Mill a piece longer than machine in multiple sections?

[Anonymous]

Is there a process for working on stock longer than machinable area?

My gantry is 4'x4' with open ended Y axis. If I want to work on something 4'x8' for instance can I separate my model or paths into sections; mill the first half, pause machine, move stock forward, mill the second half? 

I have found options in Vectric, V-Carve, and this article on fixturing but can't find anything in Fusion. 

Thanks very much for your time. 

[LibertyMachine]

To my knowledge, Fusion holds no easy method of accomplishing the task you are looking to do. Pretty much the only thing I could think of doing:

Split your model in half (so you end up with 2 equal length parts), make 2 separate bodies as well as 2 separate setups.

You would need to put some thought into how you locate your part for the second operation, as a lot of the stock will be gone from the first half. One possibility; on the first op you could put in some dowel holes (in the second body) that you could locate off of for the second operation. Make sure you have the travel to accomplish that in your first op.

Perhaps this is a good candidate for the IdeaStation? (not sure if one exists already)

Little side story: Years ago I made a small 2' x 2' gantry router from scratch. Stout little machine. I ended up making some side-boards for a friends stake-body dumptruck. They were 7 feet long, fully engraved, beautiful pieces. Using MasterCam at the time, I had no option that to break it up in the manner I described above, except I had to do more than a few setups. Fun times...

[Steinwerks · Accepted solution]

Think something like this but in 3 axes:

Yes, you'll need to figure a way to locate for your next setups, so it's best not to try and split your model into the maximum travels, but to overlap where you can. Remember: a feature you use to locate your next setup doesn't have to exist after that operation. Leave posts, boxes, shallow holes for alignment, whatever you can think of.

[Anonymous]

Thank you both. I am really enjoying working in Fusion. Bit of a learning curve but I'm starting to be able to explore new concepts with minimal frustration. I had no problem splitting the model in half with a Construction Plane and Split Body. I modeled the stock and split the same way. Also created sketches of both halves of the stock. I created a setup, selected half of the stock, set geometry to silhouette, and generated a toolpath that looks like it will work quite nicely:
 

When I attempt to repeat the process on the second half however, I get "Error: Internal CAM kernel error. Please report through your support channel."

From what I can gather online it may have something to do with stock setup. I've tried every option and combination I can think of in the Setup>Stock and Geometry>Machining Boundary but can't seem to clear the error.  The best I can get is a toolpath on the stock, not the model. Is it possible I need to create another file with an entirely separate operation? Or ideally I'm missing something simple. 

Theoretically, because of the symmetry of this piece I could just flip the stock and run the operation twice, in which case I'm good to go, but I would like to solve this.

In terms of adding to the IdeaStation, may not be needed. This appears to me an excellent way to work on a part in sections as long as the kernel error can be cleared.

As far as fixturing and orientation I'll just add some temporary blocks or rails to the vacuum table or just use some marks. This will end up being four cycles in total top and bottom so I am trying to leave stock around the edges so that when it's flipped over it still lies flat. 

Here is the file if anyone wants to take a look. Thanks again. 

[Anonymous]

Are bounties appropriate? I would be happy to send $10 in BTC to anyone with a solution.

[LibertyMachine]

Haha! Sorry, I've been buried in machine setups since I cam back from "vacation". I will try to look at your file on my lunch break

[LibertyMachine]

So, I downloaded your latest file. Little sidenote: Unless you are working with a file that references other files, a faster more efficient way (for the rest of us) to share your file is to export an .f3d of the part. To do that: File > Export > Save to local folder > Come back to thread and attach

All that aside..

Your latest attempt I think might have shown a bit of frustration and/or lack of proper flow.

For the Tail side, you did not have any Model selected in the Setup, or any model selected on the Stock page. I turned off both models for the Nose, and selected what was needed for each field.

The Nose side, you had 4 bodies selected for the model (you only need the one model of the Nose piece) and the proper body selected for the Stock.

After sorting that out, I was able to regenerate the toolpaths for the Tail side. No issues.

I then copied the Parallel operation from the Tail to the Nose (ctrl+c, ctrl+v). Since it was set to Silhouette, I was able to just regenerate and call it good.

One thing to mention; I see you had Avoid/Touch turned on, but nothing selected. That is used typically when you want to machine or avoid a certain feature. Having it on with nothing selected does nothing for you (as far as I know)

I do not have any Kernel errors using this method.

See attached file.

Oh, one last thing: With the toolpath selection, you were able to get a bit of overlap going on your toolpaths, which is good. Sometimes you might not be so lucky. What I would advise: Have 2 split lines about .125" apart instead of smack dab in the middle. So split into 2 large pieces with a small sliver in the middle. Copy/paste that small sliver (on top of itself) and then using the join tool, you can combine the small sliver with one large piece, rinse repeat. This would force Fusion to give you some overlap if the tool path automatically does not (for whatever reason)

[Steinwerks]

I still think splitting the actual part is a bad idea, and completely unnecessary. Use sketches for boundaries and constrain the toolpaths. Easy that way to use a sketch box that represents machine travels and drag it to where it will be the most effective.

