Find parting line for CNC on organic shape?

[nkloski]

Hi all!  Could someone help me with a workflow?  I have an organic shape of a vessel in the body (mostly flat but not completely planar).  I would like to subtract that from a block so I can CNC the shape, leaving the void in the acrylic.  I need to do two things:

-find the parting line on the organic shape

-build a surface from that parting line out to the edge of my block of material so that the two sides can sandwich together to re-create the shape as a void inside of the block

-also note that the CNC-ability of the file (draft angles/rounds on the flat edges, etc.) I can work out later, I am trying to even get to the point to deal with those problems 🙂

This is the vessel:

I have used the "silhouette split" command but the easy way of splitting the solid body fails because the parting line is not coplanar.  That command can create a split face, but that leaves me with going into the surface environment and deleting the top half of the vessel manually and then trying to loft various sections to the outer edge...which inevitably fails.

Can anyone help me figure out how to get a good parting line made?  The end goal is a circular disc, but I will take anything at this point, if it needs to be rectangular, that is fine as well 🙂

Just boolean-ing the object out of two halves does not work as that creates undercuts:

Here is the file (downloads enabled).  Thank you for any help!

https://a360.co/481xVQH

[evanp4509U4JZ]

Looking at your Pipe Path sketch your skills are way beyond mine but this may provide some conceptual assistance. I did an accessability analysis along the Y axis, created a plane along path on one leg of the pipe path sketch, drew a sketch on that plane through the pipe path and the approximate change over edge of the accessability analysis. In the surface environment I then swept the new sketch along the pipe path. I assume this can be done on all paths of the pipe path and the surfaces stitched together to create a parting line to split the block and combine/cut the vessel.

[nkloski]

Thank you!  I tried something similar early on but had problems stitching all of the paths together since some of the vessel branches off into "y" shapes.  I tried that on your model and got to a similar place, but thank you for the idea!

I got somewhat there by creating 3D splines that attempted to bisect the shape at the midpoint, but the resulting shape was hard to modify, but got almost there. 

I am just hoping for something easier (of course)!  

I am able to get a parting "line" by using the silhouette split, but then I am left with a line through the model.  I tried turning that into a surface, deleting one half of the model, then using a ruled surface to spread out that parting-line edge...but the ruled surface cannot extend on all sides and be parallel to an axis (like a guide surface on a sweep tries to do).

[TrippyLighting]

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@nkloski wrote:

I am just hoping for something easier (of course)!  

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In Fusion, after the silhouette spit, this is a fully manual, trial-&-error modeling approach that will take hours to complete!

[nkloski]

Yeah, that is what I am finding, thanks!    

I would assume there is software out there that would do this more readily but I am thinking Fusion is not it.  I played around with trying this in Inventor as well, but I don't know that software as well so I didn't make it that far down that path.

I may have to continue with the 3D sketch spline option and hope that I can place the control points in the best places right on the centerline, then extend them out as far as needed to overshoot the circular frame I need, then trim them away.

[nkloski · Accepted solution]

Just to circle back on this one. I figured it out once @TrippyLighting told me the unofficial answer:  that it would take a long time.  I prepared myself for the process and it actually only took me about 1 hour to do!  Here was my process:

-Take initial shape from the Form environment

-Use silhouette split (split face) to get centerline

-Create sketch, use "include 3D geometry" and click on all segments of the centerline to create sketch geometry of just the centerline (inventor does this automatically but in Fusion you have to do this step yourself)

-Since I want this to be circular, I created a new sketch with a box on the center plane that was larger than the circle I want to end up with.  I used the left and right lines of that box and created splines between the two box-edges.  I put in control points at proper places to allow tangency to flow through the points as close to the centerline as I could get, then used the "move" command to move them down/up in 3D space to align them to the centerline in that direction.  I used the "include 3D geometry" of the previous centerline to bring that into the new sketch for cleanliness of the workflow...and it is nice that the spline tool snaps to that included geometry if you rotate the viewport a tiny bit.  The resulting sketch looked like this :

-Then I created a surface loft between all the splines to make it look like this:

-Then it was simple to model the solid round body, boolean subtract the original shape from it, then use the lofted tool above to "split body" the round body into a top and bottom half, resulting in two halves, one of which looks like this:

-I then used the Accessibility analysis to see if my spline-ing was off any place and tweaked the splines a bit.  Now off to 3D print and test CNC'ing this.  Thanks, all!

[TrippyLighting]

That's a nice workflow!

Something to be aware of when developing these rather unique approaches is that one can also encounter unforeseen obstacles. It can sometimes take a number of workarounds to create a certain outcome that isn't achievable with a "standard" workflow. 

I've found that in most cases it's worth the effort and hassle, as one always learns something in the process!