Cant generate tool path with a lead in/pierce clearance

[pseebald]

Hello all, I am fairly new to Fusion 360 but have had some decent success.  I am designing a 2D sign to be plasma cut.  Everything is smooth besides one contour I cannot get to cut without zeroing out lead in and pierce clearance.  It is probably the largest hole in the design so lead in shouldn't be an issue.  I have tried every possible combination of numbers I can think of and have even redrew the circle.  The warnings I am getting are one or more passes discarded, no passes to link, empty toolpath.  

Added in the file.

Tried to add a screen cast from my screen cast but it says invalid link, added it as MP4 instead

[MattWynn]

Hello @pseebald - wow there are a lot of people cutting signs with circular holes recently!

This is a known issue with large arcs on inside holes, we have a fix but getting it delivered to users is a slow process.

The issue is the large arc next to lines.  I would say add some tiny lines along the arc to break it up into arcs less than 90 degrees.
@engineguy recently found that changing corner mode to keep sharp corners helped , see Re: Troubles with CNC plasma cuttin my fusion design so you might have success with that.

[pseebald]

Appreciate the reply!  That didn't seem to work for me.  I changed the original arc to a construction line and used the fit point spline tool to create an arc with about 10 points.  I am still experiencing the same issue.  In addition, I tried the sharp corners option and that didn't work either.  It seems my issue is slightly different than the link you provided.  I can only get a tool path to generate if I get rid of lead in and pierce clearance.  Thanks again for your time.

[engineguy · Accepted solution]

@pseebald 

Yes, your particular design does seem to be acting a little differently and the usual "workarounds" don`t seem to apply 😞 😞

However I did find that it will toolpath with Lead in/out and Pierce Clearance, I did find that it toolpathed reasonably quickly as long as the Lead out was kept down to about 0.06 with a Pierce clearance as you set it to 0.049, this is something that sometimes works and if you are not too fussy about the design and are happy to "live with" then putting a very small radius of 0.05 in each of the corners, one each side of the large central arc and it works, do it on the solid model and not on the sketch, seems to be easier there 🙂 🙂 🙂

[MattWynn · Accepted solution]

I split the big arc in the sketch into 5 smaller arcs using the sketch break function, and changed the lead to 0.2" in and .1" out and seems to work.

You should be able to download from https://a360.co/3lHtl2P 

The system is checking the angle at the corner farthest to the -X and down to -Y.  It is using the angle from the start to the end of the segments, not knowing that the segment is a huge arc, and it get the angle wrong.  Smaller arcs get better angles.

[pseebald]

That’s an interesting work around. I’ll check it out next time I get on. Thanks for the reply!

[pseebald]

I haven’t used the sketch break function. I’ll have to look around and check into that. I split up the arc like originally mentioned but haven’t tried the sketch break function. I’ll check it out tomorrow when I’m on. Thanks for the help! I’ll report back. 

[mark.garratt01]

OH OH  OH 

@MattWynn @pseebald @engineguy I think I can help........ and it's only because of this forum and a guy from Macrocut Ryan I can offer my 2c worth.

Ok, I too have the same problem as @MattWynn said:

and the issues I found were the same, it did my head in but the solution that worked for me was 

1. In the cutting Tab,> passes I changed the outer corner mode to Keep sharp corners.
2. I changed the leading radius to 180deg and had a longer lead-in so the pierce cut was well away from the stock I want to keep.

Can I assume in the fusion360 simulate the cutout works but when you go to the plasma it won't cut out properly?

If so here is my solution, but please remember am a newbie too, an older fella who is on a learning curve so big I need to nap every hour... 

In your plasma set-up in fusion , you need to check your POST PROCESSING and I will post the settings that Ryan helped me set up and this worked a treat. 

My plasma cutter is a CNC Macrocut Intercut3 running a Hypertherm 45 3phase unit. 

I hope i have not broken any rules for posting this type of file. and I hope that I have helped in any way. 

[pseebald]

Thanks for the info and taking the time to write back to me.  I am in fusion now and will check out some of those suggestions.  I wasn't even able to get to the cutting portion with this design.  I couldn't get it to generate a tool path.  To your second point, I have a post processing file I use from my table manufacturer but will keep that one in my back pocket.  Thanks again for your suggestion. I am new here as well and trying to find my way through when I encounter a problem.  Will report back here shortly.

[pseebald]

@MattWynn and @engineguy so it looks like there are a couple ways to skin this cat.  Breaking up the arc seems to be one of the solutions and removing the sharp corners at the end as well.  The easiest method was getting rid of the sharp corners at the end of the arc.  That allowed me to do any possible combination of lead in.  Breaking up the arc worked as well but was also a little finicky. This issue seems a bit strange.  Personally, I am glad it was not a major error on my part but something that is being worked on.  Thank you everyone for the quick replies and for teaching me other ways to solve some of the quirks.