[LibertyMachine]

While I don't entirely share your view of it being a bad idea, I do agree that it may be (is) unnecessary. The issue I have right now is time and knowledge. I'd like to spend some time with sketches and trying to constrain it via that route. Family re-unions, my own shop, my day job, all these things are bogging down at times.

[Anonymous]

Hooray! BTC all around. PM me both your addresses.

@LibertyMachine: Read you loud and clear on all points including sharing of models. Got my wish it was something simple and a bonus slice of humble pie. Completely spaced on selecting Model>Body in the Setup and was trying to compensate with touch surfaces. I may have gone on a bit of a rampage at the end there with some of my settings, thinking maybe if I went through every bizarre combination eventually something might work. Anyways, you are a gentlemen and I appreciate your time very much. 

@Steinwerks: I am getting proper results with the recent tips and now Machining Boundary>Selection>Sketch is working as intended. Agreed that splitting the body isn't necessary. However I am stoked to have gone through the process and learned two methods. 

Thanks! 

[dieselguy65]

john,with NYC-CNC on youtube just recently posted a video of doing this very thing. it looked like it worked great. i have not tried it yet, but i have a project coming up that will need 2 inches more travel in the Y axis than my machine has. i plan to implement his method for that

[Steinwerks]

Be aware of some of the comments regarding his use of sketch boundaries in that video, there are some obvious errors. I'm not in the business of making videos so I'm sure it's something that can be missed during a session that's crunched for time. Always simulate first!

[dieselguy65]

I'll double check, and then check again. Thanks for the heads up

[Anonymous]

Thanks @dieselguy65. Here is the link for anyone curious: Machining Large Parts in Fusion 360: Toolpath Containment!

In my case, I'm finding that while constraining the machining boundary to a sketch selection works great, it eliminates the option to machine via silhouette. I am getting results better suited to this projects needs with @Anonymous's Split Body method. 

@Steinwerks Do you still think this is a bad idea / poor practice? Is there an option with Sketches to achieve the Split Body results? I've experimented with negative offsets and that does solve the issue of leaving enough stock to lie flat when it's flipped (I'm milling both sides) but I feel it's unnecessary to remove so much extra material as the working time is already longer than I'd like. 

The project is a kiteboard, milled out of a block of extruded polystyrene (Styrofoam insulation).

The board is milled on both sides with as much stock remaining as possible. I offset the silhouette a bit so that the board is connected to the foam block by a thin line, easily cut out with a razor. This is done with a bit of math in the Heights settings. My test piece worked as intended but the toolpaths were awful and took forever. Also it was half size. And, for a bit of humor, I hand sanded it so diligently that when I was finished it was pretty much worked into a square block of foam again...

Thanks for your interest. Appreciate the discussion. 

[Steinwerks]

Well since I've come home feeling ill, I'll show you what I mean. I'm just joining the Split version together (both stock and board model). I'll upload the example when I'm done.

[Steinwerks]

Here's a real quick example. I joined your model pieces and the stock pieces and made them Components just to make it a little simpler. For some reason Fusion kept crashing on me when I tried to go back and edit your Setups so I made two new ones from scratch and stuck in some 2-minute toolpaths. Didn't do any stepover editing, depth adjustment, feeds and speeds, etc, but this should get you moving in the direction you wish to go. 

Remember that boundaries are just to keep the tool INSIDE of an area. They can be any shape, located anywhere. Geometry selection is all the same though, and the containment will keep your tools away from areas of the model even if you've selected them to be machined, because the boundary keeps the tool inside, period (see the Touch Surfaces in the toolpaths).

[Anonymous]

Looks great but it is the split body method, no? 

I should have specified that in this image, the model on the left is whole and uses sketches to constrain the toolpath, while the model on the right is split in two and uses silhouette:

Are we in agreement that leaving the model whole and using sketches does not allow the toolpath to follow the silhouette? In a perfect world the model is whole, and sketches are used to constrain the toolpath to half the model, but following the silhouette. 

Sorry if I am being dense I am trying to follow along best I can. Would like to send some BTC if you have an address (you too @LibertyMachine). It's been free money in crypto-land for a while now and I'm always trying to spread the word. 

Hope you feel better!
 

[Steinwerks]

Did you open the file? It's one model body and one stock body. No splits, just sketch boundaries.

[LibertyMachine]

Ahhhhhh.....

I see what you did now. Man that is simple. Makes complete sense now that I've seen it. It's the use of Touch that you are able to machine what you want, and the Boundary keeps it in that area. Very cool.

[Anonymous]

If you send a file please expect that I am going to open it and take notes. I have a lot to learn and really appreciate your time! Not sure what happened but this is what I see when I open your file: