Cut height and bevel

[BensPlasmaAu]

Hi all,

I have been getting some decent cuts lately in terms of dimensions etc, but I have dramas with getting rid of the bevel in thicker material especially 12mm which I use quite a lot.

Situation. G code seems to be correct on the screen in Mach3. Torch touches off raises to 3.8mm for pierce, delays properly and then lowers to 1.5mm cut height. And this is where it seems to be doing something wrong. I can’t see it on the Mach DRO, but I can see the Z move upwards after it drops to the cut height. The DRO says it is at 1.2mm but really it is much higher. I hit the pause button as it is cutting and turn the torch off, the height of the torch is about 5mm or higher. The DRO then decided to show 5.607mm.

There is no code in the post or on the Mach screen to show this raise in height after getting to designated cut height.

Theory. Perhaps. I have been having some dramas with the DTHCIV card deciding to go into a loop and keep the z down signal activated, over riding the Mach program. I have to push the hard reset button on the card and then reset and re home the Z. My quick theory is that there is something fishy with the card giving it a false voltage signal.

Known things. Z steps per is spot on. Have tested this numerous times. Table and material grounded. G code sees to be fine. Mach read outs show what I want to be seeing in terms of height voltage etc. DTHC responding properly.

I believe that the bevel I have shows the torch is way too high. Thoughts or ideas please. If I can get rid of this bevel that would be BRILLIANT!!!!!

[plasmartist]

You may check your rules in sheet cam to see if there is a rule set up. That's just an educated guess, I run commandcnc, surely others will chime in. Of coarse I'm assuming you have your voltages for dthc set correctly

[motoguy]

Is the bevel the same direction/shape on all 4 sides of the cut? Just two sides? One side only?

[sphurley]

The DTHC takes over the Z control not Mach after your wait setting in sheetcam. Your voltage is too high. Lower the voltage and the cut height will lower.

[Simko]

While cutting, the z-height is controlled independently of the g-code by the torch height controller. The torch height controller is basicallly a PID loop that monitors cut voltage and makes the required z height changes to keep the voltage close to your setting. It's not a surprise that your DRO does not know what is going on.

Have you done straight line test cuts with DTHC turned off to see what voltage you are getting when cutting at the proper 1.5mm cut height?

[tcaudle]

The DTHC moves the Z independant of MACH (which is way too slow for real time control) then when it finishes the cut its resets the Z DRO using the total of al the Z incremental moves. Its less important what the Z shows while cutting that what the actual gap is WHILE cutting. If its too high then either the voltage coming back from the torch is lower that it should be or the preset volts are wrong for that set of sonsumables and the feedrate on that material
Remember" The higher the torch the Higher the volts. The lower the torch the lower the volts . You cann FORCE voltage you can only set a value you would ike the torch to move up or down to hit.

[BensPlasmaAu]

Hi guys,

Thanks for the responses.

No rules apart from end of cut anti dive things.

With the knowledge of how it works now, perhaps in regards to the stalling and looping of the down signal when I need to reset the DTHC card, that is the card and Mach fighting each other. The bevel is on all sides, the same angle bevel on all sides, one side is inwards and the rest is outwards.

Will lower the voltage a fair bit and see what happens. Out of curiosity, can anybody share their Powermax 45 settings. I know I have set it to the book setting in sheetcam. Actually thinking of that, do I need to load settings in a different place for the DTHC as well as sheetcam tool path settings? So Sheetcam tells Mach what settings it is, but then if the DTHC is a closed loop, do I need to program these settings separately ?

Hi Tom, was typing this as you were replying. So the setting on Mach from the post processor is the right setting? Basically it sets what the DTHC is meant to be reading and then the card takes over and does it’s thing. So I should lower the voltage in the tool settings in sheetcam and see how it all goes?

Thanks again all. Brilliant!!

