I would like to improve the speed and efficiency of TrueMill® by using a constant feedrate, how can I do that?
By default, the 2-axis TrueMill™ reduces the feed rates on inside arc moves. For most machining
applications, these feed rate changes are unnecessary, since TrueMill™ is designed to never exceed
the specified tool engagement. This means that the chip thickness can never become too large anywhere
along the TrueMill toolpath and there is no need to slow down anywhere. Therefore, by keeping the feed
rate constant on all TrueMill cutting moves, milling output can be significantly increased, the quality of
the cut will improve and tool life extended. This is especially the case on hard materials.
To output a constant feedrate on all 2-axis TrueMill® cutting moves, open the SURFCAM.INI file,
scroll down to the [DefaultNCParameter] section, change TMConstantRate=0 to TMConstantRate=1.
Understanding Constant Feedrates in TrueMill®
Extensive experimentation by Surfware and others who have published their results have shown that:
If the feed rate is to be varied at all, it should be increased whenever the actual tool engagement
is less than the user specified tool engagement.
From the point of view of tool engagement, there are 3 sections in a TrueMill toolpath.
- Cutting along the radius that makes up the circle set
- Cutting along the (almost) straight section than joins the circle sets
- D-Slotting
By current default, this is how SURFCAM Velocity3 SP2 addresses each of the above cutting
conditions and varies the feedrate:
- When cutting circle sets: the tool engagement is extremely close to that specified by the user.
Therefore the best feed rate is a constant feed rate. Our current default method varies the feed rate
downward according to the radius of each circle set. For small radii circle sets, this causes too
thin a chip to be formed, increases heat (due to rubbing, especially with hard materials) and reduces
performance.
- When cutting straight line segment that joins circle sets: the tool engagement is slightly less
than that specified by the user. Therefore the best feed rate is slightly above the user specified
feed rate. Our current default method does not vary the feed rate for a straight line segment,
resulting in excellent performance.
- When cutting D-Slots: the tool engagement can be much less than that specified by the end user.
Therefore, the best feed rate is above the user specified feed rate. Our current default method
varies the feed rate downward, not upward. This causes too thin a chip to be formed, increases
heat (especially with hard materials) and reduces performance (especially in corner picking).
For some applications, the constant feed rates have been experimentally shown to be 30% faster than the current default method of varying feed rates.
|