Hardest aluminum long mill can CNC

Hi all,

I’m looking to make some things out of aluminum and wanted to know what’s the hardest I could mill? Can I work in 7075?

Thanks in advance.

Hey Sky, welcome back.

If you have a choice, use 6061. 7075 is harder, and therefore harder to machine. I have done a fair amount of 6061 machining on the LongMIll but I have not tried 7075. With a carbide 1-flute end mill I think you could do 7075, but the slower feed rates may be an issue. Remember that machines of this size are not rigid or powerful enough to push very hard. I’ve been doing depths of cut of about 0.010 - 0.015" with step overs of 10 - 20% and feed rates of 18 - 24 in/min depending on the toolpath. I think you would need to start at 50% of these numbers and increase - or decrease - with trials.

Please let us know how it works if you try.

Have fun. Stay safe.


Bill, thanks for sharing your settings and speeds and feeds for aluminum, that is really helpful. I want to give this a try once I find some pieces to machine. Hopefully thinngs will calm down soon and I can get over to the metal supermarket.

1 Like

I’m also planning on cutting some 7075 so would be interested to know what others have experienced with feeds and speeds.

@BillKorn this is really helpful info, thanks for sharing. I just did my first aluminum test last night in some plate (I -think- it is 6061, the label doesn’t specify - came from Amazon), making some accents for a desk I built with my daughter. When I dug around, one of the references I used for my speeds and feeds was Winston Moy (who uses a Shapeoko) and also Longmill T-Rex video: https://www.youtube.com/watch?v=BYkk0dFohZs

In Chris’ video notes he says: “A lot of the bulk material removal was done using a 16mm dado router bit at 1800mm/min with 40% step over while running the router at around 25k RPM. Then a waterline cleanup was run with a single flute 1/8” (3.2 mm)˜ alm flat end mill at 1200mm/min and 0.5mm step down. And finally an 1/8" (3.2 mm)˜ ball nose for the linear passes running at 2000mm/min and 10% step over with the router at 15-20k RPM."

With 20 ipm being ~500 mm/min, I’m curious why you have ended up running at that lower speed? Is that something you dialed down to in order to get the desired finish etc. or did you start low and were happy with the results so kept it there? Are you running a low RPM to go with that? And is it a 1/8" or 1/4" bit?

I’m completely new to this, so could be dead wrong, but I ended up trying 40 ipm using a 1/4" upcut bit (a brand new one), based on looking at various references. I tried a 1mm DOC but it was too aggressive to my ear so I cut it in half and used .5mm and it all seemed to work ok.

I was only doing a light facing and then a contour, but I quickly discovered my (well used) wasteboard isn’t quite level when milling at sub-mm levels. I think I was around 2-3 on the router RPM. Chris’ notes seem to suggest we could go quite a bit higher (at least if a 1/4" bit is used), as did some other videos related to the Shapeoko, as long as DOC was kept shallow.


I have the Sienci 1/8" bit for aluminum but I realized it won’t work with the router in the higher position, at least not without putting more MDF under the main wasteboard on my machine. I really wish there was a practical way to move between positions without having to take the wheels off the XZ assembly - nudge nudge @chrismakesstuff

@BillKorn I am increasing leaning towards what I think you did with the strips to raise the Y-axis rails by 3/4" and have two layers of wasteboard, and possibly a third when required. I really like your approach of having a second piece to bring the table surface up to the stock level, but the ability to remove it to get more Z-axis gantry clearance room for taller pieces. Likewise, I’m thinking of having an indexed board that I can on top as the third layer to reduce the Z room to allow for smaller bits without needing to move the router.

Likewise, in order to reduce deflection issues, I’d like to run the router higher in the mount (especially in the upper position) so the force factor of the level action is reduced as much as possible. Shimming up the wasteboard with additional pieces will help with this. Moving it to the lower position would also help but would likely cause issues working on larger pieces. Although now that I reflect on that, perhaps the lower position and shifting the router up so the typical bit I use is in the same Z height position may kill two birds with one stone… hmm…

@BillKorn What position do you run your router in?


Jeff, it’s been a while - Hope you’re well.