[BensPlasmaAu]

Hi guys,

Got to the workshop this afternoon and tried lowering the voltage. The book spec says 130v which is what i had loaded into the tool in sheetcam. I dropped it to 120v amd gave it a go. Much less bevel. I dropped it again to 110v and i got the bevel heading the other way on one part and the hole it cut was a bit tunnelly slanting off. So i will set it to 115v and give it one more blast. Ill take some photos and post up when i get home.

[beefy]

Ben,

myself and quite a few others with Hypertherm cutters have been plagued by this in the past.

One solution I heard of (and will never forget) is to replace the cap O-ring !!!!!!!!!!!! Yeah, weird I know. Get a new genuine cap O-ring (not an old hard one) and see if it helps. Several guys have tried it and to their surprise it seemed to do the trick. Please don't get the shits with me if it doesn't work, I'm only repeating what I've heard LOL.

Myself I seemed to get improved results by slowing the cutting speed down. Now whether that was a band aid fix for something else that was wrong I don't know. I haven't done much cutting on thicker stuff for a while.

Search for "bevel" and "lean" on the forum here too.

Keith.

[BensPlasmaAu]

Hi Keith, I’ll certainly give that a go. I have notices that when it pierces, the sparks always come out one side of the torch, perhaps there is something to the orient thing. Poor machine has been copping a puzzling the last couple of months, especially with the thicker stuff. I’ll be doing some more trial and error adjustments soon on the other material I use.

So far it seems to be working real well at 120v at 510mm/min. Could change it down in speed a little I would be next in trialling.

Accuracy and repeatability has been really spot on. I worked out I was about 3 steps per off in my motor tuning so that has helped heaps. I do have a minute bit of backlash somewhere between the belt drive reduction and the pinion meshing with the rack. A motor and drive upgrade is planned in the near future. I will be going for Clearpath Servos with planetary reduction drives and the rack and pinion will go from a Mod 2.0 straight cut arrangement to a mod 1.0 or 1.5 helical setup. I will also get a much better arrangement of tensioning the pinion to the rack. Should be pretty bloody good.

A couple of pictures. A few of the edge quality of the different speeds etc i tried. The dross I left on mostly, but it peels off with my hand pretty easily.

110v @510mm/min

115v @510mm/min

120v @510mm/min

Before I made the adjustments

After adjustments. Much less bevel.

[beefy]

Now, that last one looks really sexy (no I'm not talking about your hand).

[BensPlasmaAu]

It’s a great result! Just got to fix the backlash and I reckon it will be finally on point to take the business to more customers to get their work. I’m currently doing some plates for an engineering shop for their architectural brackets etc. there are 4 other workshops around my area who do a lot of architectural stuff and need simple mounting plates made up. I’m pretty happy with this edge quality, fix the tables ability to cut a decent hole and I’m off.

[Simko]

Straight line cut tests are your friend...

I have found that if you cut at the right height and at the right speed (book specs) and you aren't getting good cuts, then something else is wrong. For me it is normally the electrode that is messed up and causing the arc to do weird things, but I would also look at air pressure, swirl ring, nozzle, yes even the o-ring.

I use my table to cut a lot of thicker stuff (1/2" to 3/4") and a standard taper for a plasma arc is about 2 degrees. That means the best that you will do on 12mm is 0.42mm larger on the bottom of the part per side.

I am still learning how to get good holes in think material. The best that I have found so far is to put the holes on a separate layer and cut them with the DTHC turned off and the Feed speed set to about 60% of book speed. (Yes, this is one time where you will want to reduce the speed)

[Mac]

I found this helpful, you might as well.

[plasmartist]

One other thing others haven't mentioned as of yet is which electrodes you're using. I have used a slew of import electrodes and ultimatley switched back to genuine. a couple months back I stared using copper plus electrodes and absolutely love them. In my opinion the copper plus makes cleaner cuts than standard electrodes.

[plasmartist]

a side note, from the pictures and the amount of slag it looks like you're running your water level a bit high. The reason I mention this is because it can harden your steel and make it brittle, not something many people want in a bracket. But I agree that you seem to have your dthc settings dialied in quite nicely now.