Powermax 1000 Cut speeds and height

[CJdave]

I just upgraded my table with a new drive system with torch height control. I am trying to get the best cut quality out of my system.
Right now I cut a majority of 1/4, 3/16, and some 14 ga. I have been using the cut recommendations in the manual, but have some questions. First, on 1/4 If I use the arc voltage specified in the manual and the cut speed, the torch distance is less than the book recommended 1/16", runs around .035. So my question is should I increase the cut speed? Or increase the Arc voltage setting to get the right cut height? OR is the arc voltage more important than tip height when cutting?
I seem to have a lot of cut angularity on some of my cuts, but i can't seem to predict or tune it out. I am running 60a and 60a consumables. When I cut a 1/2" hole in 1/4 it is .5 at the top and .45 at the bottom, can i get a better hole? I am getting close to dross free cuts in 1/4.
Also Can I run fine cut consumables in 3/16" ? My manual only goes to 10 ga on the fine cut chart.

[jimcolt]

Torch height is more critical than arc voltage.....adjust your height control so the height is as the Hypertherm manual suggests...and ignor the voltage setting. Many THC systems are calibrated differently.

You can cut 3/16 very well with the FineCut part...even though the specs say maximum of 10 ga. Many people use them up through 1/4"......pierce height and pierce delay times are critical on thicker than 10 gauge....pierce as high as you can, and allow enough time for the arc to be fully through before motion starts.

For best angularity on any material...use the lowest amperage consumables. If I wanted the best holes on 1/4" I would use the 40 amp shielded parts, I would program the THC to lock at the cut height (no arc voltage adjustment on any hole under 1" diameter)...and I would program the cut speed for all holes under 1" to be 60% of the optimal cut speed listed in the manual. This will minimize taper. To eliminate taper.....you need to go to a Hypertherm HPR system with a new technology called "TrueHole"....but thats will put you up in the industrial price range!

Jim Colt

[CJdave]

Jim,
Thanks for the info. Can you give me some IPM speeds to start at with a fine cut consumable and 3/16 plate?
I priced a HPR system and it's out of the price range for my shop, but I think I can achieve the quality I need for most of my stuff with the 1000. Just trying to get the most out of my current cutter.
Thanks

[jimcolt]

I would start out with about .200" pierce height, about .8 seconds pierce delay, cut height of .062, and a cut speed of approximately 65 ipm.....set the amperage at 45 amps.

Good luck, let us know how the cuts look. If there is dross....try increasing the speed.

Jim

Jim,
Thanks for the info. Can you give me some IPM speeds to start at with a fine cut consumable and 3/16 plate?
I priced a HPR system and it's out of the price range for my shop, but I think I can achieve the quality I need for most of my stuff with the 1000. Just trying to get the most out of my current cutter.
Thanks

[WSS]

I see that cut height is more important than arc volts, but how do we know when we are tracking at the right height?

Yesterday I was cutting 1/2" AR500 and forgot to turn the THC on after I had done some dry runs (new plate on the table). When I turned it on during the cut it instantly went closer, narrowed the kerf and eliminated the top side, forward running dross. It was then that I realized how critical it was.

The plate I put on the table had a pretty good warp/curve in it, so I really could not use a set point to track it because of the height difference across the sheet. I know this is probably obvious but I am not seeing how to accurately use the arc volts to control the height.

Thanks for any input!
WSS

[jimcolt]

There, contrary to popular belief, is no piece of steel on the planet that is flat enough to plasma cut without using an arc voltage (or other type of feedback) torch height control. A variation of .010" in torch to work distance affects angularity, dross formation, and kerf width. Even if your plate is perfectly flat when you start cutting....the added energy in the form of heat will cause at least some vertical movement of the plate.

