Problems with Fusion 360 toolpaths

[daniellyall]

Do you have radious turned on or off in the pre post dialog, What is your tolerance set too, and do you have feed optimization set. And your file would help

[Andrew22]

I don't see an option to turn radius on or off in the pre post dialog when using wincnc. Tolerance is set to .005" and feed optimization is off. It sounds like feed optimization would only be beneficial if I were machining tight corners, would there be any reason to use it on this part?

[cygnus x-1]

I'm using the wincnc post processor. I tried using the cncrouterparts post as well as the mach 3 post but UCCNC tended to have lots of processing errors when I used them. Other guys using UCCNC recommended the win cnc post and it's been the most reliable, although sounds like it could be part of the problem. I don't know enough about post processors to evaluate their shortcomings.

I would need curious to know why there are no arc sections in the code. The part it's machining was made from splines driving a lofted surface, which I know ends up as lots of little segments in a tool path, but tolerances are pretty loose on this, and I would have thought a large smoothing tolerance would let Fusion fit a few arc segments together to make a smooth path.


Sent from my iPhone using Tapatalk

Oh that's why, because the resulting arcs wouldn't be planar or helical. That's a limitation of the controller. (and possibly even G-code?) It's not the post.

For complex 3 axis motion you'll have to live with mostly small line segments. One thing that helps for smoothing though is to always set the smoothing value to 2-5x the tolerance value. Outside of this range the arc fitting doesn't work as well.

For roughing paths it can also help to loosen up the tolerance (larger numerical values) and use a larger stock to leave. Then use a tighter tolerance for finishing.


C|

[Andrew22]

I'll test out a larger smoothing vs tolerance value. Fusion likes to throw up a warning if the smoothing value is larger than the tolerance value, so I've been keeping them at a 1:1 ratio. It's too bad if Fusion can't fit helical arcs to a 3D tool path, cause whenever I have a helical ramp feeding into a part or use the bore feature, the paths are nice and smooth. Not sure if the controller handles those spiral paths in a different way than it would for a more abstract 3D move. For the most part the roughing paths are quite smooth, the only time I've seen them get choppy is during a final perimeter pass where it slows down and cuts the last bits of material before a finishing pass. That hasn't really been much of an issue though, my big concern is figuring out how to get finishing passed running nice and smooth.

[Andrew22]

I used the cncdrive version today and reposted the G code of a simple little part I needed to make. It was nothing fancy, but there were lots of arcs in the g code so I got to see if one handled them differently than the other. The cncdrive post seemed to output a smoother spiral toolpath, but it's hard to say if it's much better without more side by side testing with wincnc. One thing that was rather annoying is that there seems to be so additional starting script when the program runs, and I had to hit the start button a couple times before the program actually started running. It also seems to add a retract and pause at the end of each toolpath which the wincnc post didn't do, which didn't hurt anything, but seems like an unnecessary waste of time.

[cygnus x-1]

I'll test out a larger smoothing vs tolerance value. Fusion likes to throw up a warning if the smoothing value is larger than the tolerance value, so I've been keeping them at a 1:1 ratio.

That would be odd because it pretty much has to be larger to work. Can you post a screen shot of the error? I've never seen that one before.

It's too bad if Fusion can't fit helical arcs to a 3D tool path, cause whenever I have a helical ramp feeding into a part or use the bore feature, the paths are nice and smooth. Not sure if the controller handles those spiral paths in a different way than it would for a more abstract 3D move. For the most part the roughing paths are quite smooth, the only time I've seen them get choppy is during a final perimeter pass where it slows down and cuts the last bits of material before a finishing pass. That hasn't really been much of an issue though, my big concern is figuring out how to get finishing passed running nice and smooth.

Fusion will do simple helices; meaning that two axes do circular interpolation and the third does a simple linear feed. What it can't do (AFAIK) is circular interpolation with all 3 axes. An example would be a straight bore vs a tapered bore. With a straight bore you'll get helical moves. With a tapered bore you get lots of small linear moves because fitting arcs would require simultaneous 3 axis circular interpolation. I don't believe this is allowed in standard G-code. (Somebody correct me if I'm wrong)

Roughing paths are generally planar (XY usually) so they get heavily arc filtered.

C|

[ger21]

While the tighter curves in the sample code you posted have very short segments, the larger curves have long segments, 10-12mm long. I would think that you want a tighter tolerance, for more segments maybe?

