Trigonometry help please, plunge depth for a v cutter!

[EddyCurrent]

With Excel you have to remember that the TAN() function uses Radians for the angle so the PI()/180 is to change the angle into radians.
So if you use just a calculator it would be (requiredDiameter/2) X tan(angle in degrees)

These are the angles reffered to.

[cncJim]

Ah I see, thanks for that eddy, good to know!

I am using the formula with PHP for a web application and the TAN() function uses radians so I am sorted!

[cncJim]

With Excel you have to remember that the TAN() function uses Radians for the angle so the PI()/180 is to change the angle into radians.
So if you use just a calculator it would be (requiredDiameter/2) X tan(angle in degrees)

These are the angles reffered to.

Just spotted your diagram with the angles, I think i had the wrong angle in mind...

So...if my cutter has a 45 degree angle at the cutting head (top of your diagram) that would mean the angle I need to use with the formula would be 67.5?

(180-45)/2 = 67.5

Is that correct?

[Jonathan]

V-cutters are generally specified by the included angle, i.e. the angle at the tip. In that case the formula is:

Z=d/(2*tan(a/2))
Where:
Z=depth of cut
d=diameter cut
alpha=tip angle, as above.

So for example, lets say you have this cutter:
4x40°x0, 1mm V-type Solid Carbide Engraving Tool Cutter f. CNC Engraving Machine | eBay

The angle is 40 degrees, so suppose you want to cut 1mm wide:
Z=1/(2*tan(40°/2))=1.37mm

However, there's an error since we've assumed the cutter has a sharp point when in reality it's got a flat, which makes things marginally more interesting, hence why I decided to make this post.

The formula you now need is as follows:
Z=(d-f)/(2*tan(a/2))

Using the same example, the tip flat is 0.1mm so:
Z=(1-0.1)/(2*tan(40/2))=1.24mm

There's also the chance that you're using V-cutters with a radiused tip.
Now the formula you'd need is:
Z=r-(r^2-d^2/4)^0.5, for Z<=2r [Note this is also valid for ballnose cutter]
Z=r+(d-2r)/(2*tan(a/2)), for Z>2r

Where r=tip radius.
e.g. suppose this tool:
3x20°x1mm V-type with radius Engraving Cutter graver HM for CNC engraver machine | eBay

It's 20°, and 1mm tip radius so a=20, r=1. Lets say you want to cut 2.5mm wide:
2.5>2*1, therefore:
Z=1+(2.5-2*1)/(2*tan(20/2))=2.42mm
Suppose you want to cut 1mm wide:
1<2*1, therefore:
Z=1-(1^2-1^2/4)^0.5=0.13mm

Edit: If you don't have a calculator to hand, then using google is a quick way to evaluate it, e.g.
http://lmgtfy.com/?q=1%2B(2.5-2*1)%2...20%2F2+degrees))
You could of course just draw it in a CAD program, but where's the fun in that?

[Ulsterman]

Touch the tool off at the required Dia that you can measure on the part ---- and program machine to cut to the Face -no trig needed but approach move should include room for the tip -very common practice on combo tools

[cncJim]

Touch the tool off at the required Dia that you can measure on the part ---- and program machine to cut to the Face -no trig needed but approach move should include room for the tip -very common practice on combo tools

Thanks for the advice Ulsterman, but in this case I really am after the trig as I am coding an application to produce g-code.

[cncJim]

V-cutters are generally specified by the included angle, i.e. the angle at the tip. In that case the formula is: ......

Thank you Jonathan, that is excellent information, just what I need! Will take me a little time to fully digest but will be worth it.

I didn't consider the flat spot at all. Wouldn't have been a disaster, but wouldn't have been correct either!
I asume if I use an insert v bit (such as CNC V Groove Miter Fold & Signmaking Insert Router Bit by Amana Tool) then I could just use Z=d/(2*tan(a/2)) as there would be no flat spot?

The radiused tip/ballnose cutter was also a great thought. I was only considering supporting v cutters but I think you have changed my mind.

Thanks!

(haven't seen "LetMeGoogleThatForYou" before! Almost spat coffee on my keyboard when I clicked it!)

[Jonathan]

I didn't consider the flat spot at all. Wouldn't have been a disaster, but wouldn't have been correct either!
I asume if I use an insert v bit (such as CNC V Groove Miter Fold & Signmaking Insert Router Bit by Amana Tool) then I could just use Z=d/(2*tan(a/2)) as there would be no flat spot?

There's always going to be a flat of some sort, but for the tool you linked to I expect it would be neglegible. You might as well use the formula with the flat in your program, and just set f to 0 if the flat is insignificant as that results in the same formula as for without a flat.

If you've got the tool to hand, then one way to measure the flat is to spin it round and move the Z-axis down until it just touches. Retract the Z-axis and measure the diameter of the circle left - that's your f.

(haven't seen "LetMeGoogleThatForYou" before! Almost spat coffee on my keyboard when I clicked it!)

It's temping to link people to that quite often

[cncJim]

There's always going to be a flat of some sort, but for the tool you linked to I expect it would be neglegible. You might as well use the formula with the flat in your program, and just set f to 0 if the flat is insignificant as that results in the same formula as for without a flat.:

Thats exactly what I will do, thanks again Jonathan