View Full Version : Trigonometry help please, plunge depth for a v cutter!

cncJim

05-11-2013, 11:58 AM

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))

HankMcSpank

05-11-2013, 12:15 PM

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

Right Triangle Angle And Side Calculator (http://www.csgnetwork.com/righttricalc.html)

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)

ptjw7uk

05-11-2013, 01:09 PM

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

EddyCurrent

05-11-2013, 01:28 PM

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

cncJim

05-11-2013, 01:47 PM

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

EddyCurrent

05-11-2013, 02:11 PM

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.

10583

cncJim

05-11-2013, 02:19 PM

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

05-11-2013, 03:04 PM

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.

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?

Jonathan

05-11-2013, 06:25 PM

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:

4x40Â°x0, 1mm V-type Solid Carbide Engraving Tool Cutter f. CNC Engraving Machine | eBay (http://www.ebay.co.uk/itm/4x40-x0-1mm-V-type-Solid-Carbide-Engraving-Tool-Cutter-f-CNC-Engraving-Machine-/290997516817?pt=UK_Home_Garden_PowerTools_SM&hash=item43c0cdba11)

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:

3x20Â°x1mm V-type with radius Engraving Cutter graver HM for CNC engraver machine | eBay (http://www.ebay.co.uk/itm/3x20-x1mm-V-type-with-radius-Engraving-Cutter-graver-HM-for-CNC-engraver-machine-/290979187674?pt=UK_Home_Garden_PowerTools_SM&hash=item43bfb60bda)

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)%2F(2*tan(20%2F2+degrees))

You could of course just draw it in a CAD program, but where's the fun in that?

Ulsterman

06-11-2013, 01:32 AM

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

06-11-2013, 10:57 AM

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

06-11-2013, 11:11 AM

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 (http://www.amanatool.com/cncroutingdetails/rc-1028.html)) 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

06-11-2013, 01:43 PM

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 (http://www.amanatool.com/cncroutingdetails/rc-1028.html)) 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 :distracted:

cncJim

06-11-2013, 02:41 PM

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:

Powered by vBulletin® Version 4.2.3 Copyright © 2018 vBulletin Solutions, Inc. All rights reserved.