[Knut]

In speaking with my hypertherm dealer, one of the salesman mentioned that speeds and power were really the things that will determine the amount or lack of dross on cuts. That contradicted what hypertherm seems to be selling but in his determination that was just about everything. He wasn't impressed with hidef, at least for the needs I had described.

He did mention that very high end plasma machines could vary their power on cornering to control dross at that point.

With that in mind I recall Mach3 being refered to as a constant velocity controller. Yet have also read of acceleration being set for corning therein.

I can't find a manual on the Artsoft site to clarify what these terms mean so am asking it here in the plasma forum since you must be familar with it.

If mach3 can vary the speeds for cornering, has anybody attached a stepper to the amp control pot on a their manual/machine plasma box to control power in addition to speed? Or is there a simpler way to hijack the power settings on a manually adjusted plasma box?

Thanks,

[Torchhead]

You need to understand the physics of cutting. Constant Velocity means that it looks ahead and "blends" the toolpath to smooth out the segments. In a lot of files (especially decorative cutting or ones derived from segmented line imports rather than true arcs) have bunches of "nodes" along a polyline/polygon. Each node is seen as a start and stop (separate line of g-code) with accel and decel applied by the control software . Using software that is Exact Stop (no CV) it jerks at each one of those nodes as it applies the numbers. CV works to blend those nodes together and smooth out the cutting. Smooth motion is important in plasma since any slowdown will effect the cut.

The actual speed of the cutting tool over the surface is a factor of several things. The commanded feedrate is the number in the G-code you apply. It's like planning a trip in your car and calling for an average speed of 60 MPH. You can't do 60 on a 90 deg turn or you spin out. You have to slow down then accelerate out of the turn. Thus it is with a CNC machine. It can only hit a certain speed on tight turns. If you come up to a sharp turn the machine will automatically slow down to stay on track.

Slowing down with a rotating bit does not cause a lot of issues. Running under THC, slowing down with the torch on cause the voltage across the gap to increase and for the THC to see that and move (dive) the head towards the metal. Dynamically decreasing the cut current would be one way to solve that but only the very highest level of plasma cutters ($$$$$) have any form of remote control of the current control.

The other quite usable approach is to tell the THC electronics to ignore the voltage spike if the toolpath feedrate is less than a preset percentage of the target feedrate. When the machine slows to take a sharp turn instead of the tip diving into the work the THC keeps it at the same height around the turn. This feature is only available on a THC that has knowledge of the actual toolpath.

There are several CV setings in MACH that effect the reaction to tight turns but under THC the best solution is to use the Ant-Dive setting to tell the THC to ignore the resulting voltage spike and maintain the same height. It works since it creates a clean cut.

This is one of the points I keep trying to make. Stand alone THC soltuions do not have any way to know what is happening with the toolpath and what speed the machine is actully running VS the target feedrate. They just measure the voltage and react....period. Some don't even have a provision to stop the motion if you don't get a valid pierce or lose arc along a cut.

There is no such thing a totally dross free cuts on detail cutting (lots of angles and direction changes). On long straight or arc cuts you can get dross free if you futz with the voltage (gap) setting, the feedrate, and the air pressure. It will take a lot of setting to get the perfect numbers. Once you have it you can cut that exact type and thickness of metal with similar results. As soon as you introduce angled cuts the feedrate readjusts and you start picking up dross.

If your intent is to product absolutely gross free cuts you need to buy an abrasive waterjet cutter or laser.

I find the amount of dross to be minimal and it comes off with a quick scrape with a sharp chisel (not a cold chisel) and then a quick swipe with a flap sander.

There is no "simple" way to electronically control the current setting on a manual plasma. It would mean getting into the control electronics (boo!) or mounting some kind of crude little servo motor on the pot. Just not practical.

I would not put a lot of stock in what any vendor salesman says. They only know what they are told and the selling features of their brand. You have to understand that Hypertherm sells a THC unit and even an entire plasma cutting system. The THC alone is around $10,000. A complete table and interactive system is six figures.

"If all you have is a hammer, everything looks like a nail"


Take it from someone that cuts miles of steel a year. There are a lot of other issues to worry about than a little dross! Your ability to move from idea to cut product has a lot more to contribute to profit than getting a perfect cut with a 30,000 deg flame. While there is money in repetative cutting of simple shapes you make better money doing one-of-a-kind custom jobs.

Tom Caudle
www.CandCNC.com
www.FourhillsDesigns.com

[tinman13]

Tom, Thank you for that good explanation of CV in Mach, I have wondered about those settings!
Could you go into a bit of detail about what the numbers for anti-dive and thc rate mean?
Thanks again for the explanation, Steve

[Torchhead]

THC Rate is the velocity expresed as a percentage of the max velocity of Z. You have to run at a reduced velocity since there are no acceleration or deacceleration values applied to the hundred of short moves on the Z while running under THC control. A good number to start with is about 30%. Some motors will handle more, some less. The THC rate effects the speed at which the head moves while cutting under THC control. What it means is you are doing Z moves at 30% of the max Z velocity setting. So if your Z will do 60IPM before faulting with accel/deaccel numbers applied, you will be doing THC moves at about 18IPM. Since normal moves are typically less than .060 at a time it works okay. Only if you want to cut wavey metal siding with 60 deg slopes will you face a problem. Math says to cut a 45 deg slope Up, you need to move the Z at the same feedrate as the X and Y.

Anti-dive is a number (feedrate) below which the THC signals are ignored (no adjustment). It requires knowing what the actual blended speed of the toolpath is and is applied to areas were the machine (because it has to) slows down. Without it, as the feedrate slows on a tight turn or direction change, the motion will slow and for a brief instant the tip voltage will jump based on the fact the torch is cutting less metal. The THC will react to that spike by lowering the tip towards the metal. When you only have .062 to play with too much lowering can result it a tip bounce on the metal. Some dive is inavoidable; tip crashes should be.

Tom Caudle
www.CandCNC.com

[Knut]

Thanks for the informative reply Tom.