[repauli1]

I have my homemade table and I have been playing with settings in Mach3 to improve the edge cut quality. My gantry would shake when turning sharp corners and cause a saw tooth effect in cut. I lowered my accel time from 25 to 5 ips. And increased my cut speed from 55 to 180. Now it's a smooth cut but my letters look weird. When cutting an I it rounds the corner, and has a slope effect. See attached: any help greatly appreciated. 18 ga cold rolled using Hypertherm 30 set at 30amp.

[LeeWay]

Try adjusting your CV settings on the General Config page.

[repauli1]

I have read several sources of info on CV settings, and I believe my Y axis is coasting as my X axis moves. I changed the look ahead from 50 to 200, with no change, also changed tolerance from 20 to 5, no change.
Tried saving, closing Mach3 and restarting.
Turned plasma mode on/off no effect.
The only thing that helps is slowing cut speed to 100 and increasing accel to 15-20. But then the jerkiness occurs.
Any more suggestions appreciated.

[LeeWay]

You can try cutting in Exact Stop mode and see how that works. That would really be a last resort though. Keep acceleration low in that mode.

[jimcolt]

By reducing your acceleration.....that means that in areas with detail the machine is actually cutting at very low speed, and on straights and easy radiuses it is getting to higher speeds. Plasma likes to run at high speed and with high acceleration for best performance. When the machine slows for intricate details....the cut kerf gets wider and will distort your part as well as producing dross and warpage. This is the reason why high performance plasma cnc machines use larger, inertia match motors...and the highest performing machines use servos.....which have a wider speed/torque range and generally better acceleration through the range.

Best bet is to check all mechanical components for any backlash or flex.....as this, combined with the acceleration is what causes the rough edges. You can also run a slower speed....and adjust your kerf width to accomodate for better accuracy.....although slow speed will produce dross and warpage on thin materials.

I cut 18 gauge at about 40 amps (Powermax85) at 275 to 320 ipm. My primary machine has servos and accelerates smoothly at these speeds. Very little dross...no warpage.

Jim Colt Hypertherm

[br1]

Try converting some of the fonts to arc's as a lot of fonts have a lot of tiny straight line moves to produce an arc that can cause issues and burning. More than not your machine is just fine and it is the font your using. I assume that when cutting a single square or a true circle the problem goes away?

[SaskFab]

Try dropping your CV distance tolerance down to .1 (decimal one!) which should force the motion planner to keep the path within a tenth of an inch or so when it's trying to make a tight turn. Start there and adjust up or down until you can tolerate the corner rounding. It sounds like you have Mach set to inch units, and as a result the distance tolerance is in inches as well. A setting of 5 is obviously going to generate some very well rounded corners if the accel is low and speeds are high.

Jim's advice is bang on. You will need to experiment to find some combo of reduced cut speed and reduced current that will still give you tolerable cut quality while staying within the constraints of your limited acceleration capabilities. The higher the cutting speed the more problematic low accel becomes. Set the CV distance for minimal rounding first, then bump up your accel rate to just the point before the shaking becomes intolerable.

As br1 says, some files/fonts/code is just horrible to cut if it's made up of a lot of points instead of smooth arcs/lines.

Finally, when tinkering with Mach's motion settings, *don't* make use of the feed rate override when trying out different settings. Generate new code with the desired feedrate each time. The motion planner bases its calculations on the programmed feed rate and an override throws it off with respect to it being able to make smooth transitions from one segment to the next.

Marv