How to eliminate Rings/Toolmarks/StepOver Issue Fusion 360?

Looking for a little help here.

So when I carve these I am ending up with a tool marks or rings across the radial surface.
These rings are not raised, i.e. can not really feel them when running my hand across and cant catch my nail on them, i.e. doesn’t seem like very pronounced physical ridges and it doesn’t appear to be tool burning.

There is only one toolpath for this particular inner section/pocket. My guess is that these are marks left behind due to the stepover settings. Now while yes I can sand these out, honestly it takes way too long (not cost efficient), difficult (being that its a circular area, and have to start at an 80 grit just to get them to start disappearing and go all the way to 220 or higher and still can end up with potential sanding marks.

These items are made from walnut, and are 4" in circumference if that helps.

Below I have posted photos of the item directly as it comes off the CNC bed, as well as screen shots of the settings for the specific toolpath that takes care of that inner pocket where the issue is arising.

Hoping someone can help me figure this out, because adding about an hour or 2 finish sanding by hand to each order is not only killing time and money but my hands.

Thank you in advance. Been trying to solve this for a while and my brain still struggles with step over and numbers etc.

Images of Settings.

I think this might be a result of the bit used. possibly try a 2 flute downcut with a flat bottom as opposed to the fishtail.

Some people might say tram, but since its on all 4 sides, tram wouldn’t be the answer here.

1 Like

Would any of these work? These are some of the other ones I have on hand currently -



And also, not familar with tram. Thanks as always seth!

I would give the 2 flute straight bit, the 1/8" one a shot, Also make sure that there is a thin (0.02-0.03" ish) final pass rather than all thicker even depth passes…


Will give it a shot today and update after.

How should I go about doing the thinner pass part you recommended?

I’d leave a very small amount of axial stock to leave (0.005"). Then hit it with a full depth finish pass at full feed (literally as fast as your machine will move) and a smaller stepover (0.035").

I’d also try increasing your feedrate. You’re going pretty slow and rubbing the wood. If you need to, decrease your DOC (add multiple depths in Fusion).

Ill have to play around with this, never done a stock to leave option so this is all new to me.

Gotta figure these out so I dont have to sand for hour’s by hand. :sweat_smile:

You were recommending I up my spindle speed settings correct or just the cutting feedrate section?

You want to increase your feedrate. You’re running a chipload of about .001"…that’s pretty low in wood. You’re using an X-Carve Pro, right? I think you should be able to do 75ipm without an issue. That’ll just about double your chipload and productivity. If it’s too much, decrease the DOC.
I don’t have an XCP, but I would assume it’s capable of even more than that.

You’ll never completely machine away tool marks…don’t be ashamed of them.

1 Like

in addition to the other excellent comments above, you could always look at a finishing parallel pass in the same direction as the wood grain, in conjunction with a contour pass to ensure the edge is clean.


Really appreciate this thanks, the contour toolpath for cleaning up the inner ring circumference is a great idea.

In general my knowledge of finishing passes is very low, still learning and somewhat new to cad/cnc, but not 3d.

My very limited experience with finishing passes is turning on finishing pass at final depth.

Should, or am I able, to add/edit finishing passes within a toolpath ive already created or would I need to create a new toolpath, a duplicate of the previous (first rough), and have that be set up as the finishing pass?

Really appreciate all the help guys, seriously gold!

Yes Im running the XCP. Going to definitely look at upping the ipm! Thank you!

And haha not ashamed of tool marks, just cant have them be direct in the customers face :joy:.

You can do as many finishing passes as you want. For 3d surfaces I typically finish with a parallel pass in one direction and then another at a 90° angle.

This may be a slightly different answer, as I think the question I was asking here -

May have been misunderstood.

This was specifically asking if I set up my finishing passes inside the toolpath ive created to carve out a pocket etc etc. Or if I make a seperate toolpath just specificially for finishing.

I.e. - rough + finishing = 1 tool path, or , rough + finishing = 2 tool paths.

Thank you!

I think your answers depend upon what program you are using. If you are just using Easel you would need to set up a seperate finishing pass. I use Vetrics and can set up the final pass in my normal toolpath,

1 Like

Toolpaths are just the paths the tool takes.
You can have multiple operations under one setup (I think this is what you’re asking). Meaning you can start the job and it will run all operations without your intervention (assuming no tool changes).
You can also specify multiple depths and include a finishing pass within your pocket operation. I’d recommend just creating a separate operation for the finishing, though. You won’t notice anything when it switches from roughing to finishing other than maybe a retract and change in feedrate.

The subject title says the program. Fusion 360, but thanks for the insight, good to know!


Great info but still not sure we are entirely on the same page still.

If you are cutting, say a circle shaped pocket out of wood, the first carve, or removal of material wood, is say the rough pass, and then the second pass, is the finishing pass. That is 2 different movements, 2 different actions the cnc is doing. The question is - is it easier to set up the finishing pass within the same toolpath as the first operation, or is it better and or easier to just make an entirely new second tool path, whether under the same setup or not, that is only the finishing pass.

I know about setups, how they work, that I can put as many toolpaths as I want, I know what a toolpath is, i know about nc commands, and bit switches, start, pause, stop etc. Just not well versed with soing finishing passes. Per the last part of your answer it seems you are recomending just creating a whole new toolpath dedicated to finishing?

Hopefully that clears it up.
Thank you again, still great information!

@CorbinElliot yes - new toolpaths for each part of the job - so dedicated finishing toolpaths to solve the issue your facing at the moment. You can see when you hover on a toolpath icon whether Fusion recommends it as a roughing or finishing strategy… So you could create a new parallel toolpath to follow your 2D existing toolpaths. The new toolpaths can be 2D or 3D.

I’m somewhat new to this myself but have found various great youtube videos, and I also got someone from Fiverr to run a teaching session with me on this topic.