Re: [CAD_CAM_EDM_DRO] CNC drilling

Hello Ron,

Here is the article that I referenced in my previous response.

http://www.desktopcnc.com/drill/optimize.htm

Tom Hubin
thubin@...

*******************

Tom Hubin wrote:

>
> Hello Ron,
>
> I use a formula from a 2 page article. I have a copy I can send to you
> but will try to find it on the web first for proper credit.
>
> They suggest 0.017 * N * D * S = F
>
> where:
>
> N = number of flutes
> D (inches) = drill diameter
> S (rpm) = spindle speed
> F (inch/minute) = feedrate
>
> This works if you have enough power but is a problem for a large bit
> on
> a small machine. I have found that my Sherline 5410 can mill and drill
> up to about 4 cubic inches per hour or 1/15 cubic inches per minute.
> Attempting much more than that usually results in the steppers or the
> spindle coming to an abrupt halt.
>
> Vrr = F * D * D * pi / 4
>
> where:
>
> Vrr (cubic inches per minute) = volume removal rate
>
> So I choose spindle speed for my machine's max of 2800rpm, calculate
> feedrate, calculate volume removal rate. If the volume removal rate is
> greater than 1/15 cubic inches per minute then I scale down the
> spindle
> speed and the corresponding feedrate.
>
> I should also limit surface speed to recommended values but that seems
> to never be necessary on my little machine.
>
> This usually works for me.
>
> Tom Hubin
> thubin@...
>
> ***************
>
> Ron Ginger wrote:
> >
> > I just finished a new Jet mill conversion. In the past I have always
> > been afraid to drill under CNC control- Ive let the program single
> > step
> > to location, then I operate the quill by hand.
> >
> > What feed rates are used for CNC drilling? Do you calculate chip
> load
> > like you would for an end-mill? What is a reasonable chip load for a
> > drill? I suppose that varies by drill diameter?
> >
> > ron ginger