Complex Object Cutting

[Anonymous]

Hey there!

So I have this pot mesh (stl) that was then converted to BREP. My end goal is to create a 3d printable Pot mold, so I need to split this beast into two halves.

However, I am trying to avoid flashing lines, so I've created a rather complex selection lines which I then created a selection set. I have done this on both sides of the pot.

My question is, how I can split this pot using those lines. I've attached a screen shot of one of the selections. I tried doing a Surface extrude on the line, no dice.

In a previous model I was actually able to create a Loft (using lines that were twisted) and it magically worked, but that was modeled from scratch, not imported from an STL..

Any ideas welcome! Thanks!

-Marc

[TheCADWhisperer]

What will it look like on the other side?

1. Project lines on the other side and Loft (I doubt you will get good results.

or

2. Project those lines to a Plane and then Split with the new 2D sketch and turn the other side to the wall so that nobody sees the back side.

[Anonymous]

Hey @TheCADWhisperer  thanks for the reply. I should have hollowed this out first, it would only need to cut to the hollowness 🙂 but presumably if I can figure out how to cut this side I can repeat on the other side.

I can't seem to loft multiple 3d sketch lines like this, unless there's a trick I'm missing? Your approach definitely works, and I used it on a twisted square test mold.  Attached working loft (twisted square) since it's also the same result I'm going for, but on a far more complex set of 3d lines on the pot. 

Regarding the 2d sketch, I did try that earlier, but due to the nature of the geometry it would never quite line up properly. Attached. Perhaps I need to project this on the inside, and cut outward? It may not be possible, just tinkering with the concept. I have a feeling any 2d projection approach would be imperfect?

Thanks again!

-Marc

[TheCADWhisperer]

Can you File>Export your *.f3d file to your local drive and then Attach it here to a Reply?

[etfrench]

Try splitting it in half first at 90 degrees to your desired split.  Split each half with your multi-segment line.  Combine the appropriate bodies together for the mold.

[Anonymous]

Hi @TheCADWhisperer thanks again for your reply! 

See attached. Both fusion file + diagram of what I'm attempting. The component is the actual mold, and for simplicity I just left it open on both ends. You will also see Selection Sets. One for each side of the Pot along the complex 3d lines.

Ultimately I would like to cut one side of the mold component with one of the Selection Sets, and then cut the other side using the other Selection Set. However, I am unable to do an Extrude on those lines (from one of the selection sets) using the Surface Extrude. This of course works fine on a 2d projection of those lines, which I left in here so you could see, but I don't think that approach will line up nicely.

I'm open to trying something else, but I think the real issue is I can't extrude the 3d geometry outward for cutting purposes!

Thanks again to any brave takers
-