Hmm - is it unrealistic to use feed/speed calculators on home built machines?

[Rufe0]

I like to use this calculator to calculate the Tangential cutting force, that is how hard the machine is pushing the bit sideways through the material. In my experience you can bet any speed/feed/DOC/WOC combination that exceeds a certain amount (you will have to find experimentally on your machine) will pretty much always cause chatter or be bad. The exception is smaller diameter longer cutters will always be worse than shorter fatter ones, but that might be less important on a machine that's not very rigid. Also obviously the smaller the diameter the cutter the more likely it is to snap completely, so watch your tangential cutting force very carefully.


http://www.kennametal.com/en/resourc...and-power.html




One thing I have to mention, if you where hand coding you would have complete control over the feed rate. So you can make it slower for parts where the WOC increases (inside corners for example) and speed it up for the other parts.




I almost feel I should start a movement or protest or something. Maybe I'll make a website, banspeedsandfeeds.com. Speeds and feeds are an artifact left over from the days before CNC. They shouldn't be used in CNC software and someone should really do something about it.... lol


What we should be using is surface speed, that is how fast the tip of the cutting bit is traveling across the surface of the material per minute. Which is tool circumference(Pi*dia) times the spindle RPM, (Pi*dia)*RPM. This is the primary cause of heat and it's obvious why when you think about it. Rub any two things together even smooth things and you get friction, friction means heat, how much heat is directly proportional to how fast your moving them. The frictional coefficient of the material is the thing that effects this so that will dictate your spindle speed.


Then there is chip load per tooth, this is how big a bite each tooth takes. This is important to make as big as possible so your tool lasts as long as possible. Taking a small bite or a big bite makes no difference to the tooth it wears the same either way. So if you take fewer bigger bites your tool will last longer. However there is a limit of course, bigger bites take more power and more force. Power isn't usually the limiting factor, most people have way over powered spindles for what they are doing. Force can be an issue, a tiny little tooth will snap off more easily than a big one. The hardness of the material makes a big difference. You can generally find information from the tool manufacturer on chip load, then you need to do some maths. For example lets say they recommend 0.025mm chip load per tooth, you have a 3 flute cutter. With 3 flutes/teeth you need to travel your chipload distance * 3 every revolution so 0.075mm per revolution. Your surface speed calculation says you need 10,000rpm spindle speed. So your feedrate will be 0.075mm*10000rpm = 750mm/min.


WOC is important but only really in terms of power and force required for a wide cut is obviously more than a thin cut. Same for DOC. Where you get a problem is when you try to do both a wide and deep cut. Then your going to have problems clearing the chips. However it shouldn't really ever come up if you've done your surface speed and chip load calculation correctly because your machine won't have the rigidity and power for both a wide and deep cut. Not on home hobby machines anyway.


In any case you should try to take as deep a cut as possible so that you wear the tool evenly, it's no good buying a 50mm long endmill if you only ever use the first mm of it.

WOC 30% of the diameter is generally considered to be 'safe' from chip clearing problems. You can of course go wider without problems, especially if the cut isn't deep. But again if your really driving the tool as hard as is recommended(chipload) then it's unlikely your machine will have the balls for a wide cut. You might even have to go much smaller on the WOC.