Anybody spend the money to buy a Speeds & Feeds Calculator that takes the type of wood into account. There are such huge differences between the hardness of the different species that it wood seems to require one. There is one for sale on CNC Cookbook. Anyone have any experience with it?
Or is that a pipe dream? Maybe it’s not a calculator per say but a ‘multiplication factor’ of wood based on some standard.
Usually you can find recommended speeds and feeds for bits at the manufacturers website. Some even have tool databases of all their bits that you can import into your CAD/CAM software.
I have tried CNC Cookbook in the past but now I just use the manufacturers recommendation and adjust it if needed.
i have some SPE bits and their website has a downloadable tool database that goes directly into fusion 360. pretty awesome. pick the tool, the type of wood and it presets all the numbers based on their manufacture recommendations. has worked really well. that doesn’t mean i haven’t edited some of the numbers but their numbers have worked 95% of the time without any changes.
@Enginerd Chris, I’ve uploaded the Amana database and it’s a great place to start but it doesn’t take into account the type of wood.
@RockingMallet Joshua, thanks for the heads up. Funny, because I’ve used SPE tools a lot; cheap and easy to get on Amazon (which I hate to use so much but I’m not a patient person and returns are so damn easy…).
UPDATE: Tried it and it worked great. For example, one bit shows a feed rate of 54 ipm for hardwood, 90 ipm for softwood and 126 ipm for MDF/Laminate. The Amana database only has a default preset.
to keep on the feed/speed train with different bits, here is a link to Cody’s bits
https://www.cadencemfgdesign.com/feeds-and-speeds
can’t wait to get my kickstarter order hopefully in July - love seeing small business makers get support.
@RockingMallet Hey Joshua, thanks for that link. What I like about it is that it takes into account the depth of cut and the stepover as well.
Usual preface, I’m with PreciseBits so while I try to only post general information take everything I say with the understanding that I have a bias.
I’m not aware of a good one. The closest you’ll get for less than the cost of a kidney is Millalyzer (Link) and it doesn’t have a lot of woods or a way of dealing with most of the below.
There’s multiple issues with wood and correct chiploads (feed and speed). Since it’s a grown material it starts off variable and get more complicated from there. For a few common examples, woods cut differently with changes in grain structure, material integration, and moisture content. Some of those change it a lot like Rosewood or Ebony that integrates silica into the wood or very tight grained wood vs wide grain with the same hardness.
There’s also the issue that any calculator to have better than a quick “start here” number would need to know more about the tool than most ask for. Millalyzer is better at this as it’s looking for tool geometry like rake and helix. However, most don’t and even Millalyzer is missing a lot of them. There’s also an issue of getting those numbers as most manufacturers rarely if ever give them out.
In the same strain tool geometry will effect where your best cut will be as something like a tighter helix changes things like tear out chiploads, cutting forces, and what direction those forces are in.
There’s also other machine variables like runout that add and subtract from chipload (feed/speed) in multi flute cutters. Resonance and CNC/tool rigidity would be 2 other quick examples that can’t be completely accounted for in most of the calculators.
This functionally means that the only way to get “optimal” or the “best” settings is to test. Even big production shops with 6 figure machines do and only use calculators or manufacturer data as a starting point. I feel I should point out though that unless you are doing repeated cuts with the same tools and material or are on the margins of deflection/tool strength it may not be worth the time.
For the most part if you are using decent size and quality tools in soft material there’s a large range of “usable” chiploads. That’s not to say you can’t get better results digging into it but it’s more complicated than most assume. I feel it’s also worthwhile to learn a lot of these types of things to add to your troubleshooting and starting points. But not to the point of obsessing over the “optimal” vs cutting and making parts.
The closest you can get to this is Janka rating and only for like grain structure and integration. It’s a hardness rating created by measuring the amount of force it takes to embed a steel ball to a certain depth in the wood. Again though that’s, only one part of the wood variability. It can be useful if you have good data in a similar wood. You can use it as a ratio to your chipload/feed or pass depth. Won’t be ideal but it will get you a starting number that’s decent IF your original is good.
Be careful with these. There’s multiple issues but a quick summery would be that they are almost all making machine and material assumptions or giving conservative numbers. That not necessarily wrong, and to create a chart like this there’s not really a lot of options, it can lead to issues though. E.g. if they tested to get the numbers with an industrial machine those numbers will straight up break tools in a deflection limited system. The conservative ones, as long as they aren’t too conservative (rubbing) should be fine to use. You are probably leaving cut quality and tool life on the table but that may be worth the trade if you are doing one offs or short runs. Keep in mind that this will become less true as you get into larger tooling. There’s an assumption that as the tooling gets larger the machine gets more rigid. So you can get into areas where you’re machine limited even on the conservative numbers with larger tools.
Hope that’s useful. If anyone wants me to go more in depth on any of this let me know but I already am running into text wall territory.
Won’t go too much into this for bias reasons. However, I do like that they list chip thinning compensation for the listed stepovers. That will save a lot of people some headache.
