Bevel on 1/4” plate (Everlast 82i)

Cut my first piece of thicker plate today. Need some help.

Been cutting tons of decorative stuff and had noticed a slight bevel, but nothing major for decorative.

I started by checking the squareness of the torch to material and indeed it was out a fair amount. I adjusted it to be square and got started….

It was a mess of a day. Burnt a bunch of metal figuring out speeds and amps…my best product ended up being at 45A/60 psi/32 IPM at a height of .063 (I think, need to verify this). I ended up with really straight cuts on the straight portions but the turns and especially the hole leave a lot to be desired.

Any help is appreciated and pics for reference.


I realize these don’t show the issue well so will update tomorrow with pictures showing the bevel.

Bevel is top to bottom. Part thicker at bottom than top.

You should increase air psi to torch 70-75 psi and cut height set .060, you will have better outcome.

10-4. Thanks for the feedback. Will do a test run there and report back.

If your going to be using 45 amps you need to be using a 1.0mm/50 amp cutting tip for best results.

I was using a 1.0 tip. I’m open for suggestions.

I have been using the chart I found here for a 62i machine and adjusting it as I go.

If the bevel is only on curves, that indicates that you need to slow down on those areas. The arc trails the torch and that is not a problem on straight cuts. On curves, that trailing arc doesn’t exactly follow the same path as the torch. The result of that is the top of the cut matches the torch path, but the bottom of the cut will be beveled. The slower you go around curves, the less the arc trails behind the torch, so there is less bevel.

In Sheetcam, you can set path rules that slow down the travel speed on tight curves and holes. In Fusion, I don’t know if you can slow down for curves, but you can program the holes separately.

1 Like

I posted a link on the Facebook page you posted in, it helped me some. I’m using fusion 360 and I think my issue now is it won’t slow down for corners. I make two cut paths for my circles and outlines. Fusion just made this Harder because the free version won’t let you post process two cuts paths at the same time anymore. Hope it helps

1 Like

George, I have heard people say it’s best to run the max amperage for size of tip and adjust feeds from there. Any truth to that? I understand the size difference and amperage that correlates with that. Along with air pressure.

For this example as he said he’s running 45a. If he uses a 50a tip, she he just run at 50a and dial up his feed rate?

You can but some times it seems to work out better with less amp settings.

You could also use a 40 amp tip and run it at 45 amps. You get a finer cut, but the trade off is tip will wear out a lot faster as its not made for a higher amp setting.

This is where you may adjust feed rate optimization to slow down in corners.

3 Likes

Oh man. Thank you! I tend that once I find something that works I don’t like to change it. (Put my head in the sand) Fusion has so many features it’s mind boggling. I’ll definitely be trying this out. I guess I just watched too many youbtube videos where people get the settings working close enough and then don’t touch anything else that could make it better.

1 Like

You are welcome.

A good staring point for your “reduced feedrate” is about 60% of your “cutting feedrate”

So for your current “cutting feedrate” setting of 32 ipm I would your “reduced feedrate” to 19 ipm

(The slow feed will increase dross but reduce bevel)

a few other tips.

  • use a “finishing overlap” ( picture below )

  • make sure the “reduced feed radius” is less then the hole being cut. ( picture below )


And it is constantly being added to and updated.

Are you developing tool paths from a sketch or a body in Fusion 360?

Please let us know how the changes works for you.

1 Like

Using fusion 360. Was looking at sheet cam but I have a mac so not the easiest to swap over to pc or run parallels.

Most recent change in fusion I noticed was making multiple tool paths for different speeds. It now doesn’t allow it when is used to unless you pay for it. So I make two files and make sure I go to work 0 on my table and run inner cuts first then go to work 0 and run outline cut.

Thanks so much for that! I haven’t done a ton of g-code so learning as I go!

1 Like