I’ve been staying up late and playing in Fusion 360 and making good progress. Other than a supplementary spoil-board, the linked model will likely be the first thing I attempt to cut with my Shapeoko… (or any CNC ever for that matter).
https://a360.co/2Qn2quh
As you can see I’ve been taking everyones advice to take it slow and start simple to heart
This was my first time taking someone else’s STL files importing them into Fusion 360 dealing with a bunch of faceting and triangle errors and creating tool paths which will completely cut through my material.
There are a few things that aren’t abundantly clear to me at this juncture…
For facing operations… since i’m not defining the thickness of my stock in my model are the facing operations intelligent enough to know that since my model components are ~.6225" tall… not only should a facing operation make the work piece machine-flat but if I stick in a 2" thick stock it should face the material at the maximum stepdown (.125) for (2 - .06225)? Ergo, any machining time estimation in Fusion is totally irrelevant and will be reevaluated when I zero the z-axis?
How are my tool paths, component spacing, tab size and placement, etc…? Again, I followed a few tutorials; I’m not overly concerned with feeds and speeds at this point because I’m not sure what scrap wood material I’m going to use to create these.
Is cutting into my spoil-board on operations such as these basically unavoidable? Even if I were to get all of my stock perfectly flat on my jointer; then run it through my planner to get it co-planer, and then using the facing operations to make it machine-flat I have to imagine that there will still be 1/64" of deviation SOMEWHERE. I’m fine with having to resurface my spoil-board occasionally, just wondering if there was a trick here.
Hey Mark! That’s awesome you’ve jumped into Fusion 360. It’s a great piece of software and provides awesome functionality for milling whatever you want.
Facing operations are one of the dumbest operations in Fusion. It’s essentially a pocket but only cuts in 2 directions (one way, then 180° in the other way). All you need to specify for them are stepover and stepdown. Also, you have to define the thickness of your stock when you do CAM. Fusion won’t let you CAM anything until you tell it what stock you are cutting your parts from. So go back to your stock setup (it’s in the tab as “setup” in the CAM module) and see what you put in for your z-height.
If you put in a piece of stock 2" tall and your parts are 0.6225" tall, assuming you didn’t specify a stepdown, Fusion will try to make your Shapeoko take 1.3775" deep cuts. Make sense? So the machining time it tells you is relevant and is irrespective of where or how you zero the z-axis. Fusion doesn’t care if you zero your z-axis at all and will tell the Shapeoko to do exactly what it shows in the simulation in Fusion.
I can’t comment on this right now. I’ll add a new post when I can. Fusion is updating and won’t let me view them until it finishes…
No, it’s not if you don’t want it to be, although you are correct in the premise that there is always deviation somewhere. Typically I mill my parts down and set the bottom height ~0.1mm above the actual bottom so that I end up with an “onion skin” that I can easily cut or break off. This saves my wasteboard from being marred and I can quickly finish the part manually.
Since Fusion is done updating, I can add to my previous statements.
If you right click your setups (labeled “Dogs”, “cams”, and “Handles”), under the “Stock” tab, you can see what Fusion believes the size of your parts are. So it assumes your parts are 0.04in taller than the models you made and that’s why it can face them.
Here are my thoughts on your CAM toolpaths.
Cams
Facing stepover is fairly conservative. 0.33" stepover with a 1" face mill is only 33% of the bit being used at any time. You could probably go up to 60% stepover, just watch the depth of cut.
Your pocketing with your 1/4" endmill might be aggressive. I’m not sure what material you’re going to use but a 0.2375" stepover with a 0.125in stepdown might be too much. Typically I like stepovers around 40-60% for wood so I can cut deeper and use more of the sharp flutes I paid for.
For 2D Contours, make sure to go into the “Linking” tab and select “Keep tool down”. It’s the stupidest option that should always be checked. Without it selected, after every stepdown, it will raise the tool up and then lower it back down, oftentimes putting gouges into the work.
Also, in your 2D pocket and 2D contour toolpaths, you can go to the “Geometry” tab and change the “Top Height” from “Stock Top” to “Model Top”. You just faced your material down to the stock top so without changing this, you’ll be cutting air in these next two operations.
Dogs
I’m not sure why you went with an adaptive for these holes instead of a pocket like you did for the cams. It is fun to run and will get the same thing done in wood that pockets will with less problems.
For your 2D contour (this also applies to your other 2D contours), you don’t really need finishing stepdowns. What that does is make small stepdowns near the bottom to get a nice bottom finish on a part but since you’re cutting straight through, it just slows things down. I would remove the finishing stepdowns and save a little time (without them your time goes from 9:58 to 6:41)
Handles
The use of a 1/4" ball endmill will work well here for the sloped area but not so much for the flat areas. It will leave scallop lines or ridges and not be flat. You could constrain your 1/4" ball endmill to the sloped area and then do the flat areas with the 1/4" flat that you’ll have to use to contour the outside.
Those are all my thoughts for now. Let me know if you need anything clarified.
Everything makes sense, thank you! One quick clarification, the onion skin you speak of… is that easiest to do by setting a negative value of -.01mm in “Stock Bottom Offset” in each Setup?
There are 2 ways to do it. One method is going to the geometry or heights tab (I forget which one it is) and set the bottom height to 0.1mm or whatever height you want. The other method is to go to the “Passes” tab and go down and set the “stock to leave” z-axis height to 0.1mm.