We created CNCExplorer for this purpose. Select bit and material and you can optimize your feeds and speeds (including depth of cut). We hope to have an iPhone app out in the near future, but the web app is available now. https://www.cncexplorer.com
Happy answer any questions.
-Tom
@cyberreefguru Hey Tom, I’ll give it a try. It’s $14.99 and I’ll provide a review here for all who may want to consider it. It looks like it could have good information and, hell, I stood here and asked for it.
BTW, when you sign up for an account, the text I entered was white on a white background. Couldn’t see it at all. Should be a relatively easy change for you.
Hi Jim - it’s free for 30 or 60 days – don’t recall which. That lets you evaluate it without committing. We can probably arrange a discount code too 
WRT the text, I thought we fixed that bug! It’s browser dependent. Maybe we didn’t push it to prod – I will check.
-Tom
I already bought it at full price. Gawd, I’m such a sucker… I’ll let you know what I think.
I’m using Chrome on a pretty new MacBook Pro w/M1 Max processor; if that helps.
I made a video about this to help explain chip load a bit better in simpler terms. The main take away should be that testing for bit temperatures is the key to getting the perfect chip load. Pause the project a few min into the cut and see how hot the bit is. I use a thermal heat gun to shoot my bit temps. Make adjustments until you have the coolest temps and that will be the best chip load possible. Link to the video. Beginners Guide To Feeds Speeds & Chiploads - YouTube
@JDog Thanks for the excellent video. (One note: You kept saying “eighteen hundred RPM” instead of 18,000. But we know what you meant.). You don’t mention using a thermal heat gun in the video. That’s an infrared thermometer, I believe. What is the temperature range you’re seeing? What’s an ideal temp for a 1/4" two spiral upcut? (Just as an example.)
Thank you for bringing that to my attention… I did mess up where I said eighteen hundred rpm instead of 18,000. I need to add a note in that video about that correction.
Its hard to give specifics because these numbers are different with every wood type and every bit size and depending on what time of year it is. !/4EM DC in pine was around 140deg F when dialed in while the upcut would run slightly cooler at around 120deg F. but that was in the fall when my shop was not really hot. I would usually take whatever temp it gives me and make small adjustments to see if there are changes or improvements looking for the lowest numbers. Over time you start to get a sense of what it sounds like and looks like when it is dialed in and you will be able to adjust it without the aids.
Quick question on this subject.
do you use different settings when carving a 3D relief.
As opposed to flatwork like a sign.
an example is a 1/4 ballnose in maple.
I used to be particular about chip load etc but after burning out three Makitas in a year decided to use setups that are easy on the router.
I think that router bit longevity being shortened due to possible overheating is less expensive than replacing routers. So far have had no reason to change this after about 4 months of daily use.
I also have one of these mounted on a bench lathe, but it would be simple to put it on a drill press or hand drill. which I use to clean each bit when I change bits. Very quick and very inexpensive.
amazon.com/Jewelry-Polishing-Bristles-Polisher-Diameter/dp/B0B5QLVJT3/ref=sr_1_38?crid=U5OFE62M4Y4K&keywords=jewellers+bristle+brush&qid=1707684079&sprefix=jewellers+bristle+brush%2Caps%2C397&sr=8-38
Get a MakerMade router. You’ll be MUCH happier! And you’ll have an actual ER-11 collet then too.
Pony
@Pony
did that in December quite pleased so far.
In general, yes. This is due to most 3D work requiring stepovers of less than 10%. Any stepover that is less than 50% will have chip thinning which will make your actual chipload less than typically calculated. As an example let’s say that we are cutting with that 1/4" ball-nose (assuming a 2 flute) at 10KRPM with a 0.004" chipload. This would workout to 80IPM (RPM * Flutes * Chipload). However, let’s now say we are only using a 20% stepover. To cut that same 0.004" chipload we need to cut at 100IPM (1.25x). This gets worse the lower you go where 10% requires 133IPM (1.67X) and 8% where most will recommend a 3D finish pass is 147IPM (1.84x).
There’s also an issue of potentially needing a different chipload if the rake in the ball is not aggressive enough to match the side flutes of the cutter.
Unless there’s something I’m missing this doesn’t need to be an either or. Depending on where you are having issues (high RPM, or cutting force) you can change the cut to get both a decent chipload and something that the router can handle. e.g. Too much force cut the pass depth, too much RPM scale the RPM and feed.
While you can use heat as a sort of litmus test it’s not the most important part of hitting a minimum chipload. The real issue is that if you are not taking a large enough bite (chipload) you are not “cutting” but “rubbing” or “grinding” the material out of the way. Not only does this generate heat and reduce tool life but also increases the cutting forces (worse for the router) and produces a poor quality cut.
To be clear, I don’t know what you’re cutting at, your tool geometries, or materials so you may be hitting a minimum chipload.
Out of my own curiosity, have either of you measured the runout on these. There a few versions we’ve seen of these ER11 router and we can never seem to get any real data on them.
Hope that’s useful. Let me know if there’s something I can help with.
