I tried running at 60 IPM but here’s what happened:
Also I noticed even though I use a probe to zero off my piece the first pass doesn’t even touch.
Do you suggest I lower the depth per pass or the feed rate?
My first instinct would be to lower the RPM. It looks like you’re melting the aluminum.
The chips look good. Is that the #274 single flute cutter?
Until you’re confident with the probe, I would always double check my Z by touching off to the top of the part after using the probe. Sanity check!!
2 Likes
Unfortunately it’s a dewalt router so my RPMs are stuck higher than ideal. I’ll drop it 2k RPM and give that a shot. I think it’s 16k rpm at the lowest.
Usually with a 1/8" end mill I’m doing 0.008" depth per pass and 18 feed rate, 18k RPM. That feels pretty slow but stable (result is clean and end mill doesn’t get clogged). Do you have a S3 XXL? I’d like to hear what numbers others are doing on the same machine. Also interested in the numbers the HDZ can do since I’m looking to get a second machine very soon.
I’ll try doing a few different contour passes and see if I can get something working by playing with the numbers. Also I’m printing a chip fan, hopefully that helps. I’ve noticed the air blast struggles to reach certain areas when the pocket gets deep and the angle isn’t right. When it has to rip an area with no air blowing in it the chances of clogging become 100% once it’s deep enough.
When I read the A-Z manual I think it remember there being something about pocketing past the diameter of the tool. My tool is 1/8" and the material is 1/4", is that not going to be a problem? I think I’m maybe supposed to add an offset so I take off some extra material and it’s not a 1/8" pocket anymore, it would give some extra chip clearance. If you look at the first few cuts into the material it’s near perfect. Once it gets deeper the cuts get worse and worse. I think this is maybe a chip clearing issue.
1 Like
I have an HDM. I cut with a 1/8" O-Flute at 10000-12000 rpm, 30-60 ipm, 0.010 doc.
Pocketing would definitely help. However, pocket paths don’t recognize tabs, so you would have to pocket down just to the top of the tabs. AND… there is a bug in pocket toolpath cutting narrow pockets. It cuts them just like a contour (depth first), so you don’t get the benefit of the stepover to clear chips.
Think about adding mist to your air blast. That helps a lot!
2 Likes
I think your machine is a lot more rigid so you can handle that speed, plus you have access to lower RPMs which helps too. I hear the S3 XXL has some rigidity issues especially towards the center of the bed. I might have to put some focus into trying to fix that in the future. Maybe epoxy granite in the rails and a steel bed or something. Then get my 2.2kw spindle installed so I can get those low RPMs. Sadly I can’t get this done for at least 3-4 months but I’ll just try to optimize what I’ve got the best I can. If it takes 6-10 hours to cut the tabs it’s not the end of the world. I’ll just pass on costs to the clients. Maybe offer a wood option too, since those will cut faster.
What kind of mist would I use? I have the air blower that can mist but I’m scared to ruin the MDF wasteboard.
A lot of guys use alcohol/water (10% alcohol), which evaporates fast, both good for cooling & keeping the table dry.
I’ve been using “Kool Mist”. It comes concentrated so the gallon I have will likely last the rest of my life 
The mist is so fine it rarely gets on the spoilboard. Unless I forget to point the nozzle up after using it. I have to use my thumbnail, a piece of paper, or look through the mist at something black just to see if it’s on.
If you get a minute, try cutting one of the holes using hole-milling. If that works without gumming up, I can program the pocket with adaptive milling for you.
1 Like
Damn I just shut down the machine and laptop then came downstairs and read your message. I didn’t test cut any holes but my machine is definitely maxing out at the following numbers:
0.008" depth per pass, 8 plunge, 18 feed
16-18k RPM (no noticeable difference)
I tried multiple variations going more aggressive with the feed rate but the cuts weren’t turning out nice. Even just boosting the feed to 22 started to create problems.
Next I tried taking more shallow cuts and keeping the feed rate high.
Even 0.005" at 40-60 feed is too much for my machine.
0.003" at 45 feed creates a nice, clean result. Maybe the cleanest cut I’ve made yet! The chips aren’t as big but still passable. The issue is it’s just as slow as my usual feeds and speeds haha. I think the machine likes taking more shallow depths of cut, it sounds like it’s in less pain 
No worries. I’m playing around with adaptive, if for nothing else my own curiosity. I’ll try it out a 0.025 DOC ( I think we might get away with 0.050), and a 0.003" stepover at 45 IPM. I’ll let you know what kind of time I get.
1 Like
Always wanted to try adaptive but seemed a bit scary to engage so much of the end mill. At least with a 1/8" end mill it seems like it could break fairly easily.
With a 1/4" I’m curious what the damage to the machine would be. Can the machine actually snap a 1/4" end mill or would it stall the servos and make them skip over and over?
Just a heads up btw, when I was testing before I had a piece fully cut out and held by tabs, then on the next piece it wiped out some of the tabs from the first piece and allowed it to come loose 
it launched into orbit. just warning ya in case you try to cut some haha
PS - how did you make that 90 degree line to cut out towards the center hole?
I do aluminum on an S3 XXXL (unsupported modification where I joined XXL and XL Y extrusions) with a Z plus. 1/8 inch two flute upcut bit, 0.010 DOC, 10 in/min plunge (but I override this way down), 24 in /min feedrate, 16000 RPM. Contours are a no go unless very shallow. I turn profile contours into a wider pocket to tab depth and then contour the remaining depth. No air, no mist.
