Fusion
Hi, does anyone know how to cut a sketch where it intersects at a plane, or how to sketch so that a line drawn on one plane has to end on another intersecting plane? In the picture below, I have marked the shape I am trying to cut in light blue, and on the lower two views, I have marked the intersecting plane that I want the blue shape to be cut by. I also have the link to the file pasted below so that you can download the file if you want to experiment.
Hi, I'm not exactly sure what you are trying to achieve here, can you possibly add some more details? The model that you shared does not contain this blue shape, so I had to guess a bit what it was supposed to look like.
Here's what I tried to do to reproduce it:
Then, I projected the other plane (plane12) into this sketch (actually, this didn't work correctly, which I think is a bug, and I'm investigating that, so as a workaround, created a sketch on that plane, and drew a line and projected that line into this new sketch). Then, I trimmed my parallelogram against that projected line. This is what I got, but I'm not sure that this is what you wanted:
ANyway, any clarity that you can add will help. You can also turn on 3D sketching, if what you are trying to do is make a 3D sketch here.
Jeff Strater (Fusion development)
Jeff Strater
Engineering Director
Thanks, I am trying to make something similar to following bottle without the cap. if you check the most current version here, it shows a semi decent but not connected and well done rendition of what I did on one side, however, I want it to all be connected and done properly. Ill try to make everything I post here a seperate one so that updates wont change the one I posted.
OK, I see now. Cool design.
There are probably many ways to address this design. If I have time, I will try to post some workflows that I might consider. One of them might be to use 3D sketching instead of just 2D sketching. Another might be to start with a solid and remove material to get this shape.
But, your approach is just as valid, so I'll start with it (although I took a shortcut to get there, which is yet another approach to start from the beginning). Here's what I did:
First, there is one triangle missing from sketch 14, so I edited it, and added that triangle. I also added another line at the midpoint, which will be used later:
Then, in the Patch workspace, the Boundary Patch command can be used to make surface bodies from the sketch regions:
you will notice that I did not do all the regions - that's my shortcut - I'm only going to do one side of this...
next,add a workplane through that sketch midpoint line:
then, use the Stitch command to stitch everything together:
This is the result:
Next, I want only half the model, so I'll use Split Body to split using the workplane:
Here is the result:
Finally, use Mirror to get the left half of the model:
And one final stitch to make it a solid. This is the result:
I have also attached the completed version here, if you are interested
Hope you find this helpful
Jeff
Jeff Strater
Engineering Director
Here is another way to model this shape as a solid:
Start with this sketch. The angled line will be used later:
Then extrude it to half the ultimate desired width:
Next, add an angled workplane through that angled line:
the angle determines the angle of the side face.
Next, use Split Body to split by this plane:
Then, use Mirror to mirror this front half:
and mirror again, side-to-side:
giving the final result:
I will try to answer your unfolding question. This may require a slightly different approach...
Jeff
Jeff Strater
Engineering Director
Accepted solution
OK, on to your "paper box unfolding" question. In general, Fusion does not yet have any sort of unfolding capability.
However... I was able to fake it, sort of...
This will not work in all cases, and does not account for any deformation caused by folding, etc.
So, I started with the same basic model as yours, but I skipped the final stitch, so each face of the design was a separate body:
Then, I used Create Components From Bodies:
to put each face into a separate component.
Next is the trick. Use "as built" Revolute joints to define the folding lines:
And continue to define revolute joints where you would unfold this:
Then, once you have all the joints defined, it's a case of using Drive Joint to fake out the "flatten" process:
This was a bit tricky at times, it required doing some measuring of angles, and some angle complement calculations. but, I was able to get to:
Model is attached...
That was kind of a fun way to spend a bit of time. 
Jeff
Jeff Strater
Engineering Director
That's an incredable job of unfolding. I couldn't resist trying a T-Spline approach to developing the bottle shape. One advantage with the T-Spline approach would be playing with the shape and developing alternatives. Here's a screencast of how I approached it. Thanks for the inspiration.