As you’ve seen, there are more considerations involved to get good results when milling aluminum than there are for even hard wood, like how sharp the mill is, how fast you’re going, RPM, length of the mill, router position, where you set up on the table, the surface quality you’re looking for, the type of aluminum…

So to answer your question about how I chose my settings - I am rarely in a hurry, I’m usually looking for at least a SPI #3, or 320 emery cloth, finish right off the table, and I do zero-stock-to-leave and follow it up with what amounts to a polishing pass using the same mill as the roughing pass - easy in F360. I use the Sienci 1/8" 1-flute for aluminum mill. Notice that it’s hard to get a precise measurement of this tool because of the flutes, but it cuts like it’s really 0.118" diameter. Also note this may be due in part because I do keep the router low the mount, so I may get a couple extra thou deflection. So, slow. Slow also keeps the heat down, but makes me keep the router low in the mount - see below. If you use F360’s adaptive tool pathing, you can set the upper limits of speed, DOC, and step over a little higher and it will optimize them, to a point.

I bought the LongMill intending to use thicker stock for some projects I wanted to do, and I saw that the design would make it very easy to adjust the elevation of the cutter relative to the table with spacers. When I did the initial assembly I put a continuous piece of 3/4" MDF under the mounting pads. This works great with either thick stock or an extra thickness of waste board to get the stock higher, but can necessitate keeping the router lower in the mount, which can increase deflection. As you said, if you have the room keeping the router high in the mount is better. I have shortened some mills to get the router lower when I need the travel. For smaller jobs I work as near the limits of the axes as the dust shoe mounts allow. I just got the magnetic shoe so that should gain some travel in at least the negative x direction.

I routed a series of 1/4" holes in the main table surface spaced 5" apart in a line centered in the x direction, and another in the y direction. Then I did the same in each layer of spacer board. I use 1/4" drill rod pins to fit the holes and lock the table and spacer boards so there are no screws needed to hold them in place. Some of my spacer boards for small jobs are only 18x24 - easy to surface - so the pins let me move or rotate the boards. The spacers also get the stock higher so I can raise the router in the mount. I’m currently milling waterline sections of a 28" model tugboat hull that require stock that are 37" long and 4" thick, and the adjustable spacers let me mount the stock diagonally in the table low enough to clear the shoe mounts and the x axis beam. I like to keep my main table untouched as much as possible, so I prefer milling registration holes in one of the small spacers for flipping the stock over to do the other side, like a hull section.

Anyway, good to hear from you. Stay safe.


1 Like


Thanks for the detailed and fantastic follow-up. I’m about to machine the inlay inserts for my daughter’s desk so I’m going to give your settings a try. First I need to see if I have enough MDF to elevate my work piece up to a height I can safely use the Sienci 1/8" mill… Going to check that now…


One thing I forgot to mention is that it can be a pain to get a good level final surface with multiple spacers. Even if you face both sides of each one, when you stack them up you can still get a top surface that isn’t parallel to the cutting plane because little errors add up.

I don’t surface the plywood main table. I put a full size - 36x48", with 1/4" inserts inserted from the back - piece of the flattest fine grain 3/4" MDF I can find on top. This gets me up to what would be normal zero counting the spacers under the feet. My travel with the magnetic dust shoe is 30" X and 32.7" Y, and the facing mill cut beyond the X and Y travels, so I surface an area about 30.75x33 in the MDF. This lets me put up to a 30x32" spacer, with inserts, into the faced area. Then I surface this whole spacer. The facing mill will extend off all four edges so there won’t be a lip. This spacer can be removed and replace without needing to be re-faced.

Now I have a flat, versatile surface that has lots of hold-downs, can be replaced easily if damaged, and can be swapped out for different sizes. And for thicker jobs, like my tug hull, the small spacers an be removed so I can use the bottom one. I put a self-healing cut mat on top for cutting card stock with the drag knife.

Hope it helps. Please publish how well your aluminum insert goes, and if you change the speeds and feeds. Also, chuck the Sienci mill as high in the router chuck as your Z travel will allow. Unless you go slowly it’s easy to deflect a 1/8" mill when cutting aluminum. I also go 18-20,000 RPMs with that mill. I have not had heat issues even at slow cutting speeds.

Have fun.

As always, super helpful info. I went through the “little errors adding up” issue yesterday when stacking up some (damaged) finished cabinet doors to get the height I needed. Thankfully as I was through cutting and the material is only 1/8" it didn’t cause too much of an issue on this project.

It did, however, lead me to wonder how the heck I am going to hold down metal workpieces. In this case I used the drill press to put pilots through the four corners of the 6" x 12" plate and then I screwed it down to the unblemished cabinet door surface. However, as you will likely predict, I had a slight upwards bow in the middle, maybe .75mm, enough to through out my precision through cuts.

