Problems making a cookie cutter

[DaveGadgeteer]

I want to take the cut lines of a jigsaw puzzle and use them to split the bodies I've designed. 

I.e., I want to turn a 3D object into a 3D jigsaw puzzle.

To do this, I got jigsaw outlines from the web, and extruded them in Z in the Patch environment.

That gives me the form I want to use as the cutter, but I can't use it--it's a bunch of surfaces, not one thing, and I can't find any way to join them so that I can use them as a splitting tool

In principle I could use the Thicken tool to turn this into a single solid, but the thicken operation takes forever and seems to lock up Fusion360 so I eventually have to kill it.

Thickening would have also had the desirable property that there'd be a kerf between the 3D parts, which I'll be 3D printing.

Anybody have any suggestions that I might try?

[etfrench]

It would be easier to help if you attached your file (File|Export|Archive files *.f3d).

[mavigogun]

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@DaveGadgeteer wrote:

I want to take the cut lines of a jigsaw puzzle and use them to split the bodies I've designed. 

I.e., I want to turn a 3D object into a 3D jigsaw puzzle.

To do this, I got jigsaw outlines from the web, and-

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-why not just use those outlines to split your target body?

[chrisplyler]

I think the complaint is that he has several lines he wants to use as splitting tools, and he doesn't want to have to go through the splitting process a zillion times. He would like to be able to select ALL the lines at once and split a single body into a hundred (or whatever) bodies all with one operation.

[etfrench]

The answer would be obvious if we had the file or even the jigsaw pattern.

[DaveGadgeteer]

I don't understand how one can split a solid using a line?

Anyway, here is my design, attached. I thought this would be a simple small starter test...

[etfrench]

Here's one way to do it:

Do the vertical rows using the sketch in the copied component. 

[DaveGadgeteer]

I don't understand why the puzzle pieces aren't consistently treated like profiles.

Most of the area is that way, but two whole edge rows/columns are treated like one single profile.

If I could get each piece to be a profile, I could extrude each as a solid and use Combine to get separate 3D pieces.

I assume the problem is related to not having proper constraints at the piece intersections, but I can't make the constraints display at all, much less edit them.

I've turned on Display Constraints in the sketch, but no effect. What else may be suppressing their display?

[chrisplyler]

One can split a Body using a sketch line as the splitting tool. The line will project out from the sketch plane it is on, and wherever that projection slices through the body is where the body will split.

[DaveGadgeteer]

Thanks! The "Thicken" approach is exactly what I have been trying to do.

But I think the problem comes because I need more complicated curves, to get some interlocking.

When I do the Thicken, it isn't just slow, it brings Fusion to a complete unresponsive stop. After some hours, I have to Force Quit.

How could I do this in smaller sections so it can finish, then combine the sections to make the cutting tool I need? Tedious.

Hmm.

[DaveGadgeteer]

Wow, I had no idea you could use lines like that.

Maybe I can build on that approach. I could thin each solid slightly to get some kerf if necessary. Maybe I could do that in the 3D printing, if I print each block separately.

[chrisplyler]

I don't know how many elements you're working with when you try to thicken.

You could just thicken a few at a time, and then perform a combine operation back in the Model environment to make all of them into a single body.

Or it might be less time consuming to just do a Sketch>Offset of each line by your desired gap width, manually close each pair of lines into a profile by drawing little lines at the ends, and trimming all the intersections so that you get one continuous profile of the whole cutter.

[etfrench]

In the video, I had to extend the puzzle piece lines on the right because the end points were not coincident with the vertical line.  This is also why some of the pieces were treated as one piece and others were not. 

You can use an offset of the splitting lines to create a small gap between the pieces.  Use Extrude|Cut when doing it this way.

[DaveGadgeteer]

I'm trying separating the horizontal and vertical cuts into separate SVG files.

I did that in Illustrator, but now Fusion crashes everytime I import such a file.

I added a bit of thickness to the lines, maybe that's the problem--it didn't help anyway, because the lines look thin as usual just before Fusion crashes.

I like the square pipe solution, if I can ever get there.

Is there a way to trace curves in a Fusion sketch that keeps them separate? If there were, I could trace the old version into separate H and V subsets. But just redrawing by hand is difficult.

[chrisplyler]

Trace? Not exactly, but something that will produce a similar result.

Start a new sketch, and then use the Sketch>Project tool and click on whatever you want. The stuff you click on will be "traced" (projected) into the new sketch.

[DaveGadgeteer · Accepted solution]

OK, I finally got the desired result. 95% of the time went into restarting Fusion because it almost always crashes when inserting an svg file into a sketch.

Here's what worked:  Generate puzzle cut pattern using online tool http://www.wolfiesden.com/Laser/PuzzleCreator.asp

Edit that pattern in Inkscape .91

First delete all the vertical cuts and save the horizontals, then reload and delete all the horizontals saving the verticals.

Use Inkscape tools to extend the cuts past the edge of the desired area and tie them together with curves (not necessary, but maybe handy--fewer tiny profiles to select). Draw with stroke set to the kerf width desired. I used 1 point, =1/72 inch. Take great care to make sure the lines don't have tiny disconnects in them. I found half a dozen 0.026mm gaps, which caused great trouble. It takes a lot of zooming in Inkscape to be able to find and see such tiny gaps. There must be a tool that closes tiny gaps, but I'm not an Inkscape user normally.

I chose rounded end caps for the lines.

Then convert the stroke to paths, which gives a closed profile that I can extrude later, and save the file(s).

In Fusion, create an offset plane to sketch on, new sketch, and insert the horizontal cuts. Save. (It may take 10 tries to insert an svg without a crash. Starting from a brand new sketch may help.) Select the tiny thin long profile and extrude it some useful distance as a new body. Hide the sketch and extrusion. Make another new sketch (I put it on a different but parallel plane to try to keep the complexity of one from somehow affecting the next.) Import the svg for the vertical cuts. Show the previous extrusion. Extrude the vertical cutter profile similarly, using join option. Now we have a cutter.

Then make visible the items to be cut--it would be better to combine them first, as you can only cut one body at a time. (I tried splitting body, but that always failed to compute, while combine/cut worked.) Use combine, with the cutter tool and cut.

Done.

The hard part was finding a pathway that Fusion could handle, and most of the time was spent waiting for Fusion to reload after the svg-insert crashes. Some of the early crashes were doubtless caused by the complexity due to tiny gaps, but Fusion still crashes very reliably even after the curves are smooth and the gaps are gone. You just have to save often and keep trying. Usually the crash happens during the move-into-position phase of the insert svg, but sometimes it doesn't get that far. Painful.

Now I want to change the puzzle details and sizes etc etc, but it's so tedious I'm kind of inclined to live with what I got.

It's a real pity one can't edit such curves in the sketch. Constraints refuse to display, etc. Necessary to use some tool like Inkscape.