Hi all, my simple part has a 1/4 inch hole in it. The hole is not coming out perfectly round. Looking for suggestions on settings that may be affecting how the hole is coming out. The outside of the part is cutting perfectly with very little backside dross. There is no topside dross at all. Material is 16ga steel.
Thanks
–Corey
What is your amperage and cutting speed set at? Are you using a lead-in or lead-out radius/distance? Is the tool moving clockwise or counterclockwise when cutting the inside hole?
Tool speed is 300 ipm with 25 amps of power. I do have a lead-in distance set, but I think it was too small. I just increased the lead-in, but have not performed another cut yet. Rotation is clockwise.
Thank you
–Corey
Generally you want to cut counterclockwise inside, and clockwise outside. 300 is also probably a little high for cutting, but is fine for travel speed. A lead-in radius of 0.05” at a 90° angle with no linear distance might also help. Good luck!
300 is way to high for a hole that size, try 70. I usually run 135 to 155 on that gage metal.
Found it and fixed it. Thanks for all the guidance fellas. I did several things to resolve this issue:
I created a separate 2D profile setup to cut the hole separately from the rest of the part. With this separate profile I was able to adjust the tool speed much lower than the tool speed for the body. The tool speed is now set to 73 in/min for the hole only. I also adjusted the lead in/out distances and angle.
I adjusted the amperage down to 27 amps from 30 amps.
I used the large shim instead of the small shim to set the torch height.
I found that the X-axis motor side set screw had worked its way loose. I tightened this up. This made a huge difference in the overall shape of the hole.
For the tool profile, I adjusted the kerf width to 0.06 inches
So, with these new settings I get very good results with little to no dross on the backside of the part. No splatter on the front either. The backside dross that is there comes off easily with a fingernail of a small chisel.
Here are the results.
Looks fantastic. When you find the sweet spot for feed rate, try 70-80% of that number for small holes and details. My opinion is 70ipm is way too slow for 16g steel. The low speed dross (round clumps and thick) at that rate is annoying. I have a 40 amp machine with a S40 torch and I cut 16g at 180ipm at 30amps .08 tips and small holes at 140ipm with great results. For really small holes, I’ll drop down to 120.
Glad you got everything dialed in! Part looks great.
