I have been trying to chase away the chatter I am facing with my machine for a while now but am having no luck. Posted are videos of the machine running and I will post my cut file in a follow up post as well. I am using Freud 76-102 bit, however this chatter and tearing is occurring with similar Amana DC bits, both both old and new bits alike.
I am cutting into Hickory in the above example but I am seeing this issue with walnut, oak, and even plywood (to a lesser extent). Parameters: 1/4" DC bit 12,000 rpm 0.125" DOC 2400 mm/min feed 600 mm/min plunge 0.1 mm chip load
Difficult to tell from the view angle of the video, but you seem to have a quite a lot of tool stick-out.Tool deflection will contribute to chatter. For slotting type situations, you will probably need to slow your feed rate down - Try 1200mm/min and 2mm DOC and see if it cuts more cleanly.
I will get it slowed down and see how it goes. I have the tool stick out where I do to reach the bottom of the bed.
I would do a finsih pass, slotting is always a problem since the cutt is cutting on both sides. For the roughing add 'radial stock to leave' (in Fusion360 terms) of about 0.2mm or whatever your software needs, you may have to lie to it about the cutter size. Then for the finishing pass I would try going the same direction (climb cut as you are now) and also going the other direction (conventional cut) and see what gives me what I want. in that segment where the bit is descending for the next pass, what is the finish like there?
Unsure on the finish in the desending area, I will cut a new part to test and report back. I use Vcarve for my cut files, I am running a seperate last pass of .003 inches (.08mm) for a finishing pass. Can you get chatter from a lack of engagement of the bit with the part? I can also test a seperate part with a conventional cut but in previous testing this tended to shift my chatter from the Y to the X axis.
I have been using ChatGPT 4.0 to help me setup speeds/feeds and it tends to push on the need to hit certain chip loads. ChatGPT is recommending I would need to run at 6000 RPM if I am running at 1200 mm/min which is impossible since the makita router only goes down to 10000. TLDR: My question, how much does chip load matter, and if so, does chatGPT's goal of .1mm make sense?
The curse of AI! It’s a starting point, but it clearly isn’t working for whatever reason, so you need to change something. It’s not a magic number - if your machine / tool bit isn’t stiff enough to take the load, then you need to reduce it. Different types of machining operations are limited by different factors - slotting, in particular is s demanding operation. Experimentation and building up experience with your machine and materials is the only way. Leave the RPM where it was, just reduce the feed rate and/or depth of cut. (Reducing the feed rate with constant RPM will reduce the chip load.) FWIW, my readyreckoner (based on my machine) suggested the figures I quoted above, based on 12000 RPM
I run the same doc and feed rate as you posted above but at about 16000 rpms and do not experience chatter. I do try to insert the endmills in as far as is reasonable for the material to minimize deflection. Because mine is not an industrial machine I use the recommended rpm/chip load as a starting point, but will manually adjust the rpms while listening to it cut. I can tell by the sound when I am getting chatter.
Thanks for the help. I just tested my machine at 12,000 rpm @ 1200 mm/min and at 17000 rpm @ 2400 mm/min, both of which eliminated my chatter and significantly improved my cut quality. Looks like the 0.1mm chip load was to high for the machine and it is better to shoot for 0.05 - 0.07 mm chip load. I have a few followup questions as well since I have figured out the issue. Giarc, I am sure this is something that will come with time, but is it possible for your describe what you are listening for when changing your RPM? I think I have a pretty good idea of what chatter sounds like at this point, but is it possible for the machine to not be cutting "enough" material? ChatGPT also mentioned watching for different chip formations, is this something I should be paying attention to and if so, are there any examples of what they should look like?
Glad to hear you're making progress Yes - you get things like scorch marks when cutting wood, or the cutter rubs and grabs intermittently. Always worth paying attention - as long as the chips look like chips (small curls rather than dust), then the cutter is actually cutting. The best thing to do is to spend an afternoon experimenting - push the feedrate; dial it right down; try deep and slow cuts vs shallow and fast, and home in on where your machine gives you the results you're looking for on the material you want to use.
