2D Pocket Machining

[dankoenigsfeld]

Hello, I have been looking at several suggestions and can't seem to get this one figured out. I am trying to cut several parts out of a sheet of plywood, with dado cuts for assembly. When using Fusion 360 2D Pocket Machining, it skips "some" of the dados. It seems to be a bit random which are skipped and which are not. The slots are 0.48" wide using a 0.25" endmill. I've tried a number of tips found in forums, but none seem to work. There is also no error in Fusion telling me that some of my geometry has been skipped.

Please help!

[engineguy]

@dankoenigsfeld 

Does the image below work for you ? Used "Both Ways", reduced the "Stepover" and set "Preserve Order", then removed the selections and re-selected, all seems good 🙂

[dankoenigsfeld]

Yes, the image shown is exactly what I'm after. But I have a few questions:

1. I cannot repeat the success you had on my PC. When I reduce stepover to 0.1" and check both Preserve Order and Both Ways, it still will not machine the other pockets. When I download and open your file, and right click the 2D Pocket feature and click "generate", the toolpath again skips those 3 pockets.

2. Is there a reason that you need to run 0.1" stepover with a 0.25" bit? In plywood, nearly full diameter stepover is pretty standard.

Thanks!

[engineguy]

@dankoenigsfeld 

I am afraid that I don`t have an answer for you on the failure to re-generate the Pocket Toolpath, it works fine here, I have done a small Screencast that I hope is of some help to you.

It also explains why I changed the Stepover, it wasn`t really a big deal as you have Leadin/out and Cutting feedrates the same so for this particular job it is OK, just explaining why I did it 🙂 🙂 🙂

Green lines are Transition/Leadin/out feedrates, Blue lines are Cutting feedrates.

Screencast link:-  https://autode.sk/2Z0DKyF

[dankoenigsfeld]

I appreciate the screencast and the help. I'm not following, why does the larger stepover require longer lead in / lead out moves? It seems like Fusion is "defaulting" to making many more moves than VCarve. For example, in the images attached, the tool "leads in" for the whole length of the slot, carves a small corner of material, lifts, rapids back to the beginning of the slot. It then leads in following the same path to machine the next corner, rapids back to the beginning of the slot. Why won't it machine its way to those corners? I'm trying to figure out if this is user error, or if the CAM functionality isn't quite ready to compete with traditional software packages.

[dankoenigsfeld]

It seems like this should be the very basic functionality of the 2D Pocket command. I design a part with a pocket in it. I select a tool that is smaller than the pocket, select my feeds and speeds, and a toolpath is generated that machines that pocket. What am I missing? Why do we need to find work arounds to generate a tool path for a flat rectangle?

[dankoenigsfeld · Accepted solution]

Found another clue along the way. If I change the origin from "Model Origin" to "Model Box Point" in the Setup dialog, it will now machine these slots as expected. Is that a bug, or is there some reason behind that?

[mattdlr89]

@dankoenigsfeld 

You need to go to preview features and turn on the following option to get it to work as you expect it to

[dylan_smith]

This seems to be a problem on our side. We're working on a fix.

[dankoenigsfeld]

Any updates on the pocket machining bugs? For a reference of just how "not optimized" the toolpath generation is, consider the part attached. The 2D Contour toolpath (manually selecting the edges of the pocket) has about 13 feet of machining distance. The 2D Pocket toolpath covering the same geometry has over 30 feet of machining distance!

The 2D Pocket toolpath will "lead in" along the slot, machine a small section, lift and rapid back to a starting point, then follow the same lead in path to get to another small pocket, lift and rapid back to start, and keep repeating. I have to be missing something painfully obvious in the settings here, right?

[engineguy]

@dankoenigsfeld 

Hmmm, apologies but I don`t see a "bug" here, this is user use of Toolpaths.

In your original example yes, the Contour is considerably faster, however it doesn`t cut all the material away, leaves a small block at every junction, the Pocket takes longer but it does clear all the material away, do you want to have to go clear those leftover small blocks later by hand? Yes save machine time but then becomes more Labour Intensive ?

That is your choice as the Operator.

By far the easiest way to do it would be to use a slightly larger cutter, a 5/16 or 3/8 instead of a 1/4 actually does the full clearance of material in about the same time as the Contour not clearing it away, see the numbers below 🙂

Contour using 1/4in cutter = 13.264ft in 2.42 mins but doesnt clear all

Pocket using 3/8in cutter = 14.578ft in 2.47 mins and clears all (5/16 is almost the same)

That`s with Feeds set "like for like".

Summary, you are expecting the Pocket to clear all material away using the 1/4 cutter versus the Contour that is not clearing all the material away in the same time? This it cannot possibly do, IMHO your expectations are a bit "skewed" as far as your example is concerned anyway.

Either us a larger cuutter or run the smaller one faster, only options that I can see 🙂 🙂

Aplogies if this not what you want to hear 😞

[dankoenigsfeld]

But why is there so much additional, overlapping, duplicated, lift out of the cut and return to the beginning of the cut toolpath here? The pocket toolpath cuts the exact same path over and over as a lead in on its way to those intersections, and then cuts it again as a final cut. Why doesn't the pocket tool path cut like the contour tool path and knock out the extra material at the intersections as it goes by? I would expect a few extra inches to cut the pocket, not an extra 10-15 feet!

I understand that I could use a 3/8 cutter to work around this issue. But I don’t accept that the tool path generated is anywhere close to reasonably optimized. The fact that it makes so many long, duplicate "lead-in" cuts, removing no additional material along the way, seems like it has to be either a bug or a setting I've incorrectly applied.

I sincerely appreciate the help. But there are other features that I need to machine with a 1/4" bit on this project. I’m just looking for finding a tool path that doesn't make anyone watching ask "why are you cutting the same spot over and over?"

[seth.madore]

@dankoenigsfeld I've taken a look at this file and the toolpath, and I do agree, it could be a heck of a lot more efficient than it is. I've opened up CAM-35342 to investigate this issue. I don't think it's a bug, just doing a poor job of calculating an efficient path.

[dankoenigsfeld]

Thanks Seth. Don't rule out the possibility of user error as well. I'm pretty new to the manufacturing piece of Fusion. Appreciate the look!

[seth.madore]

I've thrown a bunch of different options at it, and the results are always the same. I don't think it's user error, but just a really poor solve on Fusion's part.