3 to 5 ax conversion smoothing

[LucasGC]

Hi all,

Was hoping for more of an explanation for this option. I've been using it with distance 5(mm) and it's helped the transition but I'm not sure what it affects. 
Does this mean that the movement it takes to get to the next angle is spread out over 5mm? Or is it averaged every 5mm and blended?

Does this change the tolerance at all? 

Any extra info on this option would be appreciated

Thanks

[gcode]

17 minutes ago, LucasGC said:

Hi all,

Was hoping for more of an explanation for this option. I've been using it with distance 5(mm) and it's helped the transition but I'm not sure what it affects. 
Does this mean that the movement it takes to get to the next angle is spread out over 5mm? Or is it averaged every 5mm and blended?

Does this change the tolerance at all? 

Any extra info on this option would be appreciated

Thanks

I believe it means a point is being added every 5mm, whether it is needed to meet the defined tolerance or not.

This may or may not add rotational output, depending on the angular changes between the points.

I have found I get much smoother motion on 5X swarf toolpaths on our big Okuma if I force a small stepover.

for example,

.001 tolerance/.008 distance will yield a  much smoother tool path than a .0002 tolerance setting with distance unchecked

[huskermcdoogle]

1 hour ago, gcode said:

.001 tolerance/.008 distance will yield a  much smoother tool path than a .0002 tolerance setting with distance unchecked

This is because the linear acceleration caused by the angular change from point to point is less when you break it up finer.  This is mostly evident when you get further from the center of rotation, and your "small" angular movements causes large linear (XYZ) displacements.  The finer you make the tool paths the less violent, and less blocky the linear moves become.  In my experience, on head head machines, this is a big challenge on all paths.    

[gcode]

3 minutes ago, huskermcdoogle said:

In my experience, on head head machines, this is a big challenge on all paths.   

our Okuma is a table/table trunion with a 1000mm square table table.

Lathe A axis displacement can be quite violent.

[huskermcdoogle]

7 minutes ago, gcode said:

Lathe A axis displacement can be quite violent.

Assuming you meant large.

Yeah the bigger the trunnion machine, the more accurate the rotaries need to be....  What is the least increment for your rotaries on that machine?  4, 5, or 6 places?  Assuming .001 degrees and 500mm radius, you are talking .009mm displacement.  I would hope you have at least 4 places commanded on your rotary.

[LucasGC]

1 hour ago, gcode said:

I believe it means a point is being added every 5mm, whether it is needed to meet the defined tolerance or not.

This may or may not add rotational output, depending on the angular changes between the points.

I have found I get much smoother motion on 5X swarf toolpaths on our big Okuma if I force a small stepover.

for example,

.001 tolerance/.008 distance will yield a  much smoother tool path than a .0002 tolerance setting with distance unchecked

Thanks,

I have a Thermwood and I've been told to give it lots of code, so I'll have to try that. I wonder what difference this would make on a 3 to 5 ax conversion - after filtering the toolpath in the 3d scallop, then adding max step to the 3 to 5 would break it back down

[Aaron Eberhard]

All of the above points are true, but to get your original question on the smoothing option available to Convert to 5 Axis collision control option (and also Change Tilt Angle), what the tilt & rotary fields allows you to do is smooth out tilt relative to a selected axis.  Say you're machining a cone with vertical cut outs.  It's oriented so you're rotating around the Z axis.  You may not want it to tilt into the cut outs (or at least, don't do it abruptly), you would set Rotary Axis to Z, then smooth the Tilt Angles.  The values will be how much it's allowed to smooth the angles away from the original orientation.   Maybe you'd say that the tilting is allowed to smooth motion out by ±15°.  If it needs more tilt than that, it's going to tilt to clear, but it won't bother unless it's going to have to tilt more than 15°.   You probably wouldn't need any rotary adjustment in this case since you're just tilting around a cone and it doesn't try to change the lead/lag, but the same principle applies for that.

The other option here is to just to specify a blending distance like you've done.   That will allow you to work backwards from where the tilt is and start applying it early.  You'll still end up with the maximum needed tilt, but instead of applying it only when you need it, it will taper your tilt so it starts tilting X distance (in your example, 5mm) before it really needs to be tilted.   So, picture a cut where you're perfectly vertical for most of it, but have to tilt 15° for an undercut that's 10mm long on one side of the pocket.   Out of the box, the toolpath will remain vertical until you're going to collide, then it will start tilting, truly minimizing the motion, but possibly at the expense of having jerky motion on your machine.  If you enter a blend distance, it'll figure out where it needs to start tilting, then work back by 5mm and start tilting there.  You'll still end up safely clearing the part, but instead of that 15° of tilt happening over 10mm, it'll happen over 15mm.