We use cookies to personalize content, interact with our analytics companies, advertising networks and cooperatives, and demographic companies, provide social media features, and to analyze our traffic. Our social media, advertising and analytics partners may combine it with other information that you’ve provided to them or that they’ve collected from your use of their services. Learn more.
So while waiting for the replacement limit switches I ordered, I started working on a better solution for bed leveling. I designed a little bracket, (that uses the threaded holes on the side of the spindle mount), to attach a dial gauge to the spindle mount. I had some Aluminum luggage tag blanks that I thought I could use. I don’t know what alloy they are, but they seem to be pretty soft. I designed the part in AutoCad and made the toolpath with Cam Bam. I used a150 mm/sec at .15mm per pass. This is with a 1/8" two flute upcut endmill that is supposed to be for Aluminum milling. This is with the standard X-Carve 300W spindle.
Except for the fact that I screwed up the outside profile, (should have been outside, not inside), it came out OK. I think I will fix that and do it again. You can see the finish is kind of rough. The smooth parts are where I filed off the remains of the tabs. That could be from going too fast or too deep. it does produce nice sized chips instead of dust, which I think is a good sign. I used TAP Magic as the cutting fluid, which seemed to work, but made all the chips stick together into a oily mess. The noise was pretty low, (Not so loud that you need hearing protection). It did kind of resonate in places. I don’t have much comparison to identify chatter.
Any suggestions to improve the finish would be appreciated.
It’s a good start! You might try WD40 instead of TAP-magic. If nothing else it will be much cheaper. I use the long red tube it comes with to spray a line along where I’ll be working. Does your “aluminum” endmill actually say aluminum on it? The few I have are all marked Aluminum, or have an “A” in the model # and the flutes are a bit steeper than a regular end-mill.
Second attempt. Fixed the profile. The finish was looking good, but somehow it all went bad at the end. I’m thinking maybe the piece was moving a bit at the end…
You can see the right hand edge looks the worse, like it was chewed on. Maybe as it was finishing the last bit of the profile, the tabs were not enough to hold the rest of the piece, and it rattled and was chewed on by the bit.
Also that little sharp edge on the scrap. That is really sharp. It made one of those really clean cuts in my hand, the ones that don’t even start bleeding for a minute. Like a super papercut.
It does look like something was moving. You might need a different clamping strategy. But it’s nice to know the machine can cut aluminum. It’s hard to see the small circles at that angle - are they round?
It’s a Kyocera two flute solid carbide upcut mill (1/8"). I got it from drillman1, and it claims to be rated for wood, plastic, and soft metal. These are pretty cheep, so I’m not totally surprised if they are not the best aluminum endmills.
I’m open for suggestions. Preferably for endmills that don’t cost $25 for a single 1/8" mill.
Here’s a couple that are made just for aluminum - they’re called high-spiral or high-helix. The steeper spiral is supposed to cut soft metals easier, and pull the swarf up out of the way. I’m self-taught so I have a lousy teacher, and most of my tooling comes out of estate-sale machinist chests so I’ve broke/burnt/killed a LOT of endmills as Iearn. I have noticed a big difference between using a regular endmill vs one marked just for aluminum.
Well you are on the right track will ordering your bits from Drillman1 on eBay. But you need to switch to his Destiny Viper 3 flute bits for some better results like this:
The Destiny Viper 3 flute 1/8 endmills are made for milling aluminum and they work like a charm if you work within the limits of the OKO and X Carve for milling aluminum. You might try you piece this way. First mill a pocket larger than your stock about .5mm deep. This will get your stock 100 flat to your mill and make sure that your following cuts are at the right depth and not having bumps or dips in them. This is very important for the first cut into the stock. Once you have that pocket milled, place double sided tape like this http://www.amazon.com/gp/product/B00006IF5M/ref=oh_aui_detailpage_o04_s00?ie=UTF8&psc=1 on your stock and then stick it down in the pocket (make ure the pocket is super clean of dust) Then if you wish you can clamp it also. Then mill your circles out first. Then pause and use a wood screw and washer to screw down through your holes you just milled to hold the piece down as you mill the rest of it. On my mount above I milled the screw recess, then the screw holes and did as I suggested above to hold down each mount. This keeps them steady for the following 7 mill steps and even lined up perfectly for the chamfer passes.
On your first cut into the stock, make sure you are JUST on the stock top with the end mill… being off just .1mm will have an effect on the cut. Looking at your images, you are pushing too hard and take too deep a cut in one pass. I would slow down to around .75 or so while you get better feel for it and stick to .1mm DOC for now. The OKO is just not built to take large DOC cuts in aluminum but it can do well as you see above if you take your time with it.
The posters are right that using an endmill made for aluminum will go a long way to helping your cuts do better. But how you set up your cuts and feed rates will do far more in the long run. The finer details on my mounts are cut with a 1.58mm (1/16th) 2 flute endmill and it works just fine, but I have to pull back the feed rate for the smaller end mill a bit and rarely drive it faster that 75mm/m at .15mm DOC with a spiral down cut path.
