Just curious what everyone is using to calculate their speeds and feeds? I have the Lead, but have been using Carbide Create for my toolpaths. The default setting on there are working fine, but they seem really really slow to me. I see videos of other making cuts and I am not going anywhere near that quick. I have seen people recommend Mill Right and FS Wizard apps.
feeds and speeds are important enough that you can charge money for a good calculator (-: lets start with the basics...... SFM = Surface Feet Per Minute : each material has a preferred range of speeds at which it likes to be cut. BUT this also depends on the cutting tool material because heat comes into play. solid carbide can cut much faster then HSS because it can tolerate more heat and abrasion. Lists of SFM for various materials will usually give a low to high range. Tool diameter and RPM : we combine these two to get the SFM we want. RPM = SFM * Pi / diam CL = chip load : this is how much material is removed by each tooth. usually 2 to 10 thou or 0.05 to 0.08mm TN = number of teeth : this affects feedrate, a multitooth cutter can take more per rev than a single tooth cutter because the teeth are each doing the chipload depth. so finally feedrate = RPM * CL * TN so google for a table of SFM values for various materials and go from there, but NOTE: 1 - in softer materials avoid small diameter bits with high tooth counts. anything under 1/4" should be 2 or 1 flute to allow space for the chips to get out. 3mm, 4flute cutters exist, do NOT use them in a router, they are for titanium with water spray coolant that makes sure the chips are cleared. The water spray can easily be 1500psi, this is *that* important. 2 - never make dust. if you are cutting wood and getting dust you are cutting way too slow. the chips should be like coarse sugar grains. 3 - try hard to never recut a chip. This creates heat and surface roughness and wears out the tools quickly. Picture this, you have a nice smooth aluminum plate. you place on it a chip (produced from some previous cut) and you try to cut the chip in half with a craft knife. Now, before the knife cuts through it there is enough pressure for the chip to dent the smooth surface. AND you have to cut through the cut before you can cut the parent material which can easily double the workload. of course the various web sites can help you find starting numbers for feedrates but ultimately it is down to your machine so do make notes as you go along, and do some experiments from low SFM to high SFM. also vary the cut depth, you may be able to do 3 shallow fast cuts faster than 1 deep cut and get much better results as well as saving time.
Good info, thanks! I am pretty familiar with all the calculations and have used them when putting a new tool into carbide create. Just wasn't sure what everyone else used. I have seen all sorts of different tools; apps, charts, calculators etc. I find the charts to be lacking as it is hard to put all the different options and combinations on a chart. Found a few threads on here with people giving input, but they are a few years old. Just wanting to see what people were using and if a certain tool out there worked better than another. But I think you are correct in that all this is baseline, and tweak as needed to see what works best on your machine. I have found that using the Amada data from tools today works pretty well. They list out recommended RPMs, CL, SFM for generic materials. DOC would usually be no greater than half the diameter of the bit
