Reducing a 29hour Machining Time?

1

The island of Kauai is the more geologically dramatic in Hawaii’s chain. More to the point, it should be one of the most dramatic topographies to machine.

https://a360.co/2XqECHF

I figured this would pose a good challenge for me to learn more about Fusion 360 as well as the limits of my XXL.

Unfortunately, there has been a ton of “shut up and color” time waiting for the 3D adaptive clear to compute in my CAM workflow. There are a few issues that I’m not totally clear if I see a good solution:

  1. Kauai has tons of steep canyons and valley that at my current scale might cause the collet nut or spindle housing hit when plunging the end mill to the bottom of a valley. Can Fusion be programed to consider this in its toolpath? If so, how? I’m thinking that no matter what you do it will be somewhat imprecise as you will have to manually measure how much of your endmill extends out of the collet…

  2. 29 Hours of Machine time on a 3D adaptive clear and 1/4" ball nose endmill… the bit is traveling 1.588 MILES. The computation time here is insane. I’m going to bed turning on an option and waking up to see if it will increase or decrease the time. Is my issue here scale, the number of facets, or an option I simply don’t have selected? I’ve messed around a lot with flat area detection, ordering by depth, machining cavities, etc…; I haven’t been able to get a successful computation using “Most” on the Stay-Down Level, but “total rapid time” seems to only be 1hr 8mins so I’m not sure how much this would help…

  3. A finishing pass… I haven’t been able to get a parallel tool path to successfully compute using rest machining on this model. Not sure if there is something weird going on with rest machining resulting from the super complex 3D Adaptive step, but it just generates an error when I try to turn it on. With Rest Machining off and a 1/8" ballnose endmill and a 10% stepover results in 258hrs of machining time… the “Steep and Shallow” toolpath in Fusion 360 sounds like it would work well in this application… should I buy it and try that? or is trying to machine this using a square bit (maybe a downcut bit) and hand sanding a better idea?

  4. Practically speaking; how frequently should I allow the carbide compact router to cool down? How many “miles” are the S3’s motors good for? How many 1/4" ball nose endmills would this job eat through going into something like walnut or koa wood? I’ve never used only the first 25% of a bits cutting face for this amount of material removal, is there a better way to engage more of the flute without creating a dangerous stepdown value?

Thanks in advance!

2 Likes
2

Measuring extension is not a big deal. I made (many, many years ago) step gauges for this. Basically an L shape, with heights for the vertical leg in 5mm increments.

in fusion, some operations (adaptive 3d, for example) have “shaft and holder” option. This allows you to have the toolpath generator consider the tool, spindle, etc, and avoid contact. You need to model the tool and holder.

Clear with a bullnose or a square end. Then finish with the ball end. Square end computes fastest, and clearing is much more efficient.

Clear with a stock to leave of maybe 0.5mm. Then select a finishing strategy WITHOUT rest machining. Finishing strategies don’t clear. They surface. Rest machining confuses them if the rest machining isn’t from the same strategy with a larger tool (most, but not all, cases).

1 Like
3

Have you tried to reduce the facet count of your model before trying the CAM? It should definitely decrease your computation time, and should not decrease the detail.
https://knowledge.autodesk.com/support/fusion-360/getting-started/caas/screencast/Main/Details/a281d5a7-2a50-4191-ad96-199a4f49edc0.html

1 Like
4

Took it from 29hrs to 26hrs… using a square down cut. This was followed with a Contour Pass with an 1/8" Ball nose (2.5hrs) and Parallel Pass using the same 1/8" ball nose and a somewhat non-finishing stepover value of 1/16th" (50% of the bit) and NOT machining steep areas… this takes 3:3hrs. Getting better but still LONG.

I decreased facets by 75% using from the original STL; trying to keep it around 10k… any lower and it seems to do a little to much smoothing to my eye… no idea how the tools react?

5

Does it still take a full nap to compute the tool paths after reducing facets?

Also, just curious, what is the contour path for? I usually adaptive clear with a 1/4" endmill leaving 0.02". Then parallel with a ball for the finish pass. This finishing pass can be run extremely fast since it is only removing 0.02" plus the scallops.

6

Yes, the square did calculate faster than the ball as @enl_public said. Now, it’s still like 2-3 hours of computation time on the adaptive clear.