In UCCNC, try a max Linear Error of 0.5, and Unify and Addition lengths of 1.0

[daniellyall]

Andrew22 You are way better of useing the correct post, Just post on the HSM cam forum or Fusion's Cam forum and link back to this, post a file you are have this problem with and a Gcode one of the CAM guys check that forum every few hours. or do the same here you are only going to get try this not do this this works

[Andrew22]

Here's a link to the model. A360 Let me know if that works out or if you need any more info

[daniellyall]

What toolpaths where you haveing the biggest problems with.

After a look through, there are some mistakes what are NO NO's no X set in the setup (you have this set to save problems in the toolpath and so you don't need to set this in the toolpath), Model not set in the Toolpath Fusion needs this for 3D toolpaths to work as they should.

Why 3D pocket for a roughing toolpath ??

Radial doing a near 90 degree angle change it does not like this, I did a example of another way to set it, what keeps it to the angle surfaces, it has a better looking toolpath that's a bit smoother.

Added in 3D Adaptive clearing in instead of pocket, pocket had a lot of Angle changes about 160 degree and a lot of over cutting.

Do you have a 3/4 endmill you can use and what is the stock size this is one of the problems it's showing red what means there is a problem with it.

I will be a few more hours before I post the file back

[Andrew22]

There's a couple of hidden bodies and toolpaths to go with them that may be outdated, hopefully those aren't visible and causing confusion. I see what you mean by not having the X set in the setup, but what do you mean by not having the model set in the tool path? I've got the model body selected in the setup so I assume this means something else?

I went with a 3D pocket over 3D adaptive clearing as it was a fair bit faster according to simulation with the same stepover and step-down. It makes sense that radial wouldn't like a 90 degree angle change, however that transition was always smoother than when it was running up the sides of the bowl, so I didn't pay much attention to it. I'll be interested to see your solution and how my cutting improves. I'm using a 3/4 ball end cutter for both roughing and finishing, and stock size is 16 x 11 x 4. The error your seeing might be because I have a control surface in the file that extends beyond the stock size, and I use that so that the roughing operation follows the bottom contour of that wavy lip. If I let it go right down to the bottom of the stock there's a few parts where the spindle would crash into the part, and that material gets removed from the other side anyways.

[ger21]

however that transition was always smoother than when it was running up the sides of the bowl,

The "rough" part of your g-code is made up of just a few, longer straight segments. I think that's where your problem lies. The transition between those segments.
I'm not sure if it's an issue with your model, or the toolpaths. I'm not familiar with the CAM in Fusion, so don't have any advise

[daniellyall]

Ger you are correct it's the transition, it's going from running up or down a angled surfaces to a flat surfaces in the spaces of 1mm.

Also when it gets to the flat surfaces all the toolpaths go to one point so every run up the ramp has a stepover what is correct but when it gets to the flat it overlaps that much it's wasting a lot of time, so you add a angle lock to it so it can only cut from 5 degrees to 90 degrees and it wont touch the flat.

3D pocket if it's in a pocket it's good if it's in a open pocket it can be a **** of a toolpath.

There are some setting you can change in 3D adaptive that makes it way faster than the pocket.

Also in the toolpath you had for finishing the inside scallop there is a rapid move in the middle of the toolpath, this will cause problems it rapids for 1 mm, so that will be a bang and clunk, I changed it to a morph spiral the cutter stays in contact with the surfaces for the entire cut.

Using a surfaces is just one of the tools you can use in fusion cam, you can use sketches, patches and defeatured models as well.

Defeatured models can save a lot of time and leave a better finish.

The selecting the model in the toolpath is so you can add a defeatured model and have that as what you cut, you can have as many bodies as you wont in the cam and every toolpath can be from a different body all in the same file, it does not matter one bit what body you pick.
It's also important so you can have the fixture in the setup and the body in the toolpath, It's just a good habit to stick to.

Quite often when people have problems with their cam they don't have there set up done correctly, or the toolpath set correctly.

I have added 3 patches to the bottom of the model so the cut does not try to go into the 3 hole's that are there, when you wont to cut them you just turn the patch off.

The steps that are recommended is

Do the setup first setting the orgin and the body + stock
do the toolpath
sim
fix
sim
post
read through the code
test on the machine
fix or do the cut

One thing that gets most people they don't realize how simple and powerful the toolpaths are in fusion/HSM cam, as an example you can do the set up then select 3D adaptive clearing then hit ok 2 clicks done.

When you use 3D adaptive clearing and 2D you can go balls to the wall, and do it at a insane depth and width of cut, I restrict it to 75% step over 75% depth of cut, and it runs fine, I have by mistake done a 75% width of cut and a 150% depth of cut, as I was diving for the E stop it was cutting fine so I let it go and just used feed hold to stop it and fix the mistake.

