Achievable edge taper accuracy for industrial type parts

[Simko]

I have been cutting artsy stuff for friends and family now for about a month now and I am getting more comfortable with the table and the Hypertherm. The CandCNC controls, CommandCNC, and the Hypertherm really do make it pretty easy. I see a lot of posts about people fighting with feed speeds and cut heights and all I do is use the book specs in the tool set and click RUN and I end up with very good cuts with minimal dross. So far I have cut 12ga, 1/4" SS, and 1/2" mild.

When I set the table up initially, I did my motor step / travel calculations by traveling 20" in each direction. This was good enough for cutting out artsy stuff, but I was recently approached to cut some parts where the sizes of the part features were fairly critical. It was a machine spare part where I cut the outline actual size and then cut the holes / slots 0.020" under and they finish them out on a mill.

I went back and redid my motor step / travel calculations by traveling 60" in the X direction and 100" in the Y direction. I would say that right now the table is as close as it is going to get.

So my question is... What would be considered an acceptable amount of edge taper for plasma cut parts?

If I cut a 1" x 1" square and measure the top edge of the taper with calipers, I will be within 1 or 2 thou on the overall width which is better than I thought I would be able to get with a plasma cutter.

If I measure the bottom edge of the cut, I find that I am more like 20 to 25 thou. Is this an acceptable edge taper or can better be achieved?

I did not use new consumables, but the ones that I did use only have about 75 pierces on them and have been used at the proper pierce/cut heights with THC.

I just want to make sure that I am providing the best that I can achieve while also not expecting the machine to do something it is not capable of.

[jimcolt]

I have been cutting artsy stuff for friends and family now for about a month now and I am getting more comfortable with the table and the Hypertherm. The CandCNC controls and CommandCNC really do make it pretty easy. I see a lot of posts about people fighting with feed speeds and cut heights and all I do is use the book specs in the tool set and click RUN and I end up with very good cuts with minimal dross. So far I have cut 12ga, 1/4" SS, and 1/2" mild.

When I set the table up initially, I did my motor step / travel calculations by traveling 20" in each direction. This was good enough for cutting out artsy stuff, but I was recently approached to cut some parts where the sizes of the part features were fairly critical. It was a machine spare part where I cut the outline and cut the holes / slots 0.020" under and they finish them out on a mill.

I went back and redid my motor step / travel calculations by traveling 60" in the X direction and 100" in the Y direction. I would say that right now the table is as close as it is going to get.

So my question is... What would be considered an acceptable amount of edge taper for plasma cut parts? This is dependent on what you mean by plasma. Air Plasma? Oxygen Plasma? HyDefinition Plasma? Hydef plasma on steel can cut holes with no taper, no ding or divot and virtually no edge hardening, assuming the cnc machine and software can use TrueHole technology from Hypertherm....expect to pay over $80k for one of these machines. At the other end of the spectrum...a Hypertherm air plasma using shielded technology with cut 1/2" steel with a 1.5 to 2 degree taper (larger at the bottom), however holes (if done using best practices) will have a taper that is more pronounced as the diameter gets smaller. A 1/2" hole in 1/2" steel will have a bottom dimension that is approximately .035" smaller in diameter than the top. There will also be edge hardness that is caused by the nitrogen content in air....which creates a nitride hardening of about .006" thickness on the cut edge.

If I cut a 1" x 1" square and measure the top edge of the taper with calipers, I will be within 1 or 2 thou on the overall width which is better than I thought I would be able to get with a plasma cutter. What thickness? Thicker will have more deviation between top and bottom, but less measured angularity, thinner is just the opposite with less measured top to bottom diviation, more angularity.

If I measure the bottom edge of the cut, I find that I am more like 20 to 25 thou. Is this an acceptable edge taper or can better be achieved?

I did not use new consumables, but the ones that I did use only have about 75 pierces on them and have been used at the proper pierce/cut heights with THC.Assuming you pierced at the correct physical height and use the suggested pierce delay time....the nozzle was probably cutting like a new one. If you see dramatic variation in angularity, then your nozzle or shield are damaged from piercing.

I just want to make sure that I am providing the best that I can achieve while also not expecting the machine to do something it is not capable of.

Attached is a cut sample with various hole sizes on 1/4", and a cut sample showing edge angularity on 3/8"


Jim Colt Hypertherm

[/attachment]

dimensions.jpg (106.35 KiB) Viewed 1447 times

dimensions.jpg (106.35 KiB) Viewed 1447 times

Powermax45 edge angle 003.jpg (28.45 KiB) Viewed 1444 times

Powermax45 edge angle 003.jpg (28.45 KiB) Viewed 1444 times

Powermax45 edge angle 004.jpg (36.83 KiB) Viewed 1444 times

Powermax45 edge angle 004.jpg (36.83 KiB) Viewed 1444 times

[Simko]

Thanks for the response Jim.

I was looking for input on what to expect from my Hypertherm 85 on my custom table with CandCNC controls. I guess I also should have mentioned what thickness plate I was cutting...doh!

The parts that I cut last night were cut from 1/4" stainless steel and the holes/slots were 0.235" diameter/width. The top of the features were within a few thou of the programmed dimension, and the bottom was about 0.025" smaller. According to your picture, my cut was actually pretty good as your 1/4" hole in 1/4" mild shows 0.040" smaller.

Being new to this, I guess I was just trying to see when I should be making adjustments and when I am at the limits of the process. The pictures you posted are perfect and make me feel much better about how my cuts went last night.

Thanks!

[motoguy]

With everything cutting correctly (consumables in good shape, etc), I just plan on 3 degree taper. Jim states that 1.5-2 degrees is possible, so 3 gives me some "wiggle room". You can take 3 degree taper and your material thickness, and get an idea of the distance. Just figure the triangle. For instance as a visual reference, use:

http://www.calculator.net/triangle-calculator.html

Enter your material thickness as side X (.5 in this case), 90 degrees as angle A (perpendicular to the table), and 3 degrees (expected taper for air plasma) as angle c. Click calculate. Side 3/Z is the distance off the cut line you'll be, due to taper. .0262", in this situation.

plasma taper.JPG (40.36 KiB) Viewed 1433 times

plasma taper.JPG (40.36 KiB) Viewed 1433 times

That's for a single side. So, if you're cutting a half inch hole, you'll need to double that (for both sides), meaning the bottom of your hole will be .0524" smaller than the top. That assumes you slow your feedrate down 50% or so to offset the bevel issues that occur when cutting holes. For outside cuts, your part would be .0524" oversize on the bottom.

[Simko]

Thanks motoguy....

Good info!