Hypertherm publishes a suggested arc voltage that is usually very accurate....in other words...if you are running at the speed listed in the Hypertherm manual, using the consumables listed, and at the amperage listed.....the the torch/work distance will be correct at that arc voltage. If you decide to cut slower tha the recomended speed...and you leave the voltage at the recomended setting...the torch will move closer to the plate. If you operate at a different amperage the torch to work distance will change. As the electrode wears...the torch will move closer to the plate. If you have mositure in your air (on an air plasma system) the torch will often rise....as the mosture changes the resistance of the arc.

The best thing to do is to develop a fixed height and speed that gives you the best cut on a particular material.....then read the arc voltage. This is the voltage that will be your arc voltage setting.....as you get near the end of the electrode life....bump the voltage up...2 to5 volts at a time to maintain the correct distance.

Many high end industrial torch height controls have automatic compensation for changes in speed, and electrode wear. Most low cost...or homebuilt or entry level THC's need more attention from the operator for best performance.

Jim Colt

[WSS]

Jim,
Thanks! That helps. I have copied/pasted and will print this info for my command center.

I have not reached a point yet where it is all common place. I am still having trouble walking and chewing gum. At least now I can assemble the torch without having to reference a diagram. The most common problem I have is forgetting to set back the speed after I dry run the file. Ya, I know, eventually I will skip the dry run as well!

The machine I run is a PM1650 (100a). I use 60, 80 and 100amp parts. I notice the amp adjustment turnpot on the machine is variable rather than step. Say I am running 60 amp consumables, should I be right at 60 on the dial or is there an advantage to "varying" the setting a bit?

Thanks again
WSS

[jimcolt]

60 amp consumables are designed by our engineers to operate best at 60 amps.....higher amperage will cause shorter life, lower amperage will create a "soft" arc and poor cut quality. You can experiment, but our process design engineers have already done so! I would suggest trying out the FineCut parts for your plate thinner than 3/16".....you will be impressed with the cut quality.

After 32 years of cutting I still trip up on settings...and mess up at least part of my cutting!

The newest HPRXD industrial high definition class plasma systems are actually easier to run and operate as compared to the air plasma systems.....all of the setup is completely automated......if a Hypertherm approved CNC control, Hypertherm THC and MTC CAM software is used. The operator only needs to ensure the right consumables are in the torch....then he chooses the material type and thickness.....everything else is automated. Cut Speed, Pierce height, pierce delay, corner speed, height freeze, gas mix change for holes, advance stop, overburn, lead ins, kerf compensation are totally transparent to the operator!

Jim

[A1CNC]

I was cutting 3/16" HR steel today on my practical cnc table. I was cutting 1/4" diameter holes at 12"/min 60 A with 60A tips. Hypertherm 1000. I don't use the height control on 3/16". If I was to increase the cut speed there would be a lot of bevel, yet at this speed the edges are nearly straight. I get some dross around holes but it knocks off pretty easy. For straight cuts I was going 30"/min. There again was some dross but not much on the straights. I was using a .04" offset. BTW when I looked at the meter on the thc it was reading ~150 when the torch was ~.06- .08" above the material.

If I increased the speed to ~60"/min on the straights I would have noticeable taper. Is my machine not putting out full power?

It seems if I don't have at least a little dross on 3/16" up material, I have a noticeable taper, so what type of bevel should I have at say 60"/minute?

Thanks,
Eric

[jimcolt]

You should be using either the 40 amp shielded consumables....or FineCut consumables on 3/16" plate to minimize edge taper. Use the speeds recomended in the manual.....and use your torch height control...by controlling the torch to work distance you will control the edge taper. 60 amp parts will cut fast.....but will produce a tapered edge.

Jim

[CJdave]

Jim,
How about fine cut in aluminum? There is no recommendations in the book for aluminum with fine cut parts? I cut some 1/8", .090 and thinner 6061 and 3003 from time to time. Should I be using fine cut parts or just standard parts?
Thanks
Dave

[jimcolt]

You can pretty much follow the FineCut charts for steel....for cutting the same thicknesses of aluminum......

Jim