Trigonometry help please, plunge depth for a v cutter!

Hello,

I am trying to calculate the required plunge depth for a v cutter needed to produce a given diameter of hole.

Can someone explain the formula I need?

Thanks!

--------------------------------------------------
EDIT:

Answer:-

Z = Depth of cut
d = Required diameter of cut
a = Cutter tip angle in degrees*
f = Flat spot
r = Tip radius

V Groove type cutter with no flat spot.
Z=d/(2*tan(a/2))

V Groove type cutter with flat spot.
Z=(d-f)/(2*tan(a/2))

V-Groove type cutter with a radius tip.
Z=r-(r^2-d^2/4)^0.5, for Z<=2r
Z=r+(d-2r)/(2*tan(a/2)), for Z>2r

Ballnose type cutter.
Z=r-(r^2-d^2/4)^0.5, for Z<=2r

* The TAN() function in some applications (such as Excel) require the angle to be expressed in radians, Not degrees. Convert degrees to radians - Radians = angleInDegrees x (PI/180)
So in excel the first formula above would become:-
Z=d/(2*tan((a*(PI()/180)/2))

I might be wrong, but you should be able to use an online calculator similar to this.....

Right Triangle Angle And Side Calculator

Just assume your cutter is lying on its side, therefore.....

In the 'side b' box (this is your experimental 'cut depth')

In the angle box (enter your V cutter angle divided by two)

the cut width will be the 'a' result multiplied by two.

Example....

say you have a 60 degree V cutter & you want to know the diameter of a hole if you go 2mm deep

enter '2' in the side b box
enter 30 in the angle box

Click calculate.

the hole will be side 'a' multiplied by 2...therefore 1.15 x 2 = 3.3mm

I realsie it's not exactly what you seek (fwiw, I suck at trig), but if nobody else chimes in, te above method should get you there! There may well be a dedicated calculator out there, but that was just a quick search/kludge! (kludge is my friend...we know each other so well)

best I can do
width of cut/2 x tan (cutter angle)
tan 30 = 0.577
Tan 45 = 1
Tan 60 = 1.732

Such that for a 60 degree cutter wanting a 3.. wide cut then 3/(2*1.732) = 0.866 ( in whatever units yo are using)

peter

Try the attached, just enter cutter angle and hole diameter required.

Thank you everyone for your input! I think I am slowly understanding :)

Depth of cut = (requiredDiameter/2) X TAN(cutterAngle X (PI/180))

So..
requiredDiameter = 10
cutterAngle = 60
(10/2) X TAN(60 X (3.141593/180)) = 8.66 plunge

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.

Attachment 10583

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!

Quote:

---

Originally Posted by 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.

Attachment 10583

---

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?

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?

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

Quote:

---

Originally Posted by 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

---

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.

Quote:

---

Originally Posted by Jonathan

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!)

Quote:

---

Originally Posted by cncJim

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.

Quote:

---

Originally Posted by cncJim

(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 :distracted:

Quote:

---

Originally Posted by Jonathan

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 :thumsup: