Jump to content
OMRON Forums

5-axis Mill using PMAC (G-code)


Recommended Posts

New User here ,

I'm using a 8-axis PMAC machine controller with G/M code gui. I have been using the machine for quite some time indexing into position and static drilling aerospace parts , (5-axis motion) XYZBC rotary tilt

(B) being the 4th axis and (C ) being the 5th axis. My problem is that I have developed a post that is using all 5-axis motion to laser cut a profile

or contour but the controller is treating the radial axis in degrees p/minute and the linear axis in feedrate mode G94 "cutting mode" I need to maintain constant surface speed. When executing just a linear move x,y,z the machine traverses in the programmed feedrate , but when there is a B or C move associated in the same line its feedrate is a fraction of the programmed speed.

Best Regards.


Link to comment
Share on other sites

  • Replies 4
  • Created
  • Last Reply

Top Posters In This Topic

This is a perplexing problem , This is a simple 5-axis rotary tilt milling machine and I just want control of the 5-axis surface speed.

I would hate to think that I need to program a feedrate for each line of code ? XYZCB how can I program 1 feedrate (F50) for example and have all of the axis move to maintain part surface feed ?

Any advise would be helpful.



Link to comment
Share on other sites

The fundamental problem you have is that when you are programming the axis moves here, the PMAC has no way of knowing what the tool-tip speed (aka part surface feed) is. It has no knowledge of the interrelated geometry of the axes.


A controller that permits you to program directly in the tool-tip coordinates to get the positions and speeds of the tip must have knowledge of the machine geometry and the capability to convert these tool-tip coordinates to the underlying axis coordinates. This conversion is known as the inverse kinematic transformation (a term more commonly used in robotics).


Unfortunately, the older non-Turbo PMAC you are using does not have the capability to perform this conversion. The newer Turbo PMAC and Power PMAC controllers do have this capability, and many people do use it for tool-tip NC programming.


If you have a controller that cannot do the conversion (which is quite common), your CAD/CAM system must do it, for speeds as well as positions. Since the tool tip speed can vary continuously as the rotary axes move even for constant Cartesian axis speed, you must split the moves into very small pieces with potentially a different speed for each little move block. It is very common to use "inverse time mode" in this situation, with a new F value on each line representing the reciprocal of the move time. (PMAC typically reads this in a subroutine and sets a move time equal to 60000/(Fvalue).

Link to comment
Share on other sites

Thank you for the reply , When powering up my GUI indicates that Im using PMAC-NC 5.1e and when I enter the PEwin the PMAC prom indicates 1.16A , I am assuming this is not PMAC turbo , but how can I check what PMAC is installed on this pc ?


Thanks again.

Link to comment
Share on other sites

This topic is now closed to further replies.

  • Create New...