Basic F&S/DOC/WOC recommendations

[adcostanza (Adam)]

Hi folks,

I have a newly assembled Shapeoko Pro XXL and have been having a great time with it so far but there is certainly a lot to learn. I have a lot of CAD experience but much less CAM, so an obvious way for me to create my 3D designs is to get better at the CAM piece. I am using Fusion 360 and have found a ton of great information online that I have been digesting. In particular, the Shapeoko CNC A to Z ebook has been super helpful. I’ve been using the simplified feeds & speeds calculator from the ebook as well as checking out gmack’s more complex calculator(s).

I am just trying to cut something rather simple, some construction 2x4s that are whitewood, just for practice.

When thinking through adaptive clearing, something I find a bit confusing is that the simplified calculator recommends 100% → 300% of diameter as DOC for roughing. Looking through the forum though I’ve seen people mention that Shapeoko actually prefers less deep cuts with a larger WOC engagement.

The 2019-09-16 SFPF Workbook specifies explicitly to use 100% of diameter for adaptive clearing and 20% width of cut. Then there is also the AC Router SFPF Workbook Ver.1.1 (2020-04-11) that doesn’t actually specify adaptive clearing recommendations at all.

It’s also a bit unclear to me what a typical range of desired feedrate really is for the Shapeoko Pro. I see it can go up to 200ipm, but what is a sweet zone? After some searching I’ve seen some people mention (not specifically for the Pro) that if you can get up to 2000mm/min (78ipm) that you should probably increase engagement, which seems strange as 78ipm seems kind of slow relative to the max possible 200ipm.

So to that end, my very basic questions I hope you can help me understand are:

For adaptive clearing, what would be your recommendations for the following:

DOC/WOC % for adaptive clearing roughing
DOC/WOC % for finishing contours
DOC/WOC % for finishing pockets
DOC/WOC % for finishing surfaces
Recommended feedrate range for Shapeoko Pro (i.e. 90ipm → 160ipm)?
Does a chipload of 0.001" cause risk of rubbing or is it a decent safe zone?
Max machine force for Shapeoko Pro, is it 18lbf?

If I try to be a bit intuitive about it, I would think finishing a contour you’d want to go with the narrow and deep approach since you are just skimming off a small amount radially. When finishing a face or a pocket I would think you’d want to go shallow and wide, since you are cutting just a small amount of material axially. With roughing, I would expect you want to go deep and narrow based on the ebook suggestions but it seems like you really can’t go as aggressive as 300% diameter for DOC. Is 100% DOC a good sweet zone as specified by the more complex ebook?

Last piece, what % of maximum force and power is recommended when using gmack’s ebook(s)? The cells turn different colors, but it’s unclear if “yellow” is actually ok or if everything should be completely green.

Thanks in advance, sorry for all of the questions! I promise to post some cool stuff once I can figure out this whole Fusion CAM / Speeds & Feeds stuff better

[Julien]

Hi Adam, welcome to the community !

@adcostanza

When thinking through adaptive clearing, something I find a bit confusing is that the simplified calculator recommends 100% → 300% of diameter as DOC for roughing. Looking through the forum though I’ve seen people mention that Shapeoko actually prefers less deep cuts with a larger WOC engagement.

It’s a matter of preference. The feeds and speeds will be limited by the fight between the cutting forces and the intrinsic machine rigidity (and to a much lesser extent by the router/spindle power, 99.9% of the time it’s not the case). You can choose to “spend” that amount of cutting force either some “shallow & wide” cuts with a large radial engagement but limited depth per pass, or in a “deep and narrow” cut with large axial engagement but (very) limited radial engagement. Yes the shapeoko likes shallow & wide better, but…

• folks who figured this out mostly cut metals, where rigidity is everything. In wood, no so much.
• it all depends on the amount of radial engagement when cutting deep. There is a point where cutting deep but with a very small stepover will actually put less forces on the tool/machine than slotting at a small depth per pass.
• and then there is the psychological effect that lead me to investigate deep & narrow cuts: I just felt bad only ever using the last 1mm of my endmills, when I paid for 1/2" cutting length That, and deep adaptive is way fun

So, the 100-300% DOC only makes sense for very small stepover (optimal load) values, AND using helix ramping into the material, such that the tool engagement even at that 300% DOC is always small.

The rules of thumb mentioned in the ebook are an attempt to capture what came out of the community discussions on the matter, as well my own experience, so do take it with a grain of salt, a healthy dose of skepticism is always a good thing.

