Anyone willing to look at a Fusion file for me?

I am going through the Titans of CNC fundamentals and I’m already stuck on the 2M.

Got it all drawn and the cam done but the tormach doesn’t like it. It throws an error that says:

G-Code error: Length of cutter compensation entry move is not greater than the tool radius

The only way I can get it to load into PP is to change the lead in to half the cutter diameter. But I think this is causing the cutter to stay off of the work by that dimension. Any thoughts? Contours 1,2,3 are the issue.

UPDATE: I can get it to load into PP by extending the lead in dimension to .255, as I said above. I am not making contact with the part even though in fusion simulation it does. All of the ops other than 2D contours are behaving as expected. I must have something set wrong either in fusion or PP.

Titan 2M v12.f3z (684.0 KB)


I would turn off wear compensation first. Unless you are running lots of parts with advanced tool measuring you won’t need or be able to use wear compensation.

1 Like

I found a work around by going to “in computer” for compensation it was able to cut the contour as designed. It does make me wonder if there is a bug in PP though.

I can’t say exactly but I know there is a lot of math going into a radius arc with lead in and wear calculation. All the fields in fusion display values but they are actually equation driven. When I have a problem I remove all of the check boxes in each operation in fusion and re add them slowly. I understand about half of the check boxes after using fusion for a couple years.


Easiest is to use ‘In Computer’ as the compensation mode. That’s all done by Fusion at the time the toolpath is calculated. The other modes involve PathPilot calculating modifications to the paths it receives from Fusion. The process it uses to do this is described starting at Cutter compensation and it is very dependent on lead in lengths. It’s pretty common for this to result in the error you’re seeing, so unless you have a specific reason to do otherwise, ‘In computer’ is generally the solution.

Thank you David, that is precisely how I resolved it (eventually). However, your explanation helps me understand why it was happening. I am using the Titan of CNC program to get my feet wet with my new machine and for some reason they have you use “wear” in the cutter compensation selection. I can’t figure out why it worked for them and not me but I can’t get bogged down with that now.

On another note, I am running your post and hope to add your probing inspection report soon!

Thanks for your help!

Titans are running industry standards. Which means using every check box in fusion and every gadget you can bolt on a machine. If you’re having problems uncheck all your boxes and try again.

Hi Scott. No problem.

Writing the post involved a lot of finding out how the code works underneath. It is Fusion that does all the calculations, but I did have to untangle some thing like this to figure out what it wanted the post to do.

I’m glad you like the post. I think many manufacturers leave a lot of untapped potential out there by spending enough time working on this. If you do try the inspection, I think you’ll find it’s another area where these machines peform much better than you’d expect.

I spoke with Kevin over at today and he believes that if I did not add the diameter of the tool in the PathPilot tool table it will work with “wear comp”. It does make sense in that it can’t be both that fixed number for diameter and a wear-adjusted number.

I’ll try to test that theory soon!


I’m not sure they are using “industry standards”. I think the are using “Titan Standards”. Different folks I’ve talked to take issue with several of the ways they do their CAM. I’m still grateful for the content and the help to get started. I have found ways to work around the issue but still want to understand it at some point. Thanks for your input.

This video from NYC CNC explains a lot of these concepts really well.


@Davie - that video is an excellent suggestion and came to me now at the right time having gotten past many basic hurdles, the advanced stuff is making sense now and stuff I can actually wrap my head around.

@Scott_Dube - Titan’s videos are supposed to be soup to nuts but IMHO they felt advanced and above my head as I’m still “just starting”, so if you keep getting stuck working through them, don’t be surprised…not sure what to recommend as slightly more basic which might be less frustrating…


I think his videos are pretty good but they do sort of dead end in certain places or just don’t always work out. That said I think they’re still worth my time to work through.

I don’t disagree of their value.

At the time, for me, they just didn’t feel like they were right for a newb looking for fairly basic material. I like a challenge but I also know when I’m in over my head and when it might be time to abandon and pivot to another approach.

I ended up with the free Autodesk Fusion training. It’s not meant to churn out parts as an outcome but I think that’s the better starting place (a few of the Fusion courses, since that’s what most folks use) and then maybe moving to their videos. I’m still learning and I don’t know that there is one tutorial to get soup to nuts for someone who has zero knowledge…

1 Like

All good points, I also think we all bring different levels of skill to the process. I’ve been using Fusion for 3 years for example. Mostly for design so I needed more help with the CAM side. I also knew very little about machining so I need help there. So for me the Titan videos were an ok jumping-off point. I’ve only done 4 so far but have 5 & 6 drawn and ready for CAM or machining.

I like the come as you are nature of this community and the ability to jump in with both feet or work around the edges.

@Ashraf_Farrag , Thanks for your thoughts and ideas!

Hi David,

I wanted to let you know I got your inspection routine running and pumping out the raw info into the .txt file. You are right it does need a front end to be more user friendly. Is your reporting program strictly windows based?


Strictly Windows I’m afraid.

1 Like

Is it OK if I pile on to the request for someone to look at a file (2 versions) and see what is going on with them? Fusion 360 on a 440.
The material is .062 copper, it’s a simple square just over an inch on each side with a hole in the center and 4 holes near each corner. The early version always cut twice the depth down from zero at model top, the latest version works better but still cuts twice the depth. If I set Z zero at .062 above the work it cuts like I want but nothing I do will change what is happening. I have measured the tool length multiple times, looked at all the tool settings and started a new sketch from what I believe to be a clean Fusion file more times than I can count. I have made so many edits to the CAM setups I am no longer sure what is what, all I know for sure is starting from scratch doesn’t seem to change anything. Can anyone take a look at these files and let me know what is wrong? (15.1 KB) (20.4 KB)

Richard these are not Fusion files they are the G-code is that what you intended to post?

Attached is the Fusion file. I’m sure it is a mess because I have made so many edits in futile attempts to correct the depth problems and search for the reasons and locations of warnings and tool path issues that Fusion tells me it has but absolutely will not tell where, what, or why so, being an absolute beginner, I either start from scratch or just shotgun edits in search of the problems.
NEW4LINK v5.f3z (652.6 KB)