1/4" Cut Conditions

[sodfarmer]

I started cutting 1/4" the first time and had a few questions and was curious to see what other people are getting. I have a home built table with CandCNC DTHC and electronics, Hypertherm 1000, sheet cam. When I cut parts I'm getting 3 degree postive angle on the outer profile. Is this normal? Does my specs seem close or am I way off? Dross comes right of with wire brush on angle grinder.

139 Torch Volts
Cut Specs:
Outer Profile
50 IPM Feed rate
.15 Pierce height
.06 Cut Height

Holes:
35 IPM
.15 Pierce Height
.06 Cut Height
I disable the torch height
Holes are .5625" for 1/2" bolts

Thanks,
John

[elkriverfab]

sodfarmer,

I think the angle you are getting is normal.
Your pieces look pretty good and clean.

Holes look real good too.

I too get a slight angle or bevel on heavier plate.

I could be wrong but plasma does that.

My torch is smaller and I have to use plyers to break off the edges but it breaks off clean.

Sometimes I can get a real straight edge but corners and speed has so much to do with it.

[jimcolt]

You don't say what amperage and consumables you are using for cutting the 1/4" at.....so I'm guessing a bit! If you have a 3 degree taper that is pretty consistent...you are doing great on 1/4" with an air plasma system. Industrial high definition oxygen plasma systems can do better....but cost 10x as much as an air plasma. The only suggestions I would have:

1. Worry more about maintaining the the physical cut height (.06") than the voltage.....adjust the voltage up or down when the cut is at speed to ensure .06" is maintained. Closer to the plate will provide less angularity.

2. I would recommend using the 40 amp shielded consumables at the Hypertherm book specs (if you are not already doing so) From your cut speed I would guess you are running at 60 amps....the 40 amp process will provide a squarer edge. Use the specs exactly as the manual lists on the mechanized cut charts....make sure you are using the mechanized consumables (even if it is a hand torch). Lower power, lower speeds will produce a smoother , squarer edge.

3. Holes.....continue locking out AVC (height control) on all holes under 1" diameter....also slow the speed in your program on these holes to 60% of the contour speed for outside cuts. For best holes use a straight lead in that starts in the center (this gives the z axis time to index down to cut height, and for the plasma arc to stablize after piercing), use adequate pierce delay time (from the manual) to allow full penetration before any x, y or z movement, and use an overurn (if your software allows it)....at the end of the cut. An overburn is a cut path that stays on the circle radius about .150" past the lead in of the hole. Ideally the plasma arc should be programmed to shut off during the overburn.....before the motion stops....leaving a nice round hole with a minimal lead in divot.

Not all machines/ software allow all of this functionality on holes. On some high end (expensive) cnc plasma's the hole profile, the hole speed, the lead ins and overburns, as well as the plasma process (gas pressure, amperage) and the height are automatically manipulated and set through the CAM software....these settings are fine tuned for each thickness, power level and hole diameter to provide near perfect holes.

Using an air plasma on a low cost machine requires a bit of experience and operator skill to manipulate all of the settings for best quality.....but it sounds like you are on the right track!


Best regards, Jim Colt Hypertherm

I started cutting 1/4" the first time and had a few questions and was curious to see what other people are getting. I have a home built table with CandCNC DTHC and electronics, Hypertherm 1000, sheet cam. When I cut parts I'm getting 3 degree postive angle on the outer profile. Is this normal? Does my specs seem close or am I way off? Dross comes right of with wire brush on angle grinder.

139 Torch Volts
Cut Specs:
Outer Profile
50 IPM Feed rate
.15 Pierce height
.06 Cut Height

Holes:
35 IPM
.15 Pierce Height
.06 Cut Height
I disable the torch height
Holes are .5625" for 1/2" bolts

Thanks,
John

[sodfarmer]

Thanks for the info. I cut the parts with 40 amp consumables and cutting @ 40amps. I will try to slow down my speeds and adjust my torch volts to maintain a .060" cut height. I'm still getting used to plasma cutting, I used to work for a company with a 1500 watt Mazk laser, and this spoiled me. I have to remind myself that comparing my plasma table to the laser, is like comparing apples to oranges.

[jimcolt]

There are plasmas in the industrial world that cut faster than lasers on 1/4" with similar cut quality.......but they are not air plasma systems. There is another whole world of indusrial plasma systems out there....in comparison to the air plasma systems that we can afford in our small shops!

...Follow the optimum travel speeds in the mechanized cut charts in the Hyperthem manual....I think you will like the results.


Jim

Thanks for the info. I cut the parts with 40 amp consumables and cutting @ 40amps. I will try to slow down my speeds and adjust my torch volts to maintain a .060" cut height. I'm still getting used to plasma cutting, I used to work for a company with a 1500 watt Mazk laser, and this spoiled me. I have to remind myself that comparing my plasma table to the laser, is like comparing apples to oranges.