It had me pining for a small vaccum table I could sit on top of the spoilboard to hold down metal pieces. I’ve been checking out DIY vaccum setups (for small areas, like 12x18 or smaller). Not sure my 5 HP vac can generate enough pull to be useful - we’ll see.

What is your preferred way of work holding for smaller metal pieces?

I’ll post photos of the inlays in the next day or two, hopefully I’ll cut the second one today (material just arrived late yesterday). The “eyes” in the ghost in one of the pieces are tiny - 10mm tall and maybe 8mm wide and I had a hell of a time cutting them with tabs. The first three broke off and went up the vaccum before they were done. I slowed things down even more and eventually got it working. I had to resort to a chisel to get them out and then some hand sanding to clean up the burrs.

How do you remove the tabs on your finished work?

Thanks for the additional details on how you handle your spoilboard, I was wondering. I don’t want to surface the base layer as I intend to continue to do pieces that requiring tiling/indexing and extend past the Y end of the table. If I surface, it will make those uneven. I like your idea of being able to insert and remove the “zero plane”. In theory I could have one that stays within the X/Y range and is surfaced (and re-surfaced as I wear it out) and also a larger one that mimics my entire table top dimension, for when I have large pieces cantilevered out the end for tiling.

I’ve got to get my new dust shoe made, the original one is driving me nuts and I really want the lost X-travel back. But I think I’ve been sub-consciously delaying the work as it will cascade in to me needed to re-mill the mounting plate I did for the proximity sensors that cantilever over the sides of the XZ top plate (for my X travel) and it also cascades in to this discussion and will require me to re-do all my spoilboard/table work. Not a bad thing, just still trying to get my arms around it so I can be confident I’ve got all the current ideas incorporated.

I find I accumulate a lot of tools, bits, dowels etc. on the patch of machine left in the left front area in front of the controller. I’m trying to decide whether a new, wider, table is in order. I’m also hoping to dig up the details on the steel frame table I think U-Line or someone has on offer that another user found. That one is 48x48 but looked VERY rigid.

I tried about 20 ipm and it worked great, if very slowly. For the detailed work I would say it is a good place to be. I had some tight inside radiuses that I did at the lower speed on their own. Moving to the exterior contours I did some at 20 ipm and some I sped up 70 ipm but then I broke the bit so I ended up slowing down again and using my second bit (thankfully there were two from Sienci :)).

It did cause me to wonder whether I should be roughing using a larger bit and move to the 1/8" for the finishing passes and up close work. It does look like 3mm is correct, as you said, not 3.175mm for the Sienci Aluminum bit cutting radius - thanks for the heads up! Everything fit nicely with that adjustment.

For depth of cut I went tried both .3mm and .4mm. Both seemed ok but I think I’d stick with .3mm, having broken one of the bits. I can’t say it was DoC, I think it was the speed and the tight turns on the toolpath that did me in, but as you said before, patience and quality finish generally beat time to completion. It’s a different world in metals, for sure.

I couldn’t find clear RPM details so I used the 24K that Chris used in his video and also that Winston Moy referenced, but I am going to try 18K-20K as you suggest, when I run the second insert today. 24K, whether correct or not, “sounded” too high to me but I had no basis until your comment, so I’m pleased to hear your suggestion.

I did move the router up in the router mount but nearly as much as I would like. However, I only had 2x cabinet doors to work with (just over 1.5") so if I move the router up much further I’ll exceed the Z-travel. You’re entirely right, deflection is definitely a consideration with the 1/8" mill, so getting it closer is better, but staring at it and wondering how to construct a more permanent but flexible solution sent my mind down the multi-layered MDF path you described. Your thinking is way ahead of where I was, so now that’s on the list too. :slight_smile:

Very smart. I have one of those on my woefully underused electronics work table, maybe I’ll steal it and bring it over now that I have the confidence to mill the drag knife (which unfortunately is still a few projects down my list - life keeps getting in the way). What kinds of projects have you been using the drag knife for? Any suggestions on where to get the vinyl/decal stock to use with it?

Given my propensity, so far, to accidentally cut too deep, I’ve been reluctant to go with a T-track system in the table top, but I’m starting to find my clamping options quite limited now that I’m working with really thin stock. If I can’t get a reasonable tabletop vaccum option working (and I am dubious I have anything with enough pull) I may need to acquiesce on the T-tracks.

