I often use this data sheet. It is in german, but I think the values are obvious.
Actually the most depend on the cutting speed (vc) and pitch per teeth per rev (fz). So for wood (Holz in german) the values are vc=450-500m/min, and fz~0.25 mm for 1.5mm endmill.
In fusion 360, both values can be added in the configuration of a tool, and corresponding feeds and speed will be calculated by the program (or can be calculated manually by the formulas given in the data sheet).
Cutting notches, the depth is mentiond to be up to 2 times of the mill diameter, but I feel better with a max. of once the diameter.
If some translations are needed feel free to ask.
@Teeman It’s true that running too fast can cause heat build up. I’m certainly no expert at this. I tend to listen to how bits are cutting and reduce or increase feed accordingly. One thing that I should have remarked on was your reference to material. You will need to vary both your speeds and feeds relative to the material you are cutting. For example, you can move faster in softwood than in hard woods. MDF cuts quite easily, but is tough on bits, owing to the high binder content. Plywood is terrible on bits owing to the glue between the plys. Pine, although it is soft, is pitchy. Acrylic and solid surface material (corian) cut nicely, but you need both slow feeds and slow speeds to prevent the material from melting. For me, it’s all an experiment.
There are lots of chip load charts available, but I don’t find most of them particularly useful as I am using a Makita router and it does not go slow enough to bring the recommendations in the charts into play. I’m likely reducing the life expectancy of my bits as a result.
@JHahn Thanks for the chart. I must admit that I do not understand the concept of pitch per teeth per rev. Is this equivalent to chip load?
Wow 1200 rpm sounds painfull slow for a diameter of 1/16". These values correspond to a cutting speed of ~6m/min, which is a ~1/15 of the cutting speed needed for steel. But ok, maybe its a really special endmill I dont know… or am I missing something?
But in general I’m sorry, I dont agree with you Grant : The sienci 1/4" 2flute upcut endmill (the one I got from the early bird starter set) cuts really nice in oak with vc=500 m/min → 25000 rpm → level5 on the makita, and chip load of 0.04mm (chart says 0.055) ->xy-feed=2000 mm/min. This seems fast, but you can adress the cutting force and load on the mill by reducing the cutting depth/vertical infeed (yesterday I used 10mm plunge/cutting depth and 1.5mm infeed). However, this is a 1/4" end mill… so wrt. the chart, especially endmills of lower diameter have the problem the max of 30000 rpm of the makita is way to slow (1/16" dia and vc=500m/min → 100k rpm).
So I would rather state that the makita turns way to slow for most operations the longmill is designed for (cutting wood/aluminium with small endmills).
But yeah for sure to start with a new tool: Better feed 100 times to slow than 100 times to fast.
@JHahn Tks Jannik. Don’t get me wrong. I get very nice cuts using 1/4" bits in all kinds of wood. However, unless I am reading chip load charts all wrong - a definite possibility - I cannot go slow enough to get a 1/4" bit into the ideal chip load range. For example, if I set the speed to 50 inches per minute on a 2-flute 1/4’ bit running at the lowest Makita speed of 10,000 rpm, I get a chip load of .003. the ideal is between .017 and .020, depending on the species. So, again, unless I am reading the charts wrong, I am not even close.
However, using the same feeds and speeds using a 1/8" bit, I am close to the ideal range.
Here is a link to one of the chip load charts that display the numbers that I am referring to. There are lots of others, as you know.
As I said previously, I tend to ignore all the “science”, listen to the machine, and look at the quality of the cut. So far, that method seems to be working for me. I have only broken bits when I foolishly hit a hold down. Perhaps I am dulling bits faster than I would if I followed the charts, but my bits seem to be lasting long enough.
I buy the carbide end mill PCB bits off ebay and have had pretty good luck with them. They range in size from .49mm to 1.37mm. I’ve used them for cutting oak and plywood and typically I’m not cutting very deep. When I do break one it’s no big deal since they are so inexpensive (a box of 10 goes for $10 CDN with shipping). I will set the feed rate to 25 inches per minute, the plunge at 10 ipm and the depth at .03 inches on the largest and 10/10/.015 on the smallest. I have only broke one of the smallest bits so far. I set the spindle speed to the lowest setting.
Like others have mentioned, these settings vary depending on the material you are cutting.
@gwilki Also if this is going to be a bit off-topic, I will try to “scientificate” the discussion a bit, but first: Dont get me wrong, I wont treat on your toes. If your results proof you right - then you are right in what you are doing. However, sometimes it is nice so see what the science says, so:
I checked your chart and I think you are not reading it wrong, but it it differs a lot from the one I linked above: The chipload for hardwood @GDP is 10 times larger. For the 1/4" endmill it says 0.5mm chip load - thats huge. I dont even get this chips using my table saw or anything else - so these values are obviously provided for some real professional machine with enough rigidity, and not for the longmill.
So maybe use the values provided by Sorotec, these seem to be more conservative and a good starting point. By the way, your values are really close to them. You estimated a chip load of 0.003"=0.076mm to be a good value for the 1/4" endmill, Sorotec says 0.05-0.06mm - so actually less than that.
Last point: The chipload calculater misleads one to choose a feedrate and then the corresponding rpm. I think one should do it the other way round:
Calculate the rpm according to the cutting speed (defined by material and diameter of endmill), and then
chose the feed rate to match the right (according to chart or feelings) chip load.
So as I said, in Fusion it is really simple to do so: Just create a tool with right dimensions, then specify the cutting speed (program will compute the rpm), and then the number of teeth and dedicated chip load (prog computes the feed rate) - and you are ready. (Provided that the computed values are realizable with the Makita.)
@JHahn Tks for this Jannik. I’ll continue to do what sounds right and gives me acceptable results. However, you are correct. It’s good to know what the “science” says.
One thing you can likely clear up for me is, for example, if my calculated chip load is .003 and the recommended range is .017, is my chip load higher or lower than recommended? I know that this displays my ignorance loud and clear, but so bit it. Clearly, I know that the number .017 it larger than .003, but does this mean that my chip load is lower than recommended or higher?
As you demonstrate, one of the problems using chip load to determine our feeds and speeds is that the available charts vary wildly. Like you, I believe that most of them are calculated for machines much larger than our Mills. i work part time in a cabinet shop that has a Biesse 4 x 8’ CNC. It has pretty much nothing in common with our Mills. So, to say that ideal or recommended chip loads for the Biesse and the LM are similar seems to me to be nuts.
Finally, you mention that Fusion will do the calculation for you. I understand that the current versions of Vectric products will do that, too. I am using a version of VCarvePro that is 2 or 3 versions old. it does not have the feature and updating it is not in the cards.
The short answer: the lower the number, the lower the chip load. For more information i recommend this 2minute video, it explains it much better than I could. The explanation starts at 0:20. Most interesting point is, that the mill will rub instead of cut if the chip load gets too low, which is also highlighted in this video.
@JHahn Tks much, Jannik. Both of the videos were excellent. That said, for us, we also need to take into account our Mills. Taking too big a chip will put a lot of stress on the Mill. The second video mentioned stressing the bit, especially if the bit is small in diameter. We need to keep in mind the stress on the Mill components.
As an aside, some time ago I spoke to a Dewalt tech about my DW735 planer; specifically how I could get better blade life. He told me that, although it is counter intuitive, taking a 1/8" pass was preferred over taking a 1/16" pass. The thicker chip takes more heat away from the blades. Of course, this must be balanced with the load on the machine and the wear that can cause. It seems to be the same principle here.