@adcostanza

It’s also a bit unclear to me what a typical range of desired feedrate really is for the Shapeoko Pro. I see it can go up to 200ipm, but what is a sweet zone? After some searching I’ve seen some people mention (not specifically for the Pro) that if you can get up to 2000mm/min (78ipm) that you should probably increase engagement, which seems strange as 78ipm seems kind of slow relative to the max possible 200ipm.

Feedrate is derived from RPM and desired chipload, bar none. There is no “desired feedrate” for the SO Pro because it depends on many factors (tool, RPM, material). What does scale with the rigidity of the machine is desirable depth per pass. I wrote the ebook based on Shapeoko3 experience, the Pro did not exist back then. I would guesstimate that you can easily double the recommended depth per pass (for “shallow and wide”) value compared to the SO3.

@adcostanza

I’ve seen some people mention (not specifically for the Pro) that if you can get up to 2000mm/min (78ipm) that you should probably increase engagement, which seems strange as 78ipm seems kind of slow relative to the max possible 200ipm.

Strange. Again the feedrate is the outcome of everything else, not an input. And one can most definitely run the machine at 200ipm when the tool/material calls for it (hint: plastics! they need large chiploads i.e. large feedrates)

@adcostanza

DOC/WOC % for adaptive clearing roughing

I don’t have a better recommendation than the one in the ebook, in the sense that I use them and they work great for me. YMMV.

@adcostanza

DOC/WOC % for finishing contours

It’s typically a good idea to shave off the remaining material at full depth, to avoid tool marks.
THAT IS, if you had a roughing pass before that that only left very little stock.

@adcostanza

DOC/WOC % for finishing pockets

Rough with some axial stock to leave, then to a finish pass at full depth that will shave off what little material remains on the bottom of the pocket, for a clean surface.

@adcostanza

Does a chipload of 0.001" cause risk of rubbing or is it a decent safe zone?

It’s the universal golden value that good for almost everything as a starting point. You can do more when the tool/material allows, but don’t do much less.

@adcostanza

Max machine force for Shapeoko Pro, is it 18lbf?

I think someone confirmed that yes, indeed.

@adcostanza

Last piece, what % of maximum force and power is recommended when using gmack’s ebook(s)?

If you come e.g. near 80-90% of max spindle power, you are probably already in a very challenging cut that pushes the rest of the machine to its limits. % of max allowed deflection is probably a better measurement of whether you are being too aggressive.

And as always, experimentation is key.

[nwallace (Nick Wallace)]

Welcome to the forum! Glad you are having a great time and learning.

As you have read, the general rule for rigidity limited machines like the Shapeoko is to do high WOC and lower DOC. The Shapeoko Pro is quite a bit more rigid than the Shapeoko 3 but the rule still applies.

As for general recommendations on actual speeds, this gets pretty hard because it really depends so much on the material, end mill, cutting strategy and geometry you are cutting. The general rule of maintaining a minimum chipload of 0.001" is a great place to start. As you get more comfortable and gain a feel for the CAM side of things, you can push that much farther. Your intuition looks mostly correct, just keep in mind the first thing I wrote about Shapeoko’s being mostly rigidity limited. If you want better finishes, go slower. If you want more material removal, go faster.

At some point you will screw up and that is okay. I would just highly recommend you have some sort of E-Stop setup. Something that will cut power to the machine and router at the same time and is in easy reach.

Here are my general rules:

I always run adaptive clearing at 75% WOC and change the DOC based on the material.

Finish contours I typically run at 150-200% DOC when compared to my adaptive DOC in the same material.

For finishing the bottom of pockets I try to run no more than 0.01" DOC just to help improve the finish quality.

I am not sure what you mean by finishing surfaces but contouring and pocketing should cover that.

The recommended feedrate range is not really relevant information in my opinion other than the concept that slower generally equals better finishes.

Depending on the end mill and materials you can have chiploads much lower or higher than 0.001" but it is a good starting place for anything with a diameter above 1/8" on these machines. I have run as low as 0.0003" and as high as 0.012" depending on material and end mill size.

Learning CAM in Fusion 360 and in general can feel like drinking from a fire hose. Just keep experimenting and you will get more and more comfortable.

