" bit would be great. And also any details on accuracy and repeatability that are dialed in. Will help with designs we work on while we wait for the machine to arrive. :slight_smile:
-Jeff

#4

I still have some project loaded into easel that I cut a ton of well maybe not a ton of birch ply but I think I can get the setting for you. BRB

Cut speed was 1524 mm or 60 in/min
Plunge Rate was 228.6 mm or 9 in/min
Depth per pass was 9.5 mm or .375 in or 3/8"
This was for my coffee coasters Chris so I think we got it nailed pretty good on that for max speeds and depth. I ran the router at about 3/4 speed I think for that. with a 1/4" Dn cut spiral bit

2 Likes
#5

I’ve been squirreling away bits and pcs for future reference which some of ye might find useful, well hopefully someone will.

Other valuable formulas:

Feed Rate = RPM x number of flutes x chip load

RPM = feed rate / (number of flutes x chipload)

Metric conversion: Divide inches per minute by 39.374 (example: 300 inches per minutes divided by 39.374 = 7.62 metres per minute)

RPM Selection

The general operating RPM for tooling contained on this site is between 10,000 and 20,000 revolutions per minute. Usually, the higher the RPM, the better the surface finish becomes. However, the higher the RPM, the higher the friction generated between the tool and the workpiece. This friction is what creates the mechanical wear on the cutting edge. Your goal is to select the lowest RPM possible for each application.

Calculating CNC Router Tool Feed Rates

The chip load is a measurement of the thickness of material removed by each cutting edge during a cut. This is a valuable piece of information that can then be used to calculate new set ups.

Chip loads are based on material thickness of average size for cutting edge length of tool. The calculation below does not apply to thicker material or tools with long cutting edge lengths. These feed rates are only a recommended starting point and may not accommodate all circumstances. Therefore, tooling damage may still occur and use of this calculator does not provide any warranty against tool breakage.

RPM Selection

The general operating RPM for tooling contained on this site is between 10,000 and 20,000 revolutions per minute. Usually, the higher the RPM, the better the surface finish becomes. However, the higher the RPM, the higher the friction generated between the tool and the workpiece. This friction is what creates the mechanical wear on the cutting edge. Your goal is to select the lowest RPM possible for each application.

The chip load is a measurement of the thickness of material removed by each cutting edge during a cut. This is a valuable piece of information that can then be used to calculate new set ups. Calculation are as follows: Chip Load = Feed Rate (inches per minute) / (RPM x number of flutes). Example: Chip Load = 500 inches per minutes / (15,000 RPM x 2 flutes) Chip Load = .017".
Chip loads are based on material thickness of average size for cutting edge length of tool. These recommendations do not apply to thicker material or tools with long cutting-edge lengths. These chiploads are only a recommended starting point and may not accommodate all circumstances.

Cheers

1 Like
#7

Greg,

Thanks again for posting these details about baltic birch.

I was intrigued when I saw over on the Facebook group that early pickup user Jeff Richardson posted about doing V-bit and straight bit 1/4" cuts at 100 inches per minute and a plunge of 30 inches per minute, with a cut depth of 1/8". His material was different, of course, but I was encouraged to see 100 ipm mentioned as I hadn’t seen any reference to going that fast before.

I’m not a Facebook user, but thankfully can still read over there. Any chance you could try and encourage Jeff Richardson to pop over this way and share some of his cutting settings with us. I saw you mention that Andy said your machine is a bit slower due to being a beta configuration, it would be good to see if we can collect some feeds & speeds info from folks with the production units too.

Thanks,

-Jeff

1 Like
#8

While I am certainly no expert on speeds and feeds I did spend a number of years calculating them for machining metals. In my experience these calculations are a simple starting point. I tend to rely more on the sound of the machine and the finish on the material.

I try to keep my chip load between .002 and .004 depending on the material. I also limit my depth of cut to half the diameter of the cutter to be on the safe side with a plunge rate of about 30% of my feed rate. These are not commercial production machines so you can’t run them at the bit manufacturers feed rate but you can certainly run faster than the very conservative feed rates calculated using easel or carbide create.

So I use the simple chip load formula noted above, chip load = feed rate / (rpm x # of flutes). My spindle sipped is 17,000 so the denominator is 34,000.

For a 1/4 inch two flute cutter I run at 100 inches per minute in Baltic birch which gives a chip load of 0.0029. I run the same cutter at 85 inches per minute in white ash which gives a chip load of 0.0025. At these feed rates the machine sounds good and I am happy with the finish. The math says I can go faster but as I said earlier these are not production machines and I don’t do production runs.

For a 1/2 inch ball nose I run at 75 IPM with a 10% step over for white ash and 85 IPM in bamboo.

The reality is there is no magic number for speeds and feeds. You have to run your machine at feed rates that YOU are comfortable with.

