I have successfully used my shapeoko 5 to cut out a profile on a 3x3 feet 1/8" piece of 6061. I first screwed down a 3/4" piece of MDF onto the bed and leveled it with a 1/4" square endmill (that took a while lol… its what I had on hand). Then I used a number of wood screws around the entire border letting the edge of the countersink style heads wedge against the aluminum to hold it in place. I adjusted the angle I used the screws until I was not cupping the center upwards.
First operation: Make the hole pattern in the top. This will double for additional workholding for when I mill out the profile shape. I used a 1/8" endmill, which had a tiny bit of spiral to make a hole a bit wider. Unfortunately this is where I had my first problems: The endmill did not want to plunge at all. I could see the gantry visibly flexing upwards quite a bit until it finally punched through. The operation technically succeeded, but it apparently needed a ton of tool pressure, and positional accuracy suffered a lot.
Any tips on punching holes in 6061 sheets? I’m thinking an extra operation to start it with a center drill possibly. Then possibly another drill before using the endmill to expand the holes out to final size?
With the holes made I secured down with more wood screws, and removed ones at the edges near where I was going to be cutting. I used a 1/4 inch endmill for the profile cut because I thought the bigger size would be better for rigidity. I then increased the travel speed until the chips started to have a better size. The machine seemed to complain A LOT. I put a line of tap magic down between each pass. Somehow the depth of cut on the first pass wasn’t very consistent even though I had just leveled the MDF that the sheet was secured to. What I mean is the depth of the first pass started a bit shallow, then near the end of the pass it was deeper than I would have liked. Any ideas there?
I definitely made things harder by cutting as a channel, but it simply would have taken 10s of additional hours to mill away all the material away from the outside of the profile shape. Is there any reasonable strategy to cut out a shape in sheet metal without the high cutting forces from channeling?
You really should just learn Fusion 360, Adaptive toolpaths, very adjustable, great ramping.
If you’re using a wood endmill for aluminum could be a very telling reason, the feeds and speeds of cutting holes with no chip evacuation, fogging, etc.
Yes a center drill is one idea but, a good toolpath and a good cutter with proper chip evacuation setup would also fix this.
In future I’d reccomend uploading the file or if it’s proprietary tell us your exact feeds, speeds, stepover, DoC etc for best answers. Even things like did you zero from bottom are huge for knowing what went wrong.
I’d check all your screws, couplers etc if you had that much flex, I bet your hybrid table flexed ALOT as well as I can see mine move if i apply more than a 20lb point load which is why I’m looking in to ordering a 24x24x3/4 6061 plate for fixturing.
What you’re looking for is called trochoidal milling and it can be done using the adaptive toolpath option in fusion 360 but it is EXTREMELY algebra intensive and probably wont be brought to C3D ever in their software. It’s just an insane amount of work for them with what I’m sure is already a huge chipload
It seems daunting but if you’re already experienced in CAD in any way it shouldn’t be a huge step. I’ve just started and it’s just alot of little things you can optimize, one or two videos and you’ll probably be making chips in a much better mood.
While cutting aluminum is one of the more advanced things you can do on a machine, it is still something that most people can do with basic tooling and software. There’s a couple area’s I think are worth looking at to see what can be done better in your case.
Can you share what endmill you were using? You mentioned it had a little bit of spiral. Every endmill should have a spiral, unless it’s a straight flute woodworking bit. Do you perhaps mean taper?
What toolpath are you using? Are you using a drilling operation in Carbide Create? Generally, the best way to make a hole on a CNC router is to use a pocketing operation, and use an endmill smaller than the desired hole diameter to cut it out.
Can you share your cut settings? Particularly with the 1/4" endmill? While you are correct that you want enough feed rate that the endmill can form a big chip, you can’t just blindly increase feed rate without factoring in what the machine can handle. As you increase speed, you generally need to also reduce depth to keep the loads on the machine reasonable.
Regarding depth of cut, how far away were you securing/clamping the material from where you were cutting? If your cut was going more than a couple inches away from the nearest clamp/screw, the material could be moving an amount that’s easily noticeable. Aluminum might be strong, and 1/8" might seem thick when you’re holding it, but as you cut, something that thin could totally deflect.
Cutting a single slot/channel is definitely waaay faster than machining away all of your excess material, but as you cut deeper and deeper, it can trap chips and lead to your endmill clogging. What I’ve found to be a reasonable compromise is to draw an offset vector from your object’s profile, by 1.5x your endmill diameter, and machine that like a pocket. Instead of a narrow channel that traps chips against the endmill and causes it to chatter/clog/ping-pong against the walls of your channel, you’ll be machining a more generous “moat” around your part that give chips more room to get out of the way.
While Dean is technically correct that more advanced software like Fusion has capabilities that would make this a breeze, in some cases it’s akin to telling someone who can’t seem to win in a go kart race that they should skip the upgrade from an 80cc engine to a 125cc motor, and instead just buy a Lamborghini. There’s plenty of tricks you can employ without employing the pro-level software to make things go more smoothly. Adaptive/trochoidal toolpaths are kind of like the gold standard for optimizing material removal, and what I used when I tried to push a Shapeoko 5 Pro to it’s absolute limits, there’s nothing wrong with a regular contour or pocket toolpath. You can even amp it up a respectable degree with features like Ramping in Carbide Create Pro, or other CAM software that can be taught in a weekend without needing a 30-hour course or something (Fusion’s learning curve is notoriously horrific).
