Hi Mel - welcome to the forums. Generally speaking, if your depth of cut is 50% the diameter of your bit, 40-60ipm will work fine (e.g., you are ‘safe’). You can go faster - you don’t have to.
Make sense?
-Tom
1 Like
The speed of your cut is determined by the size of your bit, the rpm of the router, and the material you are cutting.
Use a chart to determine proper starting settings and set the machine there.
The only reason to change these settings is to either get a better finish by making small changes to stepover or doc. or to adjust for really dense material.
Running the machine too slow causes friction on the bit and wears it out faster.
You should always look at a chart and then keep your own data as you make adjustments.
I would not recommend running your machine much slower than what the bit manufacture recommends.
Feed rate is essentially controlled by chip load, number of flutes, and bit diameter. That doesn’t mean the cut is optimal. If we just used the formula you could cut at any depth on any material and get the same results - we all know that isn’t true. I agree using a chart helps, but the chart needs to be matched to the machine. Most manufacturer recommendations are based on super robust commercial grade machines, not hobbyist machines. The OF is certainly on the upper tier of ‘hobbyist’, but it is not a Tormach or Laguna. 0.02.
-Tom
1 Like
Those machines are capable of pushing bigger bits than 1/4 and that argument is very true but in this application with 1/4 size bit or smaller I think most manufacturer settings can be more than achieved. Grab anything bigger than 1/4 including a surfacing bit and you will quickly see the limitations of our machines. Sine this forum consists of mostly users of the same machine I think all our experience with the machine should be shared openly so no one is confused about how to operate their machine on a day to day basis.
@jdog - I completely agree. But I also recommend starting slower to learn the ropes 
I’ve snapped more bits with the OF than my previous SO2 or X-Carve in 7 years, so yeah, the machine is certainly capable (and I’ve gotten lazy with double checking everything before clicking start).
-Tom
That’s just it Tom starting slow is bad advice because running your bit slow will dull or break your bits. Most bits that snap are because of too much heat in the bit. This is caused by going slow which is why its bad advice. This video from Cutting it close may help.
2 Likes
Hi all!
I am very new (2weeks) into the CNC world. Thanks for the great info on feeds and speeds. Particularly that most charts are stated for 100% bit diameter as the DOC.
One thing I don’t hear much about while reading about F&S is step over. Is there a “rule” for setting step over?
Thanks again for all the great information!
@jdog - I agree with your recommendations, and to be clear, I’m not recommending blindly going slowly without regard to the material and bit. My point is there is healthy range for an ‘optimum’ cut. I believe new users should start on the low end. Mistake #6 in the video, understanding your machine’s capabilities, is really important in this regard. My speeds and feeds today would cause nothing but belt slipping on my X-Carve. Hope that makes sense.
Eric - step over is really only key for pocketing and 3d clearing (which is sort of pocketing). You usually don’t want to do 100% step over as you will have material left behind. I generally use 40-60% depending on the cut; for a face operation I do use 95% through. YMMV.
-Tom
1 Like
100% Thank you for helping clarify those points with me for the new guys. We both want everyone to have a great experience and get the best performance from their machine.
Stepover only really matters after the first pass because the first pass is always 100% engaged in the material. The speeds and feeds are set for the first pass so it will handle the full engagement. The second pass only takes a percent of the bit as it steps over so only that portion is engaged in the wood at that point.
I just wanted to update some progress we are making on the new CNC Explorer App. We have added a new feature that calculates the required milling forces for a given cutting setup. We have a machine model for the OF that right now has an estimated max force of 35-foot lb. What does this mean? Well as people use larger big diameters and try to push their machines the required forces can exceed the capability of the machine. We are very lucky to have a very strong and rigid tool at our disposal but it does have its limits. Using this new feature will help gauge how close you are to your machine limits and give one more tool to help you optimize your cuts.
Demo LInk: cnc_explorer
1 Like
We should remember feed rate is a direct ratio of Spindle RPM. Slower feed rates require slower RPM. Granted a router like the Makita only has limited speeds available but there are still choices that can be made. I think the choice of depth of cut is probably even more helpful for the beginner. Shallow cuts at a proper feeds and speeds are very helpful while learning good work clamping techniques for example. While it will take longer for a job to finish it will be more likely to complete without fault.
This says for a 1/4 downcut endmill that my feed rate is 34ipm. I think either it is missing a factor in the calculation or I do not understand how to make it work. . 34ipm is way too slow. I am running the 1/4 at 340ipm.
I believe its the chipload. For hardwoods like the oak the one i selected the chip load should be .009-.011
Jdog, Thank you for giving our app a look. Firstly you have a 45415 bit selected which only has a recommended chip load of 1.7 mils. Cutting at 340 ipm @ 17000 RPM would require a chip load of 10 mils Chipload Calculator | GDP Tooling There are bits designed for that chip load but most are much lower. The Amana 46399-K is designed for 5 mils. With that bit, our App is going to recommend 102 ipm for example
An advanced skill level person can push the settings. If you register for the demo version you will be able to click on the Show Expanded and can increase the calculated bit chip load. In your profile - settings you can select the “Advanced” skill level. Now if you go back to the home screen and click “Show Expanded” on top you will see a Chip Load Fine Adjust Slider. As an Advanced Skill user, you can adjust the cutting chip load +/- 5 mils. With your understanding that pushing a bit might reduce its quality of cut and put increased stress and deflections you can increase your feed rates. I would rather you maximize your RPM first.
A cool feature is that once you have dialed in a particular setup you can create a named recipe and save it off for future reference. The intent of the app is not to limit you but to help you be more aware of all the parameters that go into a particular feed and speeds setup
At the default configuration, our App will be very conservative. As a user gains experience and knowledge the more advanced features can be used to push the boundaries.
I hope that helps clarify.
1 Like
Jdog, I just checked the Amana feeds and speeds for the 45415, and yes there is an error and the chip load should be 5 mils. We are using Amana’s published database and I will check where the error is.
Who you going to trust Amana or Amana? In their own tool database they have the bit at 1.7 mils but their own speeds and feeds data sheets its 5 mils for wood? Thanks for pointing the error out for us. I guess I will have to ask Amana for the correct answer. I suspect its probably 5mils.
Okay thanks for the clarification. I can see how this would be a benefit once its dialed in with the ability to save recipes. I would say at first look it seemed very very conservative for the 1F in its initial settings, from what I am running the machine at.
FYI - just saw a simple calculator on the sainsmart site. I don’t know if it’s any good since I’m still waiting for my 1F to arrive. Just throwing it out there as a resource.
@JDog I’m trying to adjust my stepover and for the life of me I don’t know where the setting can be found on the OF. Can you tell me where it is… I do appreciate it.
