Jump to content


- - - - -

Tapping Speeds and Feeds


  • Please log in to reply
6 replies to this topic

#1 Smitty

Smitty

    Newbie

  • Members
  • Pip
  • 14 posts

Posted 16 May 2000 - 02:36 PM

Could someone please tell me how they select the correct speed and feed for tapping.We just got into tapping and it seems to me that mastercams feeds are very high.maybe I am missing something, Help

#2 Carbide Pete

Carbide Pete

    Newbie

  • Members
  • Pip
  • 6 posts

Posted 17 May 2000 - 01:19 AM

Tapping feed = Spindle speed x Thread Pitch

i.e, To cut an M12 x 1.75 thread at 600 rpm the feed would equate to:

600 x 1.75 = 1050 mm/min

Use your tap manufacturers cutting data for the correct peripheral speeds to use for the material being cut.
From my experience of tapping start at the lower end of the range given and work up from there until satisfactory results for thread size, finish and tap life are achieved.


[This message has been edited by Carbide Pete (edited 05-17-2000).]

[This message has been edited by Carbide Pete (edited 05-17-2000).]


#3 TOOLDEV

TOOLDEV

    Member

  • Customers
  • PipPip
  • 61 posts

Posted 17 May 2000 - 12:48 PM

MY POST IS SET SO THAT I INSERT THE
PITCH, AS THE FEED RATE, THIS WAY I JUST
ALTER THE SPEED AS REQUIRED, AND THE FEED
IS CALCULATED FOR ME. I FIND THAT METHOD
MORE FLEXIBLE OVER A RANGE OF DIFFERENT
MACHINES, I.E SOME CONTROLLERS NEED THE FEED
RATE PER REVOLUTION, AND OTHERS PER MINUTE.
THE POST WILL DO THE REQUIRED CALCULATION,
BUT IN MY TOOL FILES THE FEEDRATE IS GIVEN
AS A VALUE PER REVOLUTION.

REGARDS
PETER


#4 johns

johns

    Member

  • Members
  • PipPip
  • 103 posts

Posted 29 May 2000 - 02:21 PM

The accuracy of tapping depth is related to how quickly your CNC can decelerate, and then reverse. Even with floating tap heads, you may find it takes 4 revs to do this. By this time, the Z axis is already going up, or you may have bottomed the tap. On our CNCs, we use 300 RPM max to prevent the tap from overfeeding(bottoming) into the hole and breaking. If the Z axis raises too early, you may just pull the tap from the holder. Try a tapping cycle beside a fixed pointer, and see how many revs it takes to reverse at a set speed. Unless you have a synchronized spindle/feed type, you may have to use the canned cycle with the dwell at the Z depth and stay short by the number of threads it overshoots for the RPM you use. We use 300 RPM all the time & program it 1 1/2 threads short.

#5 Kevin B

Kevin B

    Newbie

  • Members
  • Pip
  • 6 posts

Posted 18 June 2000 - 04:10 PM

The feedrate for tapping on most cnc's is pitch times rpm. However some controls will specify that the pitch of the thread be programmed in the G84 canned cycle. 0.03125
for an 8-32 thread for example. And this can also be changed by specifying G94 or G95 before the canned cycle (feed in inches per minute or thou per rev). One way to see how much your machine will overtravel while tapping is to set the work co-ord above the part and watch the "distance to go" page while the machine taps. You will be able to see the distance to go value go from - to + if the machine overshoots the programmed depth. And you should be able to see by how much, because the machine will decelerate and reverse giving you a chance to see read the amount from this page. It's not %100 but it will put you in the ballpark. Only older or more primitive machines should experience this problem. You can also try programming high gear for tapping, and reduce the inertia so that the machine can reverse more quickly.
This is my experience anyway.


#6 Kevin B

Kevin B

    Newbie

  • Members
  • Pip
  • 6 posts

Posted 18 June 2000 - 04:16 PM

I forgot to add my question to the previous comment. How can I modify my post processor to output the feed for tapping to 5 decimal places? Some machines will accept 5 dec. places for rigid tapping. And obviously the more accurately the machine syncronizes the rpm and the feed of the spindle, the better the thread will be.
Any suggestions?

#7 Allan Brown

Allan Brown

    Advanced Member

  • In-House Solutions
  • PipPipPip
  • 2,168 posts

Posted 19 June 2000 - 03:29 AM

In the ptap postblock, the frplunge variable is usually used to output the tapping feedrate.  This variable is used in other cycles, so you should set up another variable to output the tapping feedrate, and format it with a decimal place format statement:

#in the format statement section
fs 15 0.5       #Decimal, absolute, 5 place

#in the format assignment section
fmt  F 15 frtap # Plunge feedrate

#in the ptap postblock
           frtap = frplunge
           n, *drillref, *sgdrill, pdrlxyrot, *depthout, *refout, *frtap

->This is example of the steps you need to take.  The actual code here is specific to another post, and will most likely not apply to you own post.