[1ctoolfool]

Ok, this is a test anyone can do easily.
Using the same 3/16" endmill feed at 5000rpm 50ipm at .005" depth in aluminum.
one cut is a straight line in X with one dead stop in the middle.
one cut is a straight line in Y with one dead stop in the middle.

The x direction cut mark(s) where the tool stops is easily removed with a scotch brite pad to be invisible to the naked eye.

The Y direction cut cannot be easily "scotch brited" away and resembles the "coining" that Mr. Flat is complaining about. Approximately .0001" depth marks.

Why don't these cuts produce identical results?

[Geof]

...The x direction cut mark(s) where the tool stops is easily removed with a scotch brite pad to be invisible to the naked eye.

The Y direction cut cannot be easily "scotch brited" away and resembles the "coining" that Mr. Flat is complaining about. Approximately .0001" depth marks.

Why don't these cuts produce identical results?

Because the Y change in direction puts and impulse into the machine in the same direction that the head 'nods'; the X change in direction is at ninety degrees and does not excite the resonant 'nodding' as efficiently.

[ktm666]

haas machines are less than perfect at harsh stops with flat or bullnose cutters. just a fact of rigidity.

[1ctoolfool]

also occurred to me the y axis is carrying much more mass and this may contribute

[Geof]

also occurred to me the y axis is carrying much more mass and this may contribute

That is a good point; when X change direction only the table mass is involved but Y includes all the X axis stuff. So the 'Y' impulse is probably double and in the correct direction to excite the nodding most efficiently.

I guess it would be possible to experiment with different masses bolted to the table. Do a cut with something clamped directly to the table, then load the table to its maximum capacity and do a cut; I would expect to see some difference.

[Andre' B]

This be why when finish and accuracy really matter you get a bridge mill instead of a C-frame.

[mactec54]

Hi 1ctoolfool

I'm surprised the coining/marks left by the cutter are not greater as if you check the X-Y & Z axes you will have .001 to .0015 slop in the linear rails this is one of the problems on these Haas machines which give you not such a good finish on your work everything is moving a round while cutting

[gerard1959]

In 13.14 series software Haas added Setting 191 Default Smoothness to the settings page of the control which allows you to control the machines acceleration rates, which allows you to control the smoothness of the part, so by selecting FINISH on this setting you will eliminate the coining marks. I have attached a more detailed description for you to read.

If your machine software is below 13.14 series, then you should contact me directly and I can change some parameters on your machine to eliminate the coining.


Thank You,
Gerard Bailey
Applications Engineer
Haas Automation Inc
Tel. 800 331 6746 x7128
Fax. 805 278 1803
[email protected]

[ktm666]

we run every finish program with the smoothness on finish. still, we get coining. more of a problem on the vm6 than a vf3

[gerard1959]

then I would like to suggest you call your local Haas dealer to check the levelling and machine geometry etc.

Thank You,
Gerard Bailey
Applications Engineer
Haas Automation Inc
Tel. 800 331 6746 x7128

[Andre' B]

Does the smoothness setting just change the acceleration or does it take the motion control down to the next level, known as jerk?

http://math.ucr.edu/home/baez/physics/General/jerk.html

[MikeOD]

In 13.14 series software Haas added Setting 191 Default Smoothness to the settings page of the control which allows you to control the machines acceleration rates, which allows you to control the smoothness of the part, so by selecting FINISH on this setting you will eliminate the coining marks. I have attached a more detailed description for you to read.

If your machine software is below 13.14 series, then you should contact me directly and I can change some parameters on your machine to eliminate the coining.


Thank You,
Gerard Bailey
Applications Engineer
Haas Automation Inc
Tel. 800 331 6746 x7128
Fax. 805 278 1803
[email protected]

Gerard,

I'm not sure if you're aware, but inside of Renishaw probing software, about a year ago we found that if setting 191 was set to smooth, it could occassionally break a probe stylus on a Z surface measurement. As a result, G187 P1 was added to the Renishaw code (it was added in RENIPS.V25 or V26...I can't remember which), followed by G187 without a P after the probe has finished running. When making parameter changes to make a machine without setting 191 behave like a machine with newer software set to smooth, you might want to verify if the machine in question has probes or not as it could introduce a risk for damage to the probe stylus.

[1ctoolfool]

Setting 191 or the equivalent G187 P# simply applies a multiple to the value in Setting 85 which is the corner rounding tolerance. You can also override setting 85 with G187 E#.

"Rough" lets the machine go faster at the sacrifice of accuracy, and "finish" does the opposite, giving more accuracy at the expense of speed. "Accuracy" here means the machine actual path relative to the programmed path. The programmed path is almost always a series of tiny little straight lines which is what the processor "look ahead" and path tolerance is intended to smooth out. These values relate directly to the servo acc/dec in encoder counts/sec/sec.

The corner rounding tolerance is the deviation from the absolute "point" of two intersecting linear vectors. The larger the tolerance, the lower the dV/dt or rate of change of the velocity vector or the less you have to slow down and speed up again when two lines diverge from each other at any angle less than 180. To see the physics of this you can turn on G64 exact stop mode and your machine will physically hit every programmed point and it will also vibrate all over the place.

Remember a CNC machine can only move two ways. A straight 3d linear vector, or a planar circular arc. Everything else is just a combination of these motions and how you handle them at high speed.

[1ctoolfool]

forgot to adress ktm666 comment about using "finish" setting to try and eliminate coining. This is counter-intuitive but you should use "rough" setting and for a 2D type path this will be the setting that minimized the Z axis "jerk" which causes the "coining".

Setting to finish will force the machine to more closely match the programmed path and therefore have a more significant change in direction for the same path.

The "rough" setting will "roll" around the corners and should give the best finish in ref. to this "coining" problem we have been talking about.

[gerard1959]

how about we use Finish in setting 191 and a large value in setting 85 or large E value in G187 to make it roll smoothly around the corner.


Gerard

[1ctoolfool]

This could be redundant because 191 is just a multiplier for setting 85. So changing setting 85 for instance to .100 or 4 x the factory default of .025 is the equivalent of setting 191 to "rough" with 85 set to .025.

I'm not 100 percent on these numbers but 191 "rough" multiplies setting 85 by four and 191 "finish" divides it by four, something like that...... I might be wrong on the actual integer value of the multiplier.

[MikeOD]

This could be redundant because 191 is just a multiplier for setting 85. So changing setting 85 for instance to .100 or 4 x the factory default of .025 is the equivalent of setting 191 to "rough" with 85 set to .025.

I'm not 100 percent on these numbers but 191 "rough" multiplies setting 85 by four and 191 "finish" divides it by four, something like that...... I might be wrong on the actual integer value of the multiplier.

It is not "just a multiplier" for that, it does do that but it also controls servo acceleration. There are 3 groups of 3 parameters related to acceleration and deceleration as well that setting 191 selects that are independant from what it's doing to setting 85.

If you want a 2D toolpath to flow smoother through corners, on a machine that has setting 191, leave the setting alone (at medium), and leave setting 85 alone, then try G187 P1 E0.05 in your program on it's own line before your feed moves. Depending on the size of the machine, the rapid speed, the feedrate you're running, you might need to change the value next to E...and you might be able to go to a smaller number with it. When you're on a 3D surface path with really tight tolerances, you might want to try G187 P3 E 0.025...I've had great luck with that on both a VM-2 and a VF-2SS.