All of the milling in the pics above was down dry on the OKO with a 400w 48v spindle with these end mills: Destiny Viper 3 flute 3mm (1/8’), 2 flute 1.58mm (1/16") end mill and a 4 flute 45 degree chamfer endmill. Most of the pics are after a 3 stage finishing process in a vibratory tumbler and were anodized on by me.
I hope you get better results with all the great advice everyone is posting and if I can be of any help I look forward to answering your questions.
The issue I am currently having doesn’t appear to be with the endmill or the holddowns. I did another test last night, and I did try lowering the feed rate a bit. I also left about .05mm of stock, so it the part wouldn’t come loose, I figured I could punch out the last little bit by hand with a file.
I watched closely as it milled the profile. The first 12 passes looked about perfect. The bottom of the slot was perfectly smooth, and the sides looked pretty nice, with a little bit of a wavy texture. However once it got to about 13 (I think) something happened, it started chattering a lot, it ripped out the bottom of the slot in one spot, and made a big racket as it milled the south end of the profile. It seemed like it suddenly changed the position on the Y axis a bit. I could tell the stock didn’t move, the clamps were still in place. It wasn’t enough movement to be the belt slipping a tooth. Maybe a missed step on the Y stepper motor? Any ideas of what is going wrong here?
I think this is the pattern. It gets most of the way through, then it losses a bit of position, and the end mill starts trying to cut through the full thickness of the part, and it bounces and chatters, and produces that chewed on look.
Some things I notice. The mill spends a lot of time wallowing in a mess of its own chips. The chips don’t really clear out. If it is long profile cut, I can try and clear them out with a tool while the mill is on the other side of the piece. I don’t think a vacuum would have much effect on the chips and cutting fluid mix. Maybe attaching an air hose from a compressor to the side of the spindle mount might help.
The vibration isn’t that bad. It is a little loud when plunging into the material. Each time around the profile, you can hear when the Z axis goes down .15mm. I was thinking of clamping the X Carve to my workbench, to make it a bit more stable.
Ok, I made up a little test gcode that did a small profile halfway through, a couple of pockets, and a profile all the way through with tabs. This time the machine didn’t chatter at all. I changed the feed rates to 125, plunge rate to 25, and the depth per cut to 1.5. It made very little noise at all. I also tightened up the X belt, as it seemed a little loose. You can see from the pictures there are some places where it chipped the edges. The anoidization layer really shows this, and it is probably prone the peeling anyway. The pockets looked good, and the finish on the bottom is pretty good. The finish on the sides is kind of wavy. The worst cut is the full depth profile, where it really chipped the edges. In this case it wasn’t motion, it was just breaking the material. I’m starting to suspect this aluminum is not the best alloy for milling. I should move on to some 6061.
The sea of chips filling the pockets and slots is also a problem. Any suggestions there? The squares look OK, but the circle doesn’t seem to be round…
Anyway here are the pics. I used the SLR with a macro lens this time, so you can really see up close.
Chris, I’m a little disappointed you didn’t post what I assume would have been your next picture - “Here you can see the individual atoms from this cut”
Sorry you’re having problems with aluminum, hopefully you get it sorted soon. Thanks for being out on the leading edge and sharing your experiences with the rest of us.
Just a thought, have you considered making the cut a bit wider than your cutter, so it’s only cutting one side at a time? If you cut both sides of the feature at once, you can get some really odd vibration effects. I note that the pockets are very clean by comparison to the through cut profile.
Hey Chris if you can post your gcode here I can take a look at it and see if I can find any issues. I also plan to work up a simple test for you and send a small gcode test your way so we can find out if this is a CAM issue or mill controller issue.
I currently run the 400w 48v spindle. My larger mill (21x37) runs the 1.5kw spindle and I really think it is far too heavy for the X carve. a .8kw might be OK as they are lighter. Also going with an air cooled over water cooled will save a bit of weight also. There are 65mm .8kw and 1.5kw spindles which might work far better than the stock 80mm sized .8 ans 1.5kw spindles. The weight of the 1.5kw water cooled 80mm will put a large twisting stress on the gantry and I am not sure the gain in cutting power will be seen with a belt driven system without getting too much belt slope under heavy cutting conditions.
So I think I found the main problem. It appears there was a loose connection on the cable connecting the two Y axis motors, so occasionally only one would move (the other would just drag along), which caused a lot of vibration in the machine, and probably skewed the X axis a bit. So that appears to be fixed.
Unfortunately my first test with the fixed Y axis, I was also testing using ramping on the profile, and accidentally left the cut depth at the default of .4mm instead of .15mm, that didn’t go well. The bit was deflecting side to side, and end up making a cut about 50% wider than the bit. It didn’t break, but given the velocity at which it started throwing chips, I think I want to get some better goggles.
