How to split a swept body *without* extending, to layout for manufacture

[ericjforman]

Hello, I've been struggling with a split body issue. (Partly due to transitioning from Rhino, where this is simple.)

I have a swept closed polyline that I want to split into segments at each "joint." The eventual goal is to lay all the segments parallel for construction drawings and CAM in Manufacture space.

desired cut planes

I was hoping I could use a construction plane for this with some option to not extend past the visualized limits of the plane, but Fusion doesn't have that option. 

I created a sketch on that "split plane" but Fusion does not allow selecting the profile, only the lines, which cuts in the wrong way. 

cannot select sketch profile, only lines

I created a surface from those lines and used that to split, but I get the error "no intersection between target and split tool."

This is confusing because the same split works fine if the split tool is extended. But of course I don't want it extended. 

I also tried lofting a split tool from the existing edges to make sure (and then scaling it to be sure it is bigger than needed), but I get the same error.

One possibly relevant curiosity: I am unable to create construction planes from the edges of the swept geometry (error "input lines must intersect or be parallel"), even though the sweep by definition should create aligned edges. The exact same form swept in Rhino and imported can be used to create construction planes on the same edges. (This body is in the file named "reference polysurface from Rhino.") I would also like to figure this out, and feel like it's related somehow...

 

What is a better way to do this? 

File: https://a360.co/3etOsFK

Thank you in advance.

[Bunga777]

How about Unstich the body, cover it with Patch where needed, and re-stich it again?

Unstich.

Patch the end face as a lid.

If you re-stich it, it becomes a Solid Body.

The video is posted here.

https://knowledge.autodesk.com/community/screencast/17c22fd5-e899-45be-b28f-fbe48e45364b

Data is also attached for your reference.

[ericjforman]

Thank you Bunga, that is certainly a workaround. But the model is parametric (for example you can change the polyline or sweep profile angle), so it needs to auto-update easily...

[Bunga777]

I think it is possible to change the angle and length of the frame as long as the changes do not disrupt the operation up to the history you have provided.

However, there seems to be a problem that the joints become twisted when the profile is changed, which may be a problem to deal with.

[Leo_Dyn]

Instead of using a plane as your cutting tool, can you instead use a sketch profile? So, make your plane as normal, then do a sketch on that plane, project the body where you want to make your split, or just sketch a rectangle or something in that area (or do both). Then try to use that profile as your splitting tool?

[Bunga777]

Change the sweep so that there is a gap here.

This would open a gap here.

After that, create a surface for cutting and use Split Body.

The first gap opened can be connected later.

Oh,, I forgot to disconnect one part, but I think I can proceed now.

[laughingcreek]

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@Leo_Dyn wrote:

Instead of using a plane as your cutting tool, can you instead use a sketch profile? So, make your plane as normal, then do a sketch on that plane, project the body where you want to make your split, or just sketch a rectangle or something in that area (or do both). Then try to use that profile as your splitting tool?

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I think the OP shows why that doesn't work in the second picture.

[laughingcreek]

The reason why split body is failing with both the patch and the lofted surface as tools (without extending) is that your not creating 2 separate bodies with the split.  This situation confuses the algorithm. 

one way to work around this  would be to give a slight thickness to the splitting surface with thicken and subtract it out with the combine tool.

a second way would be to simply split the thing in two with a plane, do your splits (which will now work because each split will be producing 2 bodies) and recombine.

a third way would be to join 2 split surface with a loft, stitch them together tso the form a single body, and use that for your first split.  as before, subsequent splits will work as expected b/c you'll be forming 2 bodies with each split. 

I've attached your model demonstrating this third option using the splitting surfaces you already made for the tools.  examine the last 3 features in the time line.

p.s. - I also broke the link to the derived feature which allows exporting as a .f3d file instead of .f3z.  most everybody here prefers .f3d b/c .f3z can be a pita on this end.  I also prefer attaching a file instead of using a link.  an up loaded file doesn't get changed like a linked file might.  it's possible to continue work on a linked file and not have it reflect the question anymore when someone opens it, which can be confusing to anyone trying to help. 

[Bunga777]

@ericjforman @laughingcreek 

We have created a simple model for easy understanding. This is easier to understand.

