[jakemestre]

Does anybody know what the max rapids and accelerations are for the series 3 upgrade? I know the max cutting speed on the x and y is set to 110ipm with 90ipm on the Z but where does rapid fall? I use Gwizzard for helices and need to input the relevant data on the acceleration. Thank you in advance.
Jake Mestre

[TXFred]

Rapid is just a term that means,"The axis moving as fast as it can." In your case, that's 110 IPM on X and Y, and 90 IPM on Z.

Frederic

[jakemestre]

TXFred,
I don't think you're correct on saying that rapid is the same as max cutting speed. 110IPM is where Tormach set the x and y based on a 500lb reserve force for cutting. If the axis is not being taxed then the max speed can be greatly increased without loosing positioning accuracy. On a router I just built I designed the motion to rapid at 1000ipm while cutting at only 200ipm. This way I would reliably know with the feed forward control that the position stays accurate, and precise. I appreciate your input, and I guess a way to potentially test the speed is to send only one axis at a time and look a the speed in Mach. I'll try that when I get to my machine next, and report back. Thank you.

[Zetopan]

Jake:

"I don't think you're correct on saying that rapid is the same as max cutting speed."

TXFred is exactly correct. Tormach rates their rapids as the fastest cutting
speeds. As a result the fastest non-cutting speed is identical to the fastest
cutting speed. You can also find this information on the Tormach website.


"the max speed can be greatly increased without loosing [sic] positioning accuracy"

That is only true for position feedback systems. Since the Tormach mill does
not employ position feedback, your statement does not apply. I would also
recommend that you look up mid-band resonance in stepper drive systems.

[philbur]

I think the OP is actually asking about the PCNC1100 accelerations settings, to use for input to Gwizard.

Quote:
"Gwizzard for helices and need to input the relevant data on the acceleration."

Does anybody know. Can a person find it without unlocking the software.

As others have pointed out the Tormach series 3 axes velocities are set at 110, 110 and 90 ipm, cutting or not.

Phil

[zephyr9900]

There is a Mach3 XML viewer/editor available. Read the thread Mach XML Reader for location.

Not being a Gwizzard user though, I'm not sure I quite understand the thrust of the question. Even on simple 3D contouring, I can, say, set F20 (ipm) but on more highly curved areas the actual speed might drop to 10 or 5 or 3 ipm due to the finite acceleration. Lateral acceleration on a curve is expressed as a=v^2/r. For a constant accleration, as the curve radius r decreases the velocity v also must decrease. That lateral acceleration is resolved into the individual axis accelerations, and the limiting axis will determine the velocity of all, in order to follow the commanded path properly.

TXFred and Zetopan are correct. Tormach has already set the acceleration and maximum velocity to what is reliably possible with the Tormach hardware. Maybe a little past for individual Series 3 machines, based on VaderSpade's experience...

Randy

[TXFred]

In theory, an axis could move faster when not cutting. Because there are no cutting forces, there will be power in reserve. This would especially be true on a linear rail machine where there is almost no resistance at the ways.

But Mach isn't designed to take advantage of this. It has a single maximum speed that it uses for G00, G01, G02 and G03 moves. It could probably be increased, but only by eating into the safety margin and risking missed steps.

Frederic

[zephyr9900]

But Mach IS taking advantage of this. You set up acceleration and velocity as high as you can to get reliable G0 moves. What Mach DOESN'T do is derate the speeds for cutting--you can try cutting at the equivalent of G0 speed if you are brave enough. (Or type G0 instead of G1 by accident--no, I've never done that, not even once )

Now, there is a thing that Mach (nor any other motion control software I know of) doesn't do, but could theoretically do to bump performance. Most stepper motors have a "knee" in the torque/speed curve. The torque falls fairly slowly up to a certain speed, then falls off more quickly. With a constant acceleration, you are fitting a straight line to the "worst" point on the curve (full running speed) but then there is a torque reserve at lower speeds. You could set up a variable acceleration to track the torque curve and get better acceleration for short moves and sharper curves, where it precisely is needed. But that would need to be tailored for each motor/driver/power supply situation and would really only be for tweakers/hardware hackers...

Randy

[TXFred]

But Mach IS taking advantage of this. You set up acceleration and velocity as high as you can to get reliable G0 moves. What Mach DOESN'T do is derate the speeds for cutting--you can try cutting at the equivalent of G0 speed if you are brave enough.

Randy

Good point.

[dbrija]

(Or type G0 instead of G1 by accident--no, I've never done that, not even once )

Randy

Me neither..... However, I was surprised at how good a finish my facemill gave me at 90IPM.

In all seriousness, this isn't a machine I would want to cut with at max rate.

[TXFred]

Me neither..... However, I was surprised at how good a finish my facemill gave me at 90IPM.

If you're talking about the 1.5" Tormach facemill, then 90 IPM actually is the recommended feedrate for aluminum. So you can face a part with nothing but rapid moves.

Frederic

[dbrija]

If you're talking about the 1.5" Tormach facemill, then 90 IPM actually is the recommended feedrate for aluminum. So you can face a part with nothing but rapid moves.