[nwallace (Nick Wallace)]

@Julien

It’s a matter of preference. The feeds and speeds will be limited by the fight between the cutting forces and the intrinsic machine rigidity (and to a much lesser extent by the router/spindle power, 99.9% of the time it’s not the case). You can choose to “spend” that amount of cutting force either some “shallow & wide” cuts with a large radial engagement but limited depth per pass, or in a “deep and narrow” cut with large axial engagement but (very) limited radial engagement. Yes the shapeoko likes shallow & wide better, but…

• folks who figured this out mostly cut metals, where rigidity is everything. In wood, no so much.

This is true. However, if you are trying to max out your material removal rate (MRR) in wood the concept of maxing your WOC and then increasing your DOC until you are machine or end mill rigidity limited should still apply on a Shapeoko.

It definitely isn’t as cool as seeing your end mill at full depth in the material but it is a very reliable way of cutting.

I have not personally found a difference in tool life using either method. I have yet to replace a single tool from wear with many hours of cutting in aluminum. In the rare event that I replace a tool, it is because I dropped and chipped it… At work I have replaced many tools on our machine because of wear. This is because laminate and some woods are serial murderers of carbide. We have found that generally tool life has a direct relationship with MRR x “Time in the cut” and it did not matter whether that was deep or shallow cutting strategies.

[adcostanza (Adam)]

Thank you both. That’s very helpful feedback and I really appreciate the depth of your replies. Previously I was at just 100% DOC with 0.002" chipload it seemed like I was getting some chatter on adaptive clearing paths with the plain construction 2x4s. Per your advice, I went ahead and tried out doing wide and shallow cuts (75% WOC) with 25% DOC and it seemed to go pretty well. I was actually able to run that ta 0.003" chipload and it didn’t sound bad at all. I think I can likely increase the DOC based on the calculator and potentially the chipload as well.

I certainly learn new things every time I run a new program on the CNC. Today I learned you should definitely face FIRST before adaptive clearing otherwise you risk chipping some of the fragile bits remaining after the adaptive clearing.

I also did do some finishing passes at 300% DOC cutting off just ~0.01" of material.

Any tips for finishing passes? Would you recommend still targeting 0.001" chipload or is that more important for roughing? Also any tips to avoid tool marks on the bottom of a pocket? Maybe I just need to run multiple passes or reduce the WOC?

Thanks again for all of your in depth responses, it’s been super helpful!

[adcostanza (Adam)]

@Julien

So, the 100-300% DOC only makes sense for very small stepover (optimal load) values, AND using helix ramping into the material, such that the tool engagement even at that 300% DOC is always small.

The rules of thumb mentioned in the ebook are an attempt to capture what came out of the community discussions on the matter, as well my own experience, so do take it with a grain of salt, a healthy dose of skepticism is always a good thing.

Fair point, I was likely just trying too high of WOC. I’ll definitely revisit and play around and compare with the more complex calculator so I can see what the potential load is on the machine.

@nwallace

Learning CAM in Fusion 360 and in general can feel like drinking from a fire hose. Just keep experimenting and you will get more and more comfortable.

Definitely agreed on this. It’s certainly very rewarding though!

@nwallace

I always run adaptive clearing at 75% WOC and change the DOC based on the material.

Finish contours I typically run at 150-200% DOC when compared to my adaptive DOC in the same material.

Super helpful starting points, thank you for this!

[nwallace (Nick Wallace)]

@adcostanza

Any tips for finishing passes? Would you recommend still targeting 0.001" chipload or is that more important for roughing? Also any tips to avoid tool marks on the bottom of a pocket? Maybe I just need to run multiple passes or reduce the WOC?

The best chipload for finishing will depend on the material you are cutting. For wood, keeping a lower chipload AND feedrate will generally produce a better finish. Just don’t go lower than 0.001" with any tool 1/8" diameter or larger to prevent rubbing unless you know you need to. When you get into really small tools this rule changes. Most people don’t start out with this use case though.

Another thing to consider when looking for better finishes is to try both climb and conventional cutting. Some woods will do much better with conventional. We could get pretty far into the weeds on the pros and cons of each but the simple note to go along with this is that your feeds & speeds may be different between climb and conventional with the latter typically requiring you to be a little less aggressive.

Best way to minimize tool marks in the bottom of a pocket is to make sure your machine is well trammed, reduce your WOC and reduce your feedrate. The vibration caused by changes in direction on our belt driven machines can show up pretty easily in the bottom of pockets if you are feeding fast. This is even more pronounced in metals and I have taken the additional step of reducing the acceleration settings on my machine. In wood I expect that this will be unnecessary. You will never completely remove tool marks from any surface you touch with this class of machine but you can minimize them.