Sorry, I have been traveling for work a lot lately so I am slow to respond. I do not really know how to describe the sound other than it sounds "off" to me, like it is vibrating. I use a variety of endmills and the smaller diameter ones give the most issues. I try to design my projects around either the 6 - 8mm size corner pockets because inverse square is my friend. A 6mm diameter endmills has 4 times the material of a 3 mm of the same length. So they are much stiffer. I only use smaller than 6mm if I have to. As mentioned by others, I took use a roughing pass and leave 0.2- 0.3mm for a full depth finishing pass to give a nice clean edge. Pretty much everything thing I do is based on experience. I know that I can cut pretty much any wood from pine to oak at 2500mm/min at 18000 rpm nothing breaks. When I start with the cut, I will usually start around 16000rpms and if it is easily cutting, I turn the rpms down. If it struggles, I turn it up. For 3D carves, I can cut easily at lower rpms and hate 3000-3500mm/min because I am only stepping over at 40% roughing and 10% finishing. I bet I am down close to 12000 rpms for finishing. It is nice and quiet. One thing I do for these carves is do a profile cut around the model and leave about 4-5 mm form cutting though. Then my roughing passes never start out cutting with 100% engagement like a slotting operation. So in summary, because these are not $10000+ machines, you kind of have to experiment with your own to dial it in. Also, my x gantry is two cbeams and only 1000mm wide. If yours is longer, you may not be able to cut as aggressively.
Can I add a question?? What DOC's are you using for the listed cuts?? Both my Amana and SpeTool Feed and speed charts recommend 1x bit diameter, seems like a lot.
There's some info in the posts above (I suggested 2mm). The bit manufacturer's recommendations are likely made from the point of view of maximising material removal rates without breaking the tool; they don't really take into account anything to do with the machine. We need to experiment to see how much our individual machines can cope with, which is likely much less than the tool. The things to consider are (in order): 1) The speed that the flutes on the bit travel through the material (the cutting speed or sometimes surface speed). The spindle RPM determines this for a given cutter diameter. There are tables of optimum values for various combinations of tool and workpiece material, however In reality, for small diameter carbide cutter with wood / aluminium work pieces, most of the time we can run the spindle flat out. 2) The chip load (how thick a chip each flute on the tool is expected to cut). This is set by the number of flutes on the cutter (fixed), the spindle RPM (which we fixed in the previous step) and the linear feed rate. We can choose the feed rate to set our preferred chip load. (See the discussion above - there is some flexibility as to what exactly this number is, but I would expect something in the 0.002mm to 0.01mm range). 3) Material removal rate. The more material we are removing, the more power is required from the spindle, and the more force is generated in the tool. If we increase the amount of material removed (by cutting deeper, or stepping over more) sooner or later the spindle will run out of power, or we will generate enough force to snap the tool. Much more likely, however is that the cutting force reaches a level that is sufficient to cause deflections in the machine and/or the tool that result in instability and hence 'chatter'. This will be our limit. We can choose how deep a cut we try and make, and in some cases, how wide a swathe we try and take off the workpiece on each pass in order to keep things sweet. This is the step that can only really be determined by experimenting and gaining experience. 4) Optimise the settings for the job in hand - maybe drop the chip load a little (slow the feed) so that the machine can cut through a particular workpiece with fewer passes; Or reduce the step-over to get a better finish; Or increase the chip load or depth of cut to get the job done quicker if the machine can take it, etc. etc. But the point is that you're making these variations from a consistent starting point, having worked through the process above. TL/DR - Unless you have an industrial machine, your machine (or anyone's) will have limits that will very probably be reached before you can get to the optimum recommended by the tool manufacturer.
I always go with 1/2 of the endmill diameter. I may go deeper if there is a small step over, but I usually default to 1/2 diameter.
