Page 1 of 2 12 LastLast
  1. #1
    cncJim's Avatar
    Lives in Reading, United Kingdom. Last Activity: 3 Weeks Ago Has been a member for 4-5 years. Has a total post count of 170. Received thanks 15 times, giving thanks to others 32 times.
    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))
    Last edited by cncJim; 06-11-2013 at 12:58 PM.

  2. The Following User Says Thank You to cncJim For This Useful Post:


  3. #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)
    Last edited by HankMcSpank; 05-11-2013 at 01:18 PM.

  4. #3
    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

  5. #4
    Try the attached, just enter cutter angle and hole diameter required.
    Attached Files Attached Files
    Last edited by EddyCurrent; 05-11-2013 at 02:30 PM.

  6. #5
    cncJim's Avatar
    Lives in Reading, United Kingdom. Last Activity: 3 Weeks Ago Has been a member for 4-5 years. Has a total post count of 170. Received thanks 15 times, giving thanks to others 32 times.
    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
    Last edited by cncJim; 05-11-2013 at 03:31 PM.

  7. #6
    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.

    Click image for larger version. 

Name:	v cutter.JPG 
Views:	132 
Size:	6.4 KB 
ID:	10583

  8. The Following User Says Thank You to EddyCurrent For This Useful Post:


  9. #7
    cncJim's Avatar
    Lives in Reading, United Kingdom. Last Activity: 3 Weeks Ago Has been a member for 4-5 years. Has a total post count of 170. Received thanks 15 times, giving thanks to others 32 times.
    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!

  10. #8
    cncJim's Avatar
    Lives in Reading, United Kingdom. Last Activity: 3 Weeks Ago Has been a member for 4-5 years. Has a total post count of 170. Received thanks 15 times, giving thanks to others 32 times.
    Quote Originally Posted by EddyCurrent View Post
    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.

    Click image for larger version. 

Name:	v cutter.JPG 
Views:	132 
Size:	6.4 KB 
ID:	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?

  11. #9
    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?
    Last edited by Jonathan; 05-11-2013 at 07:30 PM.

  12. The Following User Says Thank You to Jonathan For This Useful Post:


  13. #10
    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

Page 1 of 2 12 LastLast

Similar Threads

  1. Replies: 0
    Last Post: 05-12-2013, 07:28 PM
  2. Will this end-mill plunge?
    By Tenson in forum Tool & Tooling Technology
    Replies: 10
    Last Post: 26-02-2013, 04:40 PM
  3. Z axis not cutting to required depth
    By dinasblu in forum Machine Discussion
    Replies: 10
    Last Post: 02-07-2012, 05:38 PM
  4. Taking the plunge
    By Robin Hewitt in forum Computer Software
    Replies: 0
    Last Post: 14-05-2010, 01:22 AM
  5. End mill depth 'stop' rings
    By HankMcSpank in forum Tool & Tooling Technology
    Replies: 10
    Last Post: 24-02-2010, 02:03 AM

Bookmarks

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •