Newbie Wondering about Spindle RPM

HI,

Long time woodworker and new to CNC. I have a baby CNC, the Shapeoko 3 with a Makita trim router. I'm curious about the RPM that software suggests.

The RPM suggestion that Carbide Create and Fusion 360 give me, seem very low.. Example, I am cutting 3/4 plywood just for some testing and it says to use 6,000 RPM? I tried this and it was just way too slow and seemed to really struggle. I have been sticking with the suggested feeds and speeds, but use around 27000RPM and it has been working fine.

Does anyone know why these suggestions are so low?

Thanks.

What's the tooling?

In this example I was using a 1/8 2 flute end mill, but anything I have used it suggests very low RPM.

I cut with a 1/8" two-flute upcut or downcut bit at 18k rpm in all woods, from Baltic Birch to Walnut to Ebony to East Indian Rosewood - works just fine. Matter of fact, I cut nearly everything at 18k rpm and it works for me. I ignore the speeds Fusion 360 gives me. Those might be for metal instead of wood but I'm not sure.

David

The low rpm is suggested because your machine cannot move (“feed”) fast enough to utilize that high of rpms. Look at the “chips” after cutting. Are you getting dust/powder or actual chips? Should be chips and if you feel them right after a cut they should be warm. Your bit should be relatively cool after it stops (definitely touchable). On my machine, cutting around 200-250 ipm, I am usually only around 12000 rpm when cutting wood.

Richard's comment strikes at the heart of things...it's all about chip load, which is technically a math problem. Spindle RPM is only one factor relative to achieving ideal (or at least best obtainable) chip load. The ability to move the cutter through the material by the physical structure of the specific CNC machine also enters into the equation. (literally)

That said, the Shapeoko isn't any kind of slouch within it's class of machine and I've seen Winston Moy on YouTube get his moving pretty quickly and generates some pretty impressive cutting. (You should watch his videos if you get a chance)

By the way, both Fusion 360 and Carbide Create, are not performing any calculation about Chip load. Both have tool libraries pre-populated with feed/speed and until you change the numbers associated with the tool, you will always see the same numbers. You are free to change them and save your new values. The ones in carbide create may date back to Shapeoko 1/2 days, which were less stiff than your Shapeoko 3.
Fusion 360 can do the calculations in the CAM module, but are mostly geared to metal machining and are based around SFM (surface feet per minute) that isn’t as commonly used in the router world (but can be equated to chipload). In the first tab of a toolpath, you can see “Feed per tooth” which is the definition of chipload. The numbers in the table are interactive, and are recalculated as you change one.
Attachment 391050

You will need to manually go back and update the numbers in the tool table however. The ones calculated are only stored in the particular toolpath you are working on, although there is a similar interactive calculation function in the tool library (feeds and speeds tab). Change them once and that is the default for the next use of that tool.

I'd agree that you probably need to make sure you have accurate information in your tool library for your particular tooling and its optimal chip load. No idea but you may just be relying on a default chipload setting in your software that is likely not matched to your specific tooling.

We dont run fusion much or carbide create but I dont think they have any way of knowing how fast your machine can move or how robust it is but I would agree with Jim. Just do the math for your tooling and then you will have to find the sweet spot for your machines feed speeds and spindle power. I would guess the trim routers horsepower is going to be your limiting factor but cant imagine it ever running that slow.

Optimizing your feeds is something you can do just once and save it in your library and you should be running as fast as you can and as clean as you can. Id guess you'll be in a .003-.005. The by-the-book would be something like 18K RPM, .004" chip load (average), would give you 144ipm feed rate at 1xD depth of cut.

I will emphasize that adjusting the feeds/speeds values in the tool library of whatever software you choose to use is a very normal thing. I've been doing that constantly as I get to know my machine a lot better for both specific tools and specific materials. This includes spindle speed, both horizontal and vertical feed rates and maximum depth of cut per pass. This is a really good "experimentation" exercise, quite frankly, and you'll learn a lot from it which will help immensely with "real projects" over time.

Quote:

---

Originally Posted by Jim Becker

I will emphasize that adjusting the feeds/speeds values in the tool library of whatever software you choose to use is a very normal thing.

---

Agreed. We have in our library several duplicates of the same tool with different values assigned. So we may have a tool geometry tagged as "ply", then the same tool tagged as "hard maple", same tool tagged as "hardwood", plastics, and so on. That way when you tool path a given job there is no referring to notes or having to setup the feeds, rpms, plunge, and so on, over and over again. A given tool may just sit in a position in the rack but have 5-10 different itterations of that one tool in the tool library.

Yes, that's what I've been doing, Mark...some of my tools have multiple iterations for specific purposes and I choose what the appropriate "version" is when I'm coding the toolpath. They have the same "Tool Number" to avoid conflicts with that. For example, my .125 Ball Nose has three entries: one for wood; one for HDU and one (primarily for HDU) that has custom settings to support the textured pocket technique that I learned from Rodger. I do sometime adjust a tool within the toolpath after selecting it if I want to make a non-permanent change, too.

Absolutely. Super smart. I have been working hard lately at that overall concept in a lot of areas. Toolpathing, multiple post processors, and so on. It makes running a wide array of work a lot more efficient.

I have always thought the multiple tool options for the same tool would be something completely in your wheelhouse with the Corian work and so on.

David will figure it out Im sure and if not hopefully he posts a bit more or messages someone privately. Working out all these little kinks are I think what Brad was pointing to with his webinar thread. Unfortunately in today world of "free" its hard.

I have watched a few winston moy videos but not enough to follow him. I need to revisit that.

Thanks everyone! I am very new to CNC and have only used 2 cutters (1/8 and 1/4 flat end mill) so far. It seems to me like the Shapeoko can definitely take on more than the feeds and speeds suggested by the software. I have been using G-Wizard to help me get close to the right combo of speeds and feeds and it seems to be working well.

I don't like the software that came with the Shapeoko (Carbide Create), it seems very simplistic, even for a newbie. I have been using Fusion 360 to design and Carbide Motion to run the job.

Thanks again for all of your help!

Quote:

---

Originally Posted by David Justice

Thanks everyone! I am very new to CNC and have only used 2 cutters (1/8 and 1/4 flat end mill) so far. It seems to me like the Shapeoko can definitely take on more than the feeds and speeds suggested by the software. I have been using G-Wizard to help me get close to the right combo of speeds and feeds and it seems to be working well.

I don't like the software that came with the Shapeoko (Carbide Create), it seems very simplistic, even for a newbie. I have been using Fusion 360 to design and Carbide Motion to run the job.

Thanks again for all of your help!

---

Ill bet if you look around as Jim mentioned, machine specific forums or youtube channels, you'll see that you can push your machine quite a bit harder as I can only guess many machines at that level are set quite conservatively with the notion that they are often times going to new users.

You might try delving into GWizard from CNC Cookbook. They have software that figures out all that stuff for you. It is pretty interesting reading IMO. You can use their software for free for 30 days. I'm about halfway into my use and will probably pony up at the conclusion of my freebie period.