12
$\begingroup$

How are spindle speeds calculated for a drill bit?

I've seen dozens of charts that highlight the rpm that should be used for specific drill bit types, bit diameter, and material. However, what if my chart doesn't have the particular type of material or bit that I am using? I'd also like to have some intuition to know if the chart looks right or wrong.

Upon some quick research, it appears that the "cutting speed" is what is ultimately needed for a particular material. I assume the cutting speed for each material must be looked up? Is there a standard or "go-to" place to find these? Then, information about the drill bit can be used to determine spindle speed. Again, what if I'm using a big hole saw or circle cutter, and it's not listed? How do I model the bit to use the cutting speed to determine rpm (for a given material of course)?

I'd also like to know to calculate feed speeds for a drill or mill, but there are presumably more variables. It is probably better answered in another question.

$\endgroup$
3
  • $\begingroup$ Are you doing this by hand, or programming a machine? (I could only help with the by hand type.) $\endgroup$ – George Herold Jan 22 '15 at 0:29
  • $\begingroup$ I'd like to get into CNC milling, but my primary use right now is by hand. $\endgroup$ – Justin Trzeciak Jan 22 '15 at 1:27
  • $\begingroup$ @JustinTrzeciak as a manual machinist then it isin't so important were to start then. I like 1000 rpm for a 3/8 HSS jobber in mild steel and adjust from there. Use sound, feel, and sight to tweak your speed and feed as necessary. $\endgroup$ – Corey Sep 28 '18 at 19:24
9
$\begingroup$

You are correct that the cutting speed of the material is what determines the rpm for your drill-bit. This actually makes the calculation very simple.

$$ \text{Spindle speed (RPM)} = \frac{\text{Cutting speed}}{\text{Circumference}} = \frac{\text{Cutting speed}}{π \cdot \text{Diameter}} $$

The thing you need to be careful of is the units of cutting speed and diameter. For example:

  • Metric: If your cutting speed is in $m/min$ and your diameter is in $mm$ then you need to multiply your cutting speed by 1000 so that it is in $mm/min$
  • Imperial: If your cutting speed is in $ft/min$ and your diameter is in $inches$ then you need to multiply your cutting speed by 12 so that it is in $inches/min$

For more information see spindle speed calculations on Wikipedia.

$\endgroup$
2
  • $\begingroup$ So does this simple formula hold true for any bit, or just simple twist bits and end mills and such? Will the same work for hole saws, Forstner bits, spade bits, etc? $\endgroup$ – Justin Trzeciak Jan 22 '15 at 2:44
  • $\begingroup$ Pretty much, yes, but note that some bits are not suitable for some materials or only suitable at slower speeds and/or with lubrication. The larger bits you mentioned will have slower spindle speeds because of the larger diameter, if in doubt start at 20% slower speed and increase if all seems fine. Be careful with small bits though as you can snap them very easily if they are too slow and not cutting fast enough. $\endgroup$ – jhabbott Jan 22 '15 at 16:17
3
$\begingroup$

I don't know that there's much materials science behind those charts. I suspect they are amalgamations of collective experience and wisdom.

As a general rule, the bigger the bit the slower the speed should be. So there's an inverse relationship between acceptable maximum speed and the size of the hole that's being cut.

Obviously, you can cut a small hole at a small speed if you're patient. But most folk would rather move on to the next step and are looking for the fastest speed that they can cut that particular size hole with.


So why is that general rule in place then? As a bit grinds against a particular material, it's going to generate heat from the frictional forces involved. Bigger bits mean bigger surface areas so you therefore have greater amounts of heat. That heat generation is multiplied by the rotational speed of the bit as it reflects the amount of area ground per period of time.

So by slowing the really big bit down, you're decreasing the amount of surface area covered in the same amount of time. That keeps the amount of frictional heat down (since it can dissipate more easily) and reduces the chances that you'll destroy the temper on the bit.

$\endgroup$
1
$\begingroup$

In general there will be an optimal cutting speed and feedrate for any given combination of tool material and the material being machined.

This is often drive by the heat heat generated by cutting but factors such as toughness, ductility and tool geometry will also have an effect.

Recommended spindle speeds for drills, mills etc are really just translating the linear cutting speed into a rotational format which is more convenient to work with.

In reality there are all sorts of compromises involved and quoted figures are often an average value for general use. For example you might use a low cutting speed and heavy fed rate to get the fastest rate of material removal but a higher speed with lighter feed for a better final finish. Similarly recommended tools speed are often a compromise between material removal rate and tool wear.

The specific machine characteristics also matter a lot for example a basic pillar drill with an AC motor and pulley drive may simply not have enough torque to run a large hole saw at the optimum speed.

Overall it isn't too difficult to tell when a speed is 'right' for a particular job and my experience is that the tables are very useful to get it pretty much right in most circumstances but there is quite a wide margin to adjust them to fit the needs of a particular job.

$\endgroup$
0
$\begingroup$

They say a picture is worth a thousand words, so here's a picture of the "Sweet Spot" for various machining operations including drilling, milling, and turning:

enter image description here

Now you can see what going a little faster or slower on feedrate or spindle rpm is doing for you.

RPM's are all about heat. If the cutter gets too hot, it softens and rapidly dulls. Feedrate is all about the ability to clear the chips. If they pack in the flutes too much and jam, the cutter breaks.

Those are the basics. There's a lot more too it than that, and you can learn a lot more from this free feeds and speeds course.

$\endgroup$
1
  • $\begingroup$ Welcome on the site! Your links doesn't point to images, they point to irrelevant html content (as I can see). Could you please somehow fix them, or it is only by me so? $\endgroup$ – peterh Jun 1 '19 at 19:16
0
$\begingroup$

Rotational speed is a by-product of the desired result and is generally a compromise to optimise other factors.

To give a simple example of why this is, consider that a twist drill cuts across its entire frontal surface. While the rotational speed of the bit is constant across the face, the linear speed varies from 0 (at the centre) through angular rotation multiplied by circumference (at the periphery). This continuum of speeds cannot all be correct, and some other variable must determine the selection.

The values provided by tables and formulae are necessarily approximations of the true state and this is why so often guidance is given to try a setting and then adjust it to improve the sound, for example, of the cut.

In 1906, F. W. Taylor presented On the art of cutting metals as the first rigorous explanation for setting up machine tools. This description of the process used to determine the principles for selecting cutting speeds remains an empirical marvel in engineering.

So far, this has ignored your second important variable, that of how fast to feed the drill into the material to complement the rotational cutting motion.

In many cases, rather than calculating the speed, select the value the tool manufacturer recommends for the application closest to what you require. This takes advantage of the century of experimentation and design embodied in the humble twist drill.

$\endgroup$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.