Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

TAPPING


Bama
 Share

Recommended Posts

Whats the best way to tap in mastercam never done it ive always threadmilled it but its a M2.5 x .45 thread and if I could tap it it be nice or would you single point it and call it a day? just really wondering how other people do stuff really. And how to tap in mastercam

Link to comment
Share on other sites
On 9/11/2019 at 5:46 PM, Bama said:

Whats the best way to tap in mastercam never done it ive always threadmilled it but its a M2.5 x .45 thread and if I could tap it it be nice or would you single point it and call it a day? just really wondering how other people do stuff really. And how to tap in mastercam

What machine?

On mills:

  • G84 is output (by default) for tapping, when you select the "Tap" cycle in the "drill parameters" page.
  • G84 typically uses a "floating tap head", which allows a tiny bit of axial "float". This is used when the machine reverses the spindle at the bottom of the hole.
  • More modern machines use a function called "Rigid Tapping", where the spindle rotation uses an encoder (and orients, typically with M19) to track the rotation position of the spindle, and the machine synchronizes the Z-Axis motion, so that it will tap successfully with a rigidly mounted tap.
  • Many machines will have different codes to indicate "rigid tapping" vs. "non-rigid tapping". For example, G84 for non-rigid (standard), or G84.2 for Rigid Tap.
  • Some machines have the same "G84" canned cycle call, but precede the G84 G-Code line, with M29 and the Spindle Speed for the tap. For example: M29 S350
  • In all cases, you must synchronize the Spindle Speed (RPM) with the Feed value. However, there are two ways to do this:
  1. Your machine can be in Feed per minute (Inches per Minute on an Inch Machine [G20], or Millimeters per Minute on a Metric machine [G21]). Feed per minute is typically indicated with G94. When you are in Feed per minute mode, the Feed value will always be: Thread Pitch x RPM. The calculation for Thread Pitch is 1 / # of Thread Per Inch.
  2. If you are in Feed per Revolution mode, then your "Feed value" may be specified as "E", instead of "F", or it may remain "F", but the value will always "equal the pitch of the thread". Because you are in G95 mode, you get better ability to adjust the actual cutting speed, because all you are doing is modifying the RPM value. Since RPM is always an integer value on machines, Feed per Revolution gives you the easiest ability to adjust to a "true pitch" value.
  3. Be careful when using Feed per Minute, as you can pick combinations of Feed and RPM, where the Feed value is "rounded or truncated", because the number of digits of precision allows for the "F" value, is not precise enough to give an accurate feed value. Example: Pitch of .08333333, where the F value is rounded to 3 decimal places (.083) is not an accurate pitch value. Where possible, I increase the F output to 4, 5, or even 6 decimal places, if the machine allows it.
  • Thanks 1
Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • Recently Browsing   0 members

    • No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us

×
×
  • Create New...