Quality hole cuts

[andyyang]

I am working for a fabricating shop which bought a HD260xd Plasma table recently. We follow the user manual for all the settings as we don't have enough experience with this machine. The machine is cutting thick material( 3/4in to 1-1/2in) good with 260 torch at factory setting. But when we cut 1/2" and lower using 130 amp and 50 amp, the holes and slots finish are so rough. We had technicians came in for training purpose last week, and he tried to fix the problem by slowing down the cutting speed for hole cutting. That helped, but not quite as we expect the machine can do. Also as we slow down the speed for cutting holes, the torch is trying to dive down. So we can only set it up around 85% for hole cutting. I wonder if there are any solution to this problem.

[Stout]

What do you mean by 85%? If you are following the published cut speed and the torch is still diving, then the machine is moving too slow. Is the torch dragging on the plate?

Some CNC controllers will slow down the cut speed for circles smaller than a certain diameter and will also disable THC for circles to prevent diving during circular cuts when the machine is slowed down. If the CNC is in fact slowing for circular cuts, it may be going too slow.

[wdaniel141]

Have you tried using over runs when cutting holes? Rather than using a lead out where the arc leaving the plate can wear out consumables an over run of a couple of mm will not shorten consumable life. On the Kerf machine that i currently use we experienced similar problems with hole cutting, but by using the overburns and adding .250 plasma advance off (which powers down the plasma arc fractions of a second before finishing the cut) the results were clearly better. Also using a circular lead in could help. Hope this helps.

[jimcolt]

Be happy to help you dial in your holes with the HPR260. I will need details:

-What brand cutting machine
-What is the CNC control on the machine
-What CAM software are you using to nest your parts
-What brand and model of torch height control.

Hole cutting requires that (on holes under 1-1/4" diameter) 1.the torch height control is frozen at the recommended cut height (this should be 100% automated depending on your cnc, your CAM, and your THC), 2. The cut speed is programmed at 60% of the recommended book cut speed, 3. The hole is drawn with a long lead in (can be straight or radiused, but must be long enough so the height control can fully index from pierce to cut height before getting on the hole radius., there should be an overburn (cut past the lead in kerf about .150 to .200").

Best regards, Jim Colt Hypertherm

[dkoril]

Jim

I am using a HT65 with Plasmacam, mach3, and Candcnc hardware. Where would i adjust the overburn? The holes i have cut in 3/16" have been of poor quality. I am using 60% of the recommended settings in the manual for 3/16". Any recommendations?

Thanks
Dustin

[jimcolt]

Post some pictures of your holes with poor quality....so I know what you mean by that...and I will be happy to help steer you in the right direction. I do nice holes with my Powermax85 (same torch as your Powermax65) on my cnc machine....just made a bunch of parts last night on 10 gauge steel with 3/8" holes that looked almost like they were drilled.

Jim Colt

Jim

I am using a HT65 with Plasmacam, mach3, and Candcnc hardware. Where would i adjust the overburn? The holes i have cut in 3/16" have been of poor quality. I am using 60% of the recommended settings in the manual for 3/16". Any recommendations?

Thanks
Dustin