[patriot customs]

Hi
I'm new to cnc plasma cutting, I received my new table a few months ago and have been just playing with different materials and thickneses. I have a real job now to cut, it's a bunch of .75 and 1.75 diameter holes in .375 hot roll plate. I'm getting about .025 to .035 of bevel from the top of the hole to the bottom, I don't know if this is as good as it gets or if I should be able to get better results with different settings. I have tried different THC settings,amps,cut direction, and cut speeds and can't seem to get it any better. My final settings using a Hypertherm 1250 are 137V THC, 80Amp,50 IPM. I would really appreciate any info on whether this is normal or suggestions on how to get it a little better.

Thanks for your time

Chris

[jimcolt]

Here are some rules of thumb to minimize hole taper:
- Holes are always cut counter clockwise (unless you have a special counterclockwise gas swirl in your torch!) with plasma.....as the process is directional. If the torch is moving away from you...the squarer edge will be to the right side of the torch.
-Program the cut speed on your holes at approx 50 to 60% of your best speeds for perimeter cutting....(if your cutting machine and software allows for feedrate overides in the part program machine codes) this slower speed will produce low speed dross on the bottom edge of the holes....but will minimize taper.
-If you are slowing the cut speed on holes as mentioned above....it will also be necessary to freeze the torch height, (if you don't...the arc voltage THC will move the torch too close to the plate when the cut speed gets too slow)....after the pierce is complete and the thc has indexed the torch down to the manufacturers recomended cut height. With the Powermax1250...the torch should pierce at 3/32" and cut at 1/16" off the plate.
-Holes should be programmed with a straight lead in....as long as possible to allow the torch height to adjust before getting to the radius. There should be no lead out...rather, and overburn of approx .200" that stays on the radius past 360 degrees. This will minimize the divot that is produced by the start stop action of the plasma at the lead in point.

I have a presentation on best practices for hole cutting....if anyone is interested email me directly at [email protected] and I will email it back to you.

Best regards, Jim

[patriot customs]

Thanks Jim
Just a couple questions to make sure I understand everything. So on the lead in I should go staight in perpendicular not an arc?

My perimeter cut is good around 60IPM, so I should go to 30 and turn off the THC and set it for .0625 cut height?

I am using sheetcam and then posting to Mach 3, where do I set the overburn to go past the 360 mark?

What should I expect for taper on .375 steel, best case?

Thanks in advance I appreciate youre time.

[jimcolt]

Make sure that you still allow the THC to pierce at the correct pierce height....then index down to the cut height...then freeze. On most industrial cnc controls / THC systems you would have an M50 (height freeze) code in the part program any place on the part that you expect the speed to slow down....hopefully the M50 still allows for initial height sensing and a move to the proper cut height...once the pierce is complete. These features are all pretty standard on industrial plasma/cnc/thc systems...and are necessary to get best hole quality.

Yes...I would try 30 to 40 ipm on holes.

The object of the overburn is to allow the plasma to shut off while there is still motion....with some cnc's and software you can actually program an overburn (maybe .2 " or so) and then shut the plasma off right at the kerf crossing point (from the lead in)...yet keep the motion going. The plasma does not instantly extinguish....so if you stop motion and plasma at the same time....the torch tends to make a divot in the hole......by keeping the motion going on the radius of the hole...the divot is eliminated and you have a bit of a "planing" effect that smooths out the lead in divot.

As far as my preference for a straight lead in: Straight lead ins seem to work well only if you have a mechanically tight cutting machine with good acceleration and de-acceleration rates...in other words your machine stays on path and has a very small "following error". Good accleration for a plasma machine is in the 50 to 60 miligee range.

If your machine is mechanically sloppy or has poor accleration...then you may want to experiment with radial lead ins.

Straight lead ins are good for the plasma arc.....as there is less deflection in the arc with a 90 degree kerf crossing as compared to merging into a radial lead in. The arc is a transfered arc....and it will tend to jump to the side of the kerf....and you can visualize what effect that has on the hole with a radial lead in vs a 90 degree kerf crossing on a straight lead in.

Jim

[tof1]

I'm bringing this back from the dead. I cut some 1/2" steel today w/ my Powermax 1000 w/ 60A consumables at the recommended optimum settings. I got smooth cuts with little dross but got pretty bad taper on the holes and straights. The kerf on top was 0.08" and the kerf on the bottom was 0.05". I was cutting at 27IPM, should I slow it down even more?

Reading your first post Jim, I don't understand why cuts always need to be cut counter clockwise? Does that mean everything I cut should be counter clockwise?

Thanks for any help.

[jimcolt]

Plasma is directional.....If you are cutting a ring....the ID should be cut in the ccw direction and the od cut cw. This puts the least amount of bevel on the part...and the most bevel on the scrap. If the torch is cutting in a straight line headed north.....the kerf on the east side will have less taper than the kerf on the west. This is caused by the swirl of the plasma jet...which is created by the swirl ring. If there was no swirl....then both sides would have a severe taper.

The taper on your hole sounds slightly excessive....and you mention that the taper on the edge is excessive as well. If the torch is too high off the plate...taper will be affected....try running closer to the plate. There will be a slight amount of taper with an air plasma.....a high definition oxygen plasma can eliminate taper.

Jim

[tof1]

How much taper should I expect to see? Right now it's about 10 degrees...

I was cutting at 0.062" should I try 0.050" or less?

[jimcolt]

On 1/2" material your taper should be in the 1 to 4 degree range. If you are truly seeing 10 degrees....then most likely you have a damaged nozzle and/or shield orifice. The nozzle orifice likely would be damaged from piercing too close, or with inadequate pierce delay time.

Inspect the nozzle orifice with a magnifier....if the orifice has any nicks or out of round issues...replace it.

Jim

[jimcolt]

The cut height should be set at the recommendation in the Hypertherm manual.....I don't have that manual with me right now...but I think it should be cutting at .062", and piercing at double that for 1/2" material.

[tof1]

The consumables look good... The recommended arc voltage is 141 but I had to cut at 153 to hold a 0.062" cut height. Could that be a problem??

Thanks again!

[jimcolt]

The arc voltage will vary with speed.....if you cut slower than the optimum settings in the manual.....then the voltage at a given height will be higher....this is because the plasma is still producing the same output power in amps...but you are traveling slower.....effectily cutting a wider kerf....which makes the arc length (voltage) longer (higher). It is more important to maintain the physical height than to maintain the voltage.

Any chance of getting pictures of these holes and external cuts with the 10 degree taper? Also a picture of the nozzle orifice that was used to do the cut? Which consumables are you using (amps)?

I am not sure that I could make my plasma produce a bevel that bad on 1/2" plate without nozzle damage of some sort!

Jim