There are several ways to cut using sketches, but as you can see, this method is not successful.

Unfortunately, this method also fails.

This way we can succeed.。

From the above, I assume that when splitting internally, if each Splitting tool cannot make one Body separate from the other, an error will occur. So the third splitting is successful because it is completed in one time.

So, if you leave a small gap as shown here and make each tool a separate Body when you evaluate it, it will succeed.

[TrippyLighting]

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@laughingcreek wrote:

...  This situation confuses the algorithm...

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Correct. I would consider this a conceptual flaw in implementing a tool.

IMHO that is worse than a bug!

[Leo_Dyn]

@laughingcreekOh, yep, you are totally right! And with some of these other posts, I see why as well. Makes sense that not splitting it into multiple bodies is the reason. Using that method only does a cut of the body without actually splitting into multiple.

Just did a bit of testing and I, like the OP, can't even select a profile to use. The tooltip pretty clearly states that selecting a profile should be allowed. I tried this with both a profile that was only projected geometry as well as regular lines, drawn at both the exact sizes of the projection as well as just larger to make sure it encompasses the area of the body at that point. No luck, seems like a bug, or a tooltip text error. (which I guess is still a bug??)

[laughingcreek]

I agree that the use of the term "profile" in the tool tip is incorrect.  it should say something like "sketch entity" or "sketch curve" in order to be consistent with the nomenclature used in other areas of the program.

[ericjforman]

@laughingcreek and @Bunga777 thank you for the solutions working around the issue. I think it is slightly faster to use the former's method since I can loft the cut shapes without creating construction planes or sketches, or requiring a gap in the sweep. Although it does require scaling the lofts, adding the connecting pieces, and stitching into three tools. Toss up. 

Regardless it is all pretty inefficient, and I agree with @TrippyLighting that it is a conceptual flaw.  

IMO, split should work as a cut regardless of how many bodies it results in. And if it did, maybe it should even be called a name more like "cut"? But that's another can of worms.

@laughingcreek agreed, it should say "sketch curve" - but what it should really do is allow profiles!

And thank you for the suggestion re breaking link and f3d vs f3z, I didn't know that.

With this solution, the splits continue to work even after changing parameters, which is great. 

However, I am unable to edit the sweep path: even nudging a point over makes the sweep (and everything else) break. I tried re-selecting profile and path in the feature, and even creating a new feature, because sometimes Fusion is wonky like that, but same error. Why shouldn't you be able to edit a sweep path? 

This is unrelated to the splitting, but critical for the design process of the file, so if anyone can figure out why, that would be awesome.

I should probably make a new post, but... Here's a simplified file to demonstrate:

[Bunga777]

As I mentioned in my previous post, if you change the path, you cannot set the Distance to 1.0.

If you set it to something other than 1.0, the Sweep will succeed. This will create a shape with gaps.

If you zoom in on the joints, you can see that there is a slight misalignment as shown.

Depending on the change of the path, this misalignment can become larger.

What I am wondering here is how did the first pass determine this shape? I mean, how did you determine this shape for the first path?

I find it very difficult to randomly generate a path shape that fits and joins this area tightly.

Can you tell us how you wrote the first pass?

[ericjforman]

Ah yes of course, that was stupid of me. I had just assumed the sweep would complete even with a misalignment. Thank you.

Getting the "twist" of the pieces to line up was actually quite difficult. Especially as the profile seems symmetric but side A has to meet up with itself at the end. I had to make an elaborate Grasshopper script to perform distortions on a given point until a near-zero misalignment results.  

Interestingly Fusion does complete the sweep with a teeny tiny misalignment (e.g. in this case 5.4e-7). But that could just be a rounding error in Rhino.

[ericjforman]

Here is a screencap in action if anyone is interested: 

Now, I need to get to the actual end result of my original post! --- finding an efficient way in Fusion to lay the split sections out for Manufacture. Right now I'm using Arrange which is okay (although annoyingly Fusion can't make drawings from manufacture so you have to either do it Design or export a copy and import it as a new design).

The end goal is auto-alignment in the drawing of the end faces of each section to a virtual saw blade for cutting.

For example:

[Bunga777]

@ericjforman 

Thanks, this kind of thing can be done with Rhinoceros, it's great.