If you are looking for a good source for chip load charts Amana tools publishes this data for every tool they make but please keep in mind these feeds are for commercial machines. For example they suggest running a 1/4 two flute bit at 180 IPM with a 0.005 chip load and a plunge rate of 90 IPM with the depth of cut at .250. In my opinion you would be crazy to run the LongMill at these rates.

Hope this helps.

Jeff

2 Likes
#9

Thanks Jeff. Definitely a good starting point. I’m with you about learning to “listen” to your machine. Many times you can tell something is not quite right by the sounds it makes. I also like your numbers. They make good sense to me and should to others. And welcome to the forum.

#10

What kid of machine though @JRich63? If your cutting on a big industrial machine you can’t use those numbers on a long mill. The numbers are not comparable. Amana tooling is way different and should be a ball park only.

One rule of thumb for conservative cutting set your depth and half the diameter of the bit. So for a 1/4" up cut end mill 1/8th you will be way safe. Read what I put a 1/4" DC through in my previous post on a Beta Longmill! that is a better guide for you @Heyward43

#11

Hi Greg, based on your comments I am not sure you actually read my post as I talked about being conservative and running at a speed you are comfortable with and I am sure I stated that you would be crazy to run the LongMill at the Amana feed rates. However, in my humble opinion the Amana tooling data is a good place to get cutter chip load data to assist in helping to determine that you are running within the parameters of the tool.

1 Like
#12

I skimmed over it I am not sure I didnt look just cautioning about not using industrial settings thats all.

#13

I am curious what constitutes an upper limit for performance on these machines.

I agree with you, sound is key for every cut and you can’t assume a given type of workpiece of the same material, will perform optimally just because you use identical settings, although it’s a great starting point. :slight_smile:

Lots of people are discounting what the Longmill can do, out of the gate. While I totally agree with having reasonable expectations given the price point and construction parameters of the machine I am interested to see what exactly it can do. If @andy and @chrismakesstuff have done performance validation work to explore where the upper limits of the machine are, they haven’t shared it and I don’t blame them. Better not to make promises or create liability at this point.

One of the things I’ve read repeatedly while learning about CNC over the last year or so is that it can be a mistake to limit cutter engagement too much and you will likely end up wearing the bits faster. Finding the right balance is key. Spindle power and deflection considerations, at high load especially, are definitely going to restrict the Longmill (or any unit using a consumer router as a spindle) as will overall rigidity - but I can’t help thinking there is a wider performance envelope to explore with the Longmill.

Having seen other machines with consumer routers cutting at 150 or 200 ipm I suspect the Longmill could potentially do the same. Speed isn’t everything, of course, quality of cut is often the key goal. I just wanted to raise a contrarian voice and say that until more machines are in circulation and some adventurous users push them a bit harder, we shouldn’t assume the Longmill can’t perform at higher feeds and speeds and still deliver stable, reliable cuts. It’s simply an unknown to be explored.

Often times turning up the speed or feed rate a bit can actually improve the cut. It is a very satisfying feeling to adjust feeds and speeds and suddenly see near perfect chips coming off a cut. There is definitely a sweet spot. Of course starting conservative for safety and machine protection makes sense, but my research suggests (for CNC in general) being a bit more aggressive in small steps and listening and observing can result in higher overall quality and performance.

I’ll be very interested to see how things progress over the coming months and how people enhance their machines as well.
-Jeff

1 Like
#14

Andy ran the one mountain cutting rough cut job at about 4000 mm per minute with a 1/8th end mill I think. Was crazy fast but he wanted to test to see how far he could push it. I would not go that fast out of fear of breaking the bits. Only thing I can tell you is what a much more experienced cnc fellow said in one of his videos if your breaking bits your going too fast. Why run a job so fast your ruining tooling? That costs money and I for one am not rich and don’t like breaking stuff. Though I have broke my fair share. Will I continue to? No I have learned along the way. Make sure you do certain things. Like returning to 0 so you don’t run your bit across a sheet of plywood and shatter the bit on a screw. Plus ruin the whole sheet of work.

Its easy for us to sit back and tell you do this and do that. You have to figure out certain things as you go too. What you are comfortable doing someone else may not be. Its a personal choice.

Im not discounting this machine on anything. I have used it over a year. I know what it can do. Trust me I have pushed it. Some things just have to be figured out for yourself. You will figure out and quick if you have a 1/8th endmill you sure has heck will not be plowing through hard wood at 4000 mm a minute. You will have metal shards everywhere.

#15

One other tip. Just because a 1/4" up or dc endmill will plow through baltic birch plywood at a fast rate. How long do you want it to last? If you push it you might get two 30 X 30 sheets of plywood cut out and the bit could be burned up on you. Yes they are carbide but even that will only stand up to so much heat. Run it slower and you will make your bits last longer too. Everyone says they want to run their machine and push it. But its not practical from a wear and tear point of view or loss of tooling point of view. In fact its foolish.

1 Like