I have read on the vectric forum where people say they can't see how 3D or 2D adaptive is a good toolpath to use with a router, they have never used a 2D or 3D adaptive, constraint cutter load make a big diffrences, and it's not all that slower maybe 1 or 2 mins and the saving of the cutter wearing out pays back that minute or 2.

I am optimizing the toolpaths so you have a example of a toolpath that is fast and efficient.

[daniellyall]

He's your file back I got everything optimised as best as I can, Have a look through you will see what I did, there is a few little tricks in there what are brand new as off today, before the update the did not work too well.

The pocket toolpaths I knocked a few minutes of each one, the main way is by haveing the fine step down and the roughing step down the same. Any questions just ask.

[Andrew22]

I was using radial more for cosmetic purposes than anything else, so I ignored the time wasted as all the tool paths converge on that centre point. Good point about the angle lock though, that's a handy way to limit the tool path. I did a test with adaptive clearing, and while it was more time consuming, I think you're right in that I could tweak it some more and get a bit more speed out of it. I ran it at .8" depth of cut and .2" stepover, and 6500mm/min which cut well, but wasn't all that fast. I slowly turned my feed override to 200%, and it still cut just fine, but I noticed for a lot of the cuts the machine wouldn't accelerate fast enough to hit that max speed. It's back to the same problem where the machine won't continue accelerating through multiple segments or arcs. It's not stopping and starting like it would in exact stop mode, more like letting off the gas and then ramping back up for each segment. On the occasions where it does fully ramp up it's nice to see it cutting clean @ well over 10 000 mm/min but it's proving hard to stay at those speeds. Lighter cuts at full bit depth would be really great if I can get the feed rates high enough to keep machining time down.

I've used sketches and patches before in fusion, but I haven't done anything with defeatured models. That sounds interesting I'll have to try it out.

I'm going to study your optimized version of my file as well, that should be super helpful to see where you made some tweaks.

Thanks

[ger21]

It's back to the same problem where the machine won't continue accelerating through multiple segments or arcs

You either need to increase your acceleration, or allow UCCNC to use a larger error tolerance. If you don't want it to slow down, you need to allow UCCNC to "blend" the segments.

[Andrew22]

You either need to increase your acceleration, or allow UCCNC to use a larger error tolerance. If you don't want it to slow down, you need to allow UCCNC to "blend" the segments.

Probably a dumb question, but do you know if it's possible to set one acceleration rate for roughing and another for smoothing? I'm fine if the machine shakes a little more during roughing, but it would be slick to be able to run a macro or something like that to swap in more conservative acceleration speeds when it comes time for a finish pass.

[Andrew22]

For some reason fusion doesn't want to open the file. It gives me error message: OK

He's your file back I got everything optimised as best as I can, Have a look through you will see what I did, there is a few little tricks in there what are brand new as off today, before the update the did not work too well.

The pocket toolpaths I knocked a few minutes of each one, the main way is by haveing the fine step down and the roughing step down the same. Any questions just ask.

[daniellyall]

You should just need to open new design from file, You can loosen up the toolpaths with changing the tolerances and smoothing, in fusion then use the machine controller to do it, there was a post done by one of the cam part timers that had a good break down on set up tolerances and smoothing.

You can use feed optimization to control the cornering, this is something you have to experiment with to you find what the speed is that the controller could have problems with cv, It makes a night and day differences with mach3 when doing more than a 75 degree angle change.

but do you know if it's possible to set one acceleration rate for roughing and another for smoothing. Not in the same toolpath or In a non work around way No you can't as far as I know, the same question was asked on the forum the other day, they are thinking about it, (work around warning) the only way to do it now is a workaround by haveing a copy of the tool labeled as finish or rough with or without a different tool number in a different toolpath.

You could have it added to the post processor but that would cost $$$ unless someone on the forum did it.

they have 5 diffrent things you can do with toolpaths

use sketches
use patches
use defeatured body's
use a cam simulated model as a stl or converted to a solid. this is new
use a stock body.

Andrew I would try gers ideas as well, hes very close with any sugestion with fusion and the uccnc this below you can have the uccnc and fusion do it together or let the uccnc do it

You either need to increase your acceleration, or allow UCCNC to use a larger error tolerance. If you don't want it to slow down, you need to allow UCCNC to "blend" the segments.

[ger21]

The file opened fine for me, by just double clicking it.