Cutting at an angle?

So i’m cutting some 3/8 steel flanges, about 50amps, 12ipm, and it cuts fine, but I’m getting bad holes, especially the bolt holes, so bad they are oversized on the top(like they are supose to be), and i can’t even put the bolt in on the bottom. I’ve upped the amps, but that didn’t help any. Should I slow the speed down even more? Any ideas?

Hole cutting speeds with a hole diameter under ~1-1/2" needs to be slowed down to somewhere between 50%-60% of travel speed. So about 6-7 IPM in your case. Also you didn’t mention bolt hole diameter. I limit my minimum bolt hole diameter to 1.5 x thickness. Around 9/16" for 3/8" material.


The runner holes are 1.650, and the bolt holes are 3/8. Is there a way to set the holes to 5-6 and the outside to 12? The outside looks really nice, and i think 6 would be super slow… But if that’s what it needs That’s what i’ll do.

You will need to create two different tool paths.
One tool path for the holes and another tool path for the outside profile. Then select/highlight the main setup and post process.

1 Like

So, I started cutting at a slower speed, now my flange’s bolt holes seem to be straighter down, but are not coming out circles, more like ovals, and it looks terrible. The Collector holes, and the outer parameter are really nice.

I slowed the speed to 6, and i even tried even slower then that, it doesn’t seem like its helping any. I’m about 55-60amps, if i go to 50, the holes don’t start cutting immediately and mess up.

Any ideas?

3/8 on 3/8 maybe tough maybe just drill those

1 Like

As Burgs04 said above he limits minimum bolt hole diameter to 1.5 x thickness

3/8 @ 0.375 by that formula is 0.5625 (9/16)


You are asking way too much for the process you are using. I would drill the 3/8" holes.

What I would do if I was cutting a flange is as follows.

  1. setup a tool with a kerf width of .374" and a 50 ipm speed.

  2. setup a tool with your normal kerf width and a speed of 12 ipm

  3. setup up a tool with your normal kerf width and a speed of 7 ipm

  4. in the manufacture tab create a cut profile for just the holes with a diameter of 3/8" and select the tool with a kerf of .374. No lead in, no lead out, no pierce clearance. (This will spot the center of the 3/8" hole with a pierce. The machine thinks it’s making a 3/8" hole but since your kerf width is so wide it actually creates a hole the diameter of your kerf plus .001)

  5. create a cut profile for any circles under 1.5" diameter and set the tool as the one with 7 ipm.

  6. create a cut profile for everything else with your tool at 12 ipm

  7. highlight/select the setup above the 3 cut profiles you just created and click post process and continue as normal.

  8. pull the flange off the table and dress it up. Use a drill press to drill the spotted holes.


Use a cobalt, carbide or titanium bit since the edges of the holes will be work hardened. Standard steel bits will dull zippy quick.

I mean, I purchased this for the big idea of making flanges for my shop, and that’s one of the big things in their “commercial” so I don’t think i’m asking for a terribly crazy thing. Would going to a 5/16 thickness work better, i don’t think i would have an issue in quality going to 5/16 if it means i can have a nicer bolt hole. I also realized, because i had someone make the header flange for me in autocad, that the holes are slightly smaller then 3/8, and are actually .36, instead of .375, so that may help a little bit atleast, going to the correct size, even by a little.

My biggest issue, Is i’ve purchased 3 different drill bits, and none want to drill these holes more then 2 or 3, then the bit goes dull, even with constant oil etc.

Recording a video of the process you use to create the holes with a drill bit would be helpful.



For me going to 5/16" material I would only attempt a 1/2" diameter hole. If you were to follow 1.5 x thickness equation you would need 1/4" material to yield a 3/8" hole. For plate material, 3/16" thick and up, I generally drill all my holes that are under 1/2" diameter unless I’m cutting sheet. A 1/2" hole in 16 ga material is no problem. .062 x 1.5 =.091" minimum diameter hole.

Get some good drill bits. Preferably cobalt drill bits. Black oxide and titanium is only a coating on the bits and it wears down fast. Plus when sharpening these bits you remove the coating. Cobalt is infused in the drill bit and you can sharpen these bits without sacrificing cut performance.

Drill the holes all the way thru with a 1/4" drill bit then finish the hole with a 3/8" drill bit.

What material are you cutting?

1 Like

Instead of oversizing holes (which is what I do) you can always change the kerf too if you dont want to change your design.

Also what size holes?
the general rule of thumb is the hole size should be at least the size of the material to get decent results.
And that’s with a high end system for the 1:1 ratio

1 Like

To be clear bevels on holes isn’t a failing of the machine it’s a limit of the physics of plasma. You’re cutting with a cone. The thicker the material the bigger the bevel. With a hole you see bevel x2 because both sides are beveled as well as the way curves are handled within mach 3 The bevel can be limited by slowing the cut down (this may increase the dross on the back) or designed with the limits in mind.

Bevels happen when cutting with Lasers as well. With a laser the bevel isn’t as big.

1 Like