Torch diving only on the holes in 1/2" thick steel (CommandCNC)

[Simko]

I was given some big drops of 1/2" thick steel diamond plate and what better to make from some free 1/2" steel.... Reactive pistol targets!

I made a few different size gongs and a few silhouettes. I had absolutely no issues cutting the outlines, in fact, the cuts looked great with very little dross. I used my PM85 with a 65A nozzle.

The issue was every time it went to cut a hole, it would dive to the point of triggering the e-stop. Sometimes it would stop around half way through the hole and sometimes it would dive right after the slug dropped out. The holes also had a wicked taper compared to the edge. The holes were 5/8" diameter.

I am using CandCNC electronics with CommandCNC (Linux). I tried increasing the VAD - velocity anti-dive to 90% and 95%. I tried to add a holes rule in SheetCAM. I even tried to turn off the THC manually while it cut the holes and then I was going to turn it back on after the last hole but I am not sure that I did it right. Do you select 'DTHC Manual', or select 'DTHC Off', or both? I can't say for sure exactly what I had pressed, but the CommandCNC turned the DTHC back on automatically.

Any help would be appreciated. I have been cutting mostly 12ga lately and had had zero issues with diving, so I was a little surprised with how much trouble I had with the 1/2".

Thanks!

[tcaudle]

All you have to do is set the MIn Cut Length for DTHC in the SheetCAM Operation to a value GREATER than the hole circumference + lead-in. It's better than a cut rule because it never turns the DTHC ON if it violates the setting. The software knows in advance how long a cut is and it turns the DTHC ON/OFF automatically on each cut and can decided to not enable it for a cut if needed VAD is great on corners, end of cut etc, but it only senses a velocity slowdown and that might not occur on a hole.

General rule of thumb on holes is you don't cut one smaller than 2X the thickness in diameter so on 1/2" a 1" hole is close to the limit. You also need to cut the holes at a slower feed rate (which messes with VAD because its easier for the motion to stay at the full reduced speed )

To cut holes differently group them into a separate layer (named something like "holes" ) and put that in its own operation and cut at a lower feedrate and set the Min Cut Length value on that operation.

If you have the Hypertherm with the RS485 and the HyT-Connect kit to control cutting Amps you could also so soft starts on that 1/2" to get better piercing and longer consumable life but that's another story.......

[Simko]

Thanks Tom! I'll give it a shot. I forgot about the Min Cut Length.

I do have the RS485 and Hy-T.... any place you could point me to for some reading. Is this a new function?

[tcaudle]

no not really. Its built into the software and you just set the soft pierce % in the Operations . I would try 70%.. It slows down the plunge by the same % which might not be enough so you might need to alter the plunge rate . The idea is to start the pierce and pool the metal so it does not blow straight back instantly and sorta ease into the cavity. The lower current appears to put less stress on the consumables and you can typically pierce thicker material. We have not played with it a lot because we do 90% 10ga and thinner. One area we have used is the light peck where it short fires the torch at a reduced current to mark the top without going a full pierce. I have been able to mark 14ga with no problem and I think I can do 16.