Troubles:
I had trouble using a three flute 1/4 inch. Chips glued to the end mill. I dont use that anymore.
Plunging with 1/8 in bit. It was very easy to plunge too fast, losing steps in Z (especially on the standard Z but it can still happen on the Z plus if you push too hard). I slow way down for the plunges.This might be why you sometimes are above the surface (lost steps on a previous plunge tool path).
You will not win any races but can make some nice things with patience.
1 Like
Thanks for the tips! Can you share details on the mod you did and why?
I’ll try creating a pocket down to tab depth. Also going to put in a few more test runs and see if I can optimize the higher IPM toolpaths. I might be able to get a slightly larger chip load.
I have the same issue with a 201 end mill in aluminum. It loves to get clogged. I’m only using 0 flutes now.
That’s a very good point. I’ll just take things slow and steady and not abuse the machine trying to push it past what it can handle. Upgrades will come in time. The main thing is part quality and consistency, keeping repairs to a minimum etc.
When you contour 2 pieces next to each other, you need tabs on both pieces
The blue lines to cut out the shelf to the center hole… I made a rectangle & trimmed it so the cutter is starting out in the slot.
1 Like
Interesting. I thought that shapes had to be connected, no open lines allowed. Going to test that out and play around a bit.
I did some more feed and speed testing.
0.0035" DOC 45 IPM - ok
0.004" DOC 45 IPM - ok
0.0045" DOC 45 IPM - very unclean results and end mill ended up breaking
Decided to stick with 0.004" DOC and see how much IPM I could ramp up to.
Turns out I can go up to 60 IPM at 0.004" DOC and the result is very clean. It’s possible my old end mill was messing up my test results, not sure.
I’m going to test holes and pockets now.
Any advice for stepover setting?
1 Like
What was the stepover in your tests? If you were fully engaged & 0.004 @ 45 IPM works, then you can stepover up to the diameter of the cutter.
I like to look at the cross section of the chip and not just the forward advancement (chip load). If I can use 0.004 DOC & half the diameter (0.0625") stepover, then I should be able to switch them, 0.0625 DOC & 0.004 stepover for adaptive. It’s not an exact swap as side cutting & end cutting generate different forces, but it’s relatively close.
But either way, I’m removing a cross section of 0.004 x 0.0625 = 0.00025 in² chip area.
I started with a used S3XL and regularly wanted to cut bigger things. So I bought the expansion kit (no longer available) from Carbide 3D to convert it to an XXL but I combined the XL and XXL rails to make a machine bigger than an XXL. Linked here Shapeoko 3 XL + XXL Progress. I did this only for size. At the time I don’t think Carbide 3D offered anything larger than an XXL. I mentioned this modification only because I probably lost rigidity which would be detrimental to my cut quality especially in metal. The only other modification was to upgrade to a Z plus. This was because I saw problems (lost steps) when plunging into aluminum with the stock Z. The Z plus helps but it is not a cure all. (Probably need ramping toolpaths.) I am very happy with the overall machine and Z plus but I don’t expect it to be a home replacement for a $100,000 machine.
Stepover doesn’t matter for contour cuts right?
I did some pocket tests and half diameter or less works well.
Big thanks again for your help and tips. I managed to get a bunch of the pieces cut out today. For some reason there’s a +30% time increase when the toolpaths move from Carbide Create to motion. It took me a long time but I made around 20 and they turned out nice.
Any advice for dealing with tabs at the end of a job? I’ve been thinking about skimming them down as low as possible before clean up. Maybe I’ll trim the tabs down to 0.008" and hope they don’t break off.
That’s quite the machine you’ve got there!
I’ve got the HDZ upgrade which helps for sure. For some reason my machine hates 0.010" DOC, it makes nasty build up like what’s seen in the video. The machine much prefers taking smaller cuts and moving faster. I’m not sure why my machine is like that. Kind of confusing because it can’t even handle the stock “conservative” aluminum cutting tool profiles very well.
After testing I’m getting super clean and reliable cuts. I just need to run shallow and fast. It’s actually faster than the other profile and cleaner.
2-way tape or tape/glue should let you get the tabs pretty thin, or even through cut.
At 0.008" you might be able to remove them with a knife.
Output a single contour/profile/trim path that you can drop the Z & rerun to test it out.
Otherwise, bandsaw and sand or file, or break them off, depending on the finish req.
What are these tabs for? i.e. what are the tolerance & finish requirements?
The faster you move, the less heat you build up in one spot. This is one of the key principals of high speed machining. And since we have no choice with these spindles, embracing HSM is necessary.
As for times. I view them as a really rough estimate. I use them in a relative sense. If I adjust a path & the time in CC goes down, the actual time on the machine should also go down. But I don’t trust the time calculations in CC or CM.
1 Like
Currently I’m using a fence setup. Trying to stay away from the tape and glue as much as possible though it definitely has some upsides.
The tabs are to hold acrylic (one tab for each corner). The two holes on either side are for magnets. Wanted something clean with no visible fastener and easy on / off when needed.
This topic was automatically closed 30 days after the last reply. New replies are no longer allowed.