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:

Y_max$ value

Recommended Posts

Greetings  everyone.

Related with y_max$ and y_min$  (lathe)

Why the C-Axis value is stored in the above mentioned variables?

Example output

(  | Max_Z position = +10.000 mm | )
(  | Min_Z position = -26.000 mm | )
(  | Min_Y position = -109.771 mm | )
(  | Max_Y position = +109.771 mm | )

(  | Rapid Time = 4 sec | )
(  | Feed Time = 41 sec | )
(  | Total Time = 45 sec | )
( #8. Face drilling - C axis  |  )
N15 G0 G40 G80 G13.1 G98
N20 G0 T1212
N25 G17
N30 M35
N35 M90  (Clamp Off)
N40 G28 H0.
N45 G0 G54 Z10. C12.
N50 X220.752 Y0.                                   ---->   Y=0   and there is no other Y Value
N55 G98 G97 S3820 P12 M03
N60 M08
N65 G83 Z-26. R-5. F687.6 M89  (Clamp On)
N70 C36.
N75 C60.
N80 C84.
N85 C108.
N90 C132.
N95 C156.
N100 C180.
N105 C204.
N110 C228.
N115 C252.
N120 C276.
N125 C300.
N130 C324.
N135 C348.
N140 G80
N145 M09
N150 M90  (Clamp Off)
N155 M05
N160 G28 V0.
N165 G28 U0.
N170 G28 W0. H0.
N175 T1212
N180 M30

Link to comment
Share on other sites

I have the feeling this is relative to what you are trying to accomplish....

It is directly from the MPLFAN post


#Y axis output and machining over part center:
# Output Y axis motion by setting 'Rotary axis/Y axis' in the NC
# parameter page.  This requires a valid Axis Combination in your machine defintion.
# y_axis_mch is set from the axis combination.
# Set 'Rotary axis/Y axis' in a machine with no Y axis (y_axis_mch = 0)
# to force linear/circular position moves in the XZ plane (g18).
# This allows machining over the part center.
#Caution: The machining must stay in the XZ plane at a Y fixed value
# when y_axis_mch = zero because no C (other than the Tplane) or
# Y positions are output!!!  This occurs when selecting C_axis/Cross
# Contour without 'y_axis_mch'.  Use Mill toolpaths for cross profiling.


  • Thanks 1
  • Like 1
Link to comment
Share on other sites

Greetings @JParis

I wish I had this info in my post :D
Thank you so much for pointing  this out

After few changes not it works flawlessly :)

      if rotary_type$ = 0 | rotary_type$ = 3,
        b1_ymax  = y_max$
        b1_ymin  = y_min$
Now only when I have y selected or no axis selected (while using mill operations)  buffer will fill min/max variables :)

Once again thank you @JParis

Kind regards


  • Like 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.

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.


  • 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...