TLDR: Share some more details about what you attempted and how, I’m sure plenty of us in the community would be happy to help you figure out how to optimize your process without breaking the bank, or setting you up to have to pick up a software that’s approximately 25x more complex than necessary for your particular job.
Fair enough, I’d put it more like are you going to spend 30hours learning and using shortcuts in a software that is going to put more wear and stress on your tools or would you rather spend 30 hours and save yourself money in the longterm when the software is functional in the freemium versions.
The Lambo saves you time later and money now. Why cut with only the tip of the cutter when you paid for the whole cutter.
It was a 3flt HSS endmill, there are actually no markings on it so I am not sure of the details beyond that. The smaller 1/8" one had 2 flutes. The spiral I mentioned I meant to say was the motion plunging into the material, I know that most endmills do not want to plunge straight down, so I wanted to specify that it made a spiraling down motion when entering the martial, HOWEVER, when viewing the save file again I see that that is not the case and it is straight down… oops! Clearly if I can find a way to ramp in, it should enter better.
2&3. I was using carbide create, selected the profile for the 1/4" bit I was using and the profile for metal. I did infact use pocketing operations for the small holes. I think that because the 1/8" endmill was about 80% of the final hole diameter, that carbide wasnt able to make much use of the operation for a better toolpath.
There were definitely many spots more than a few inches away from the nearest hold down screw. I need to find a better way to hold down the material because the screws along the edge have the side effect of pushing the cut-off material inwards as the last of the channel is cut away. There were not enough holes provided in the final design to get all the workholding I need. I suppose I need to make sure the stock I order is larger than the final piece by a large enough margin that I can create a hole pattern to hold down the cut off piece better.
I think this is exactly what I needed to hear, by making a channel larger than the endmill I am using, then I can make the majority of the cutting forces only be present on one side at a time.
I do actually use fusion for creating designs and toolpaths for my other machine, but Caride has so far been good enough that I havnt bothered trying to figure out how to export gcode for the shapeoko yet. I do miss the ability to simulate int he way you can with Fusion though. Honestly I feel like I need to lean in the FreeCad direction because Autodesk has been increasingly annoying me with their insistence of using their terrible cloud system. Anyways…
I can tell you the chips are much smaller than in the picture, partially because my depth of cut was about .08". I wish I took a video, because sharing that would likely tell a lot more of the story. I think for the next aluminum cut I will try to set it up and make a toolpath, then make another post here to see if you or others have ideas before I hit the “go” button.
Sounds like you’ve got a good grasp on things to try next. I’ll leave you with another thought or two.
I would start with a much shallower depth of cut, just so you have more margin for error in case the material gets pulled up a fraction of an inch. And it also gives you more ability to scale your feedrate higher without getting into a zone where you’re taxing the router. I would suggest dialing things back to between 0.02" to 0.04" vs 0.08" for the 1/4" endmill.
Certain endmills like the single-flute 278-Z Carbide sells (there are others out there too) are very clog-resistant when cutting narrow channels. The lone flute the endmill has is oversized, which helps get chips out of the way. And the geometry of having only one cutting edge means it only ever touches one wall of a slot at a time, and the material will never “pinch” the cutter. That means less friction and heat. That would likely let you get away with doing a single-width contour cutout toolpath.
Also, HSS endmills are cheap, but generally not by enough of a margin that they are worth it vs longer lasting carbide endmills.
Is there a way in carbide create to easily make the first depth different the remaining depth steps? I suppose I could get the same affect by making the starting height the amount higher up that I want the first cut to be less deep.
I’ll look into the single flute cutters, I have one I use in acrylic that I get good results with.
Regarding the heights, there’s not really a good way. If you try to trick CC by telling it your stock is thicker than it actually is, just keep in mind that it may affect how you need to set your zero. If you set your zero at the bottom of your stock, there will be no difference, but if you set it on top of your stock, you’ll need to account for the “phantom stock” difference. It may just be better to pick a depth per pass that leaves you with enough performance margin to account for any unevenness in the stock and how the cutter engages it.
Gentle word of caution/reminder: Aluminum single flutes will work in acrylic but not vice versa. Plastic-optimized endmills are very sharp and have a more aggressive angle at the cutting edge that are more fragile. You get better edge quality that way. Aluminum single flutes are engineered for durability. Make sure you don’t mix them up when you reach for an endmill at the machine.
I try to do smaller holes with a “Hole-Milling” strategy.
You can do this in CC using a mill that is ideally 2/3 - 3/4 the size of the hole.
So, for example if I wanted a 3/16" hole with a 1/8" cutter, I would set it up as a contour path, inside offset, and set the Depth per Pass greater than the Max depth. Then use a ramping angle of 1° - 3°, and a plunge feedrate the same as my cut feedrate, or just a bit less.
The path will spiral down to the final cut depth, make one level pass at the bottom, then retract.
So I inspected the bits I used, and realized that I mixed up my bits. For the small holes I used a 1/8" DOWNCUT wood endmill! What a blunder! Surprised it worked out for me at all.