If i enable “Machine steep Areas” with a 1/64" minimum step over on the Parallel pass the Machining time goes from 3.3hrs to 16hrs (lots of steep areas i guess). Basically I’m trying to recreate what I THINK the Steep and Shallow pass that you have to buy does…

EDIT, also… the 1/8 Contour Ball is going places where the 1/4" Square couldn’t (around the tips of some of the peaks)

7

At this point, more information is needed: How large is the work? Feed, depth of cut (radial and axial)?

I can’t open the model from your link (not sure if it is security settings or at the AD end, but this is fairly common with the share links. I am not waiting for fusion to finish gronking after downloading. I gave it 30min and killed it. I need to get work done.)

For a large part, this is not really out of line as a machining time or path length. You are presumably removing a substantial quantity of material with a small tool.

1 Like
8

I’m playing around with it now. It’s a pretty big piece with a ton of geometry/surface area. It’s going to take awhile no matter what.
I’m trying to reduce computation time by unchecking the “detect flat areas” the only flat area on the model is already defined in the setup, so I don’t think this option is necessary. If I happen to make any leeway, I’ll re-share the file. No guarantees though.

9

Thanks to you both, assuming it’s going to be a 20+ hour job; what should my considerations be on some of the more practical things I mention in #4 of my original post?

10

The model is 3" tall. That is a lot of stick out for your endmill. Do you have endmills long enough? There is going to be some deflection on that much stick out during the roughing pass. You have it programmed for a 1/4" bit with a 1/4" step down at 65in/min. That may be too aggressive. Especially if you are going to use a hardwood. I wouldn’t take more that 1/2 the diameter of the bit for a step down. Just my 2 cents.

11

Not yet, I was trying to figure out if they were going to be needed as I referenced my concerns in #1 of the OP. I haven’t tried a computation with the shaft and holder modeled yet on the adaptive roughing pass.

I guess this is where I’m a bit ignorant, I’ve been sticking to that 50% step down rule when it doesn’t have such a huge impact on machining time, but in this case it does. I thought the “Slot Clearing” and “Optimal Load” of 50% of the diameter of the bit would help immensely here… am I wrong?

Using a hand router I’ve routinely made 1/4” deep cuts using a 1/4” bit… hell I’ve made 3/4” deep cuts using a 1/4” bit when I didn’t care too much about what the hole looked liked.

12

PS with that turned off computation time is like 25mins and machining time is down to 18:41hrs with a square endmill… PROGRESS!

2 Likes
13

Not an expert in F360 but have you played with the plunge rate, increasing the PR just a bit can have major impact on machining time for 3D stuff.

14

Longer response than probably necessary:

Good question. I have no answer. Barring a very hot environment or out-of-spec loading, a router should really not need cooldown time. The life will depend on how hard it is worked, operating temperature, cleanliness of the work area (dust and chips entering the unit will shorten the life a lot, both by interfering with cooling and by wear of moving parts), and undoubtedly other factors.

Again, it depends. I would rough this with a square end or bull nose, use an axial engagement (depth of cut; max step down) of maybe 2 (or 3) times the tool diameter (or the full tool depth-of-cut if less than that), and start with a radial engagement (step over) of about 30 to 40% of the tool diameter. You can trade off the axial engagement for radial engagement to use more of the cutting edge. This also may have benefits in clearing the chips and keeping the working part of the end of the tool at a better operating speed. For a 1/4" tool, this would be 1/2 (12mm) depth of cut and about 0.100" (2.5mm) radial engagement. If you keep the chips appropriate (feed maybe 0.005"/0.15mm to 0.010/0.25mm per tooth is a moderate starting point for most woods) the tool will live longer than if it is buried in the material and jammed with chips, or the cuts are so light (low feed or low axial engagement) that the tool rubs.

I can’t emphasize enough that a ball end tool is usually not ideal for heavy stock removal. The geometry at the end of the a square end or a bullnose is such that, for horizontal feeding, the cutting happens at the periphery and there will be little to no rubbing of the end in most cases. With a ball end, the center, intentionally, sticks out and will be cutting, with varying speed, chip size, and comparative little clearance for the chips to get out. When doing heavy removal with a ball end, the tool will not last as long as a square end or a bullnose.