Frederic

It was my Glacern 2.5" mill, .1 DOC, full width in 6061. The load meter didn't get too excited either.... It was the actually the noise that spooked me.

[twocik]

"It was my Glacern 2.5" mill, .1 DOC, full width in 6061. The load meter didn't get too excited either.... It was the actually the noise that spooked me."


Wow ! I would really like to see that any videos ? I still haven't gotten around to buying this, every time something else pops up.

[dbrija]

"It was my Glacern 2.5" mill, .1 DOC, full width in 6061. The load meter didn't get too excited either.... It was the actually the noise that spooked me."


Wow ! I would really like to see that any videos ? I still haven't gotten around to buying this, every time something else pops up.

No video. It was an unintentional max speed cut. I will capture a video should I go for max again (intentionally).

[jakemestre]

So here are my findings after a little research, a lot of tuning, and some missed steps.
Knowing acceleration is quite useful for precise control of tool paths. If you think about it the machine has to accelerate quite rapidly in order to make a precise .25" hole in acrylic. The same principle applies to other materials and tool paths such as helices, thread milling, or ramp milling. Gwizzard utilizes the max acceleration to ultimately calculate the speed the cutter can travel without exceeding the machines capabilities.
The acceleration using the mach XML reader showed 15. I took a look at my routers settings using standard Mach3, and found the units to be in/s^2. You can do the conversion.

On the order of rapids and cutting speed:
Tormach does in fact maintain the rapid and max cutting speeds to be exactly the same. This does not however mean that the machine is incapable of moving faster. Tormachs white paper on the leadshine stepper motors and drivers states that their speeds keep, at minimum, 500lbs force in reserve. This means the motors are capable of moving the table and a lot of extra weight around at the rapid speeds without any problems.
After adjusting the gibs and knowing my own needs I've been able to push my speeds up 140% without ill effect with boosted the acceleration.
I have yet to run the machine to see if mid-band resonance at these speeds will become an issue. Leadshine drivers do not compensate for mid-band resonance so the phase shift needs to be avoided at all costs.
The testing process, as provided in the Mach3 handbook, has the user set up a test indicator on the table at an extreme of travel. The machine is then sent to repeat a rapid move one axis at a time. The idea is to see if steps are being lost with repetitive acceleration and deceleration. Basically you make your machine go until it looses steps and back off roughly 5-10%. This value will then be your max rapid speed.
Keep in mind that after tuning, rapid is NOT your max cutting speed you need to remember your max feed rate with extra force in reserve is somewhere around 110-120ipm.
That's all the info I have for you that can be readily obtained without unlocking Tormachs Mach.

[TXFred]

That's interesting research.

I don't think that I would want to increase the rapid speed of the X and Y axes. The X and Y motors take most of the cutting forces while milling. I don't think that the few seconds saved per cycle is worth the risk of missing a step.

The Z axis is another story. Z rapid speed can pay off in a big way if the mill has to do a lot of G82 deep hole drilling. On this canned cycle, most of the time is spent rapiding in and out of the hole to clear chips. It's rare that Z axis operations move at anything approaching maximum speed, so I think this would be an very safe modification.

Frederic

[Al_The_Man]

But Mach IS taking advantage of this. You set up acceleration and velocity as high as you can to get reliable G0 moves. What Mach DOESN'T do is derate the speeds for cutting--you can try cutting at the equivalent of G0 speed if you are brave enough. (Or type G0 instead of G1 by accident--no, I've never done that, not even once )

One thing that seems to have been overlooked is the definition applied to G0 and G01, G0 is/was intended to rapid position axis at NON-interpolated positioning at the machines rapid rate, some machines implement rapid overide at the discretion of the MTB.
G01 uses the F value for feed and is always Interpolated moves, there also may be a feed rate overide.
Al.

[BobWarfield]

The helix is one of the more demanding moves for these machines, and for some machines, they can lose accuracy on interpolated holes by exceeding the acceleration envelope needed for the helix. One could encounter this thread milling as well, I suppose.

Mastercam actually includes a test for this where you do a series of interpolated holes until you find the acceleration limits for your machine, so I built the helical interpolation calculator into G-Wizard so people who are concerned with very accurately interpolating holes can keep within the acceleration limits of their machine.

All that said, unless you're trying to do very accurate interpolated holes very quickly, I wouldn't worry about not knowing your acceleration too much. If you wanted to spend an afternoon experimenting with increasingly fast feedrates interpolating holes, you'd find out pretty quickly whether your machine is capable of going too fast to be accurate.

Cheers,

BW

[TXFred]

Mastercam actually includes a test for this where you do a series of interpolated holes until you find the acceleration limits for your machine, so I built the helical interpolation calculator into G-Wizard so people who are concerned with very accurately interpolating holes can keep within the acceleration limits of their machine.

I haven't seen that feature. Where is it?

Frederic

[BobWarfield]

I haven't seen that feature. Where is it?

Frederic

It's part of the Highfeed option. See this link:

http://www.mastercam.com/Support/Dow...s/hfapp_v8.doc

Cheers,

BW