I’ve also got in the back of my mind the aluminum boat building shop nearby that does CNC jobs as a side business. They have a 5x30 table and lots of aluminum sheet stock and my spidey sense tells me they may figure in to my final plans, I just don’t know how yet…


For metal holding, I’ve had good luck with double-sided carpet tape for small parts. The areas are small enough that the thickness of the tape is uniform enough not to affect the surface plane. I’ve used the duct-tape/super glue/duct-tape method for larger jobs. Non-uniform thickness can be an issue. Another reason for slower cutting speed - Less force requires less work holding. When cutting from a plate I use regular hold-downs in the threaded inserts.

Tabs can be tough. I try to make them as small as possible, particularity height. I think short wide ones are easier to remove. Slower cutting -> easier to hold, smaller tabs. I use a small belt sander, files, and sandpaper to clean up. One mistake I’ve made repeatedly is trying to be cheap and cut as close to the edge of the plate as possible. This doesn’t allow enough meat left in the plate to hold the tab and small parts go flying around.

I have used 1/4" tools for roughing aluminum, but I’m usually doing detail or contour cuts so I use the 1/8". To rough, just use lower DOC, slower cutting speeds, and smaller stepovers. I have found that climb milling works better than conventional milling. I would have thought the opposite because I use conventional milling a lot in non-fibrous wood like MDF. Winston Moy has a good video on aluminum milling with 1/4" mills.

I use the drag knife mostly for architectural models. I have an architect friend who sends me 3D models of buildings he is designing. I import them into Fusion 360, do all the scaling and cleaning up they need, and slice them horizontally. Then each slice (Lots of slices!) is cut out of card stock - the ones from Dollar Tree work great - and stacked up to make a building. Then he uses them to show clients. Apparently most prefer something they can look at and walk around than see on a screen.

The only vinyl cutting I done was with stuff I had laying around. I think it was about 0.020" and both drag knives worked well. It’s a little hard to hold down because it’s so soft. I haven’t looked for any lately, but I heard thin sheet plastics in general are hard to find due to people making face shields and barriers.

Instead of T-Track I’ve been using press-in inserts with 1/4"-20 threads inserted from the back of the board so they can’t pull out with good success. A bag of 100 is about $15 and they’re re-usable. When I face the back of a new spacer I also mill holes and countersinks for the inserts on a 4x4" pattern, along with 1/4" alignment holes to keep all the spacers registered.

I had (have) the same problem of cutting too deep, either because I mis-measured, or the design was wonky, or I don’t get Z zero set exactly right. Now for anything that goes all the way through, like contour cuts, I put a piece of 1/8" insulation foam from Lowe’s under the stock. It’s small cell foam and is already fairly compressed, and I haven’t had any trouble with it deforming and screwing up the cutting plane as I tighten the clamps. If I want to go the the bottom of the stock and it goes a little deeper, no harm done. In fact I frequently design my contour cuts in F360 to go 0.005" below the bottom surface because the bottom edge ends up looking better. It doesn’t work as well for small pieces of stock you’re clamping because you can tighten the clamps unevenly enough that you crush one corner. I use it routinely with aluminum plates.

Wish I lived near a shop that generated aluminum scrap. Shipping costs for that stuff is rough.

Have good one.



I finally had a chance to run your settings, doing some O.D. 32mm circular “inserts” for a pen/marker holder I made. Made multiple inserts with various I.D., including 10.45mm. With your settings and everything tight on my LM I was able to hit 10.45mm exactly on the I.D. first go with a lovely finish on the edges. Thank you!

If I don’t get distracted in a different direction I may just tackle the drag knife next, I finally got a selection of stock from metals supermarket…


Jeff, thanks for the feedback.

I’m sure you can push the LongMill more than I do, or change the feed rate and stepdown. I have had good luck, particularly with good quality endmills, at reducing the stepdown a little and increasing the feed quite a bit. Seems like the surface quality is better and the material removal rate is as good or better.

There is a new YouTube video by Shapeoko on optimizing speeds and feeds, all of which applies directly to the LongMill, except that they are limited by the belts and we are not.

I used .25 as a step down. What are you currently using? A guy with a steel CNC told me .25 isn’t milling it’s polishing. :slight_smile: Hey, I’m just impressed we can do it at all with such an accessible machine!

Jeff, keeping in mind that I don’t push the LM or the cutters as hard as I could because I’m usually looking for the best finish right off the table, and I often have the router low in the clamp, for a nominal 1/8" mill I use about 0.015" DOC with about 20% stepover at 22 in/min. My experience pretty much agrees with the Shapeoko video that surface finish gets better as the DOC decreases and the stepover increases. This keeps MRR the same. I have not tried the super Datron mills that reportedly cut much better with better finishes.

1 Like