As to overall life, I have never worn out a ball end in wood (never done much with exotics, though), though I have dulled them enough to replace-- still usable, but distinctly not optimal-- and broken a number of them due to poor job setup or control failure (for example, when calling the cat, be sure that the USB cable is not between him and your lap… just saying) I have worn the ends off machining glass-filled materials many times. Profiling 100mm long glass-filled PTFE bearing halves for 50mm shaft dulls a 1/8" ball end to useless in about 4 parts (roughing done with a bullnose on that one-- about two parts per tool. The glass is to cut and makes nasty dust-- DO NOT try this without appropriate extraction).

Final note: If the job is a one-off, and it will take 18 hours, but you spend 12 hours in CAM to get it down to 16, you have a net loss.

1 Like
15

Chuckle, while this is for a friend, it’s more an opportunity for me to learn. And lets be honest, I’ll probably be sitting there watching it cut nervous that Mt. Kilauea is going to get clobbered by the collet nut. So anything I can do to eat while it cuts is a win-win. Point taken though!

1 Like
16

Another “trick” to reduce computation and machining time, and to make it easy to break the job into subjobs of shorter machining time is to use the depths. Reduce the clearance height and retract height to just above the stock (On the Nomad, I tend to use 5mm or less clearance) and the feed heights to as little as practical (operation dependent).

Use the top and bottom heights to eliminate machining of already surfaced flat areas (offset the height by maybe 0.01mm into the work and the CAM will avoid it) and adjust both to break the job up into several parts (for example: top 20mm, next 20mm, next 20mm, and so on) by layers. You may be able to be more aggressive with a shorter tool and less/no collision risk near the top and gain speed.

3 Likes
17

It would seem as if these two recommendations are in conflict with one another, correct? @themillertree is saying I’m being too aggressive with 1/4" Step-down and @enl_public is saying go as high as 1/2" or 3/4" stepdown…

My understanding is that the entire purpose of an adaptive clear to to engage more of the bits cutting length… couple that with slot clearing and a optimal load of .125 (.1000 per @enl_public 30-40% suggestion) and this should be a safe operation and a way not to just use the first 1/8" of my cutting flute.

Am I correctly understanding the Adaptive 3D passes?

Also, I think from my reading engaging more of the axial length of a bit is safer/better with use of a compression bit?

18

Greater depth of cut will usually require lower axial engagement. It is not a one for one trade, but it is close for roughing. But with greater depth and lower radial engagement, you can run a greater feed rate so it is a gain in speed as well as distributing the wear better. Rigidity is the limiting factor. There is a difference here, but I am not sure we are working from the same premises.

On the Nomad, with much lower power, I rough 2m/min at 10KRPM with a 40% radial engagement and more than 3X the diameter axial in many materials-- poplar and HDPE, for example. Maybe 20% lower for maple and UHMW) with 1/8" bits. This is a nominal 0.2mm (0.008") per tooth for a two flute, but the chip is a fair bit less due to chip thinning.

You have enough power and RPM to go pretty heavy when roughing, but rigidity might be an issue. With the adaptive clear, the intent is rapdid removal of material, not finishing. Test on some scrap. You might be surprised. I do not have a shapoko, and I don’t know what you have upgraded, so I can’t speak to rigidity for you. Your tooling will be much stiffer than the 1/8 I use on the Nomad and spindle power is in your favour. I might be wrong, but I suspect you can go pretty far on cut depth and up the travel, since you have power and RPM.

1 Like
19

I’ve updated the model linked in the OP (https://a360.co/2XqECHF) based on a all the advice in this thread. 15.5hrs for clearing is manageable. then tack on another 10hours for finishing passes and we’re still below the original 29 hour time for JUST the rough clearing. So I’d say this is a Win.

The only thing still giving me slight concern is the .50" step down value on a 1/4" downcut bit, but I’ll do a test on plywood and see how it goes. Also, I plan to model the shaft and holder but I’ll need to spend some time with some calipers infront of the unit before I commit to those parameters making it into the file.

1 Like
20

Let us know how it goes.
I haven’t played with a true HSM with the Shapeoko too much, but I have wanted to. I just stick to the 1/2 of endmill diameter for DOC and 40% stepover rule for most of what I do. I goofed around with what you are working on a little yesterday, and it made me want to try a taller DOC and smaller radial engagement at a higher speed, using the adaptive tool paths. Good luck with it and please do let us know how it goes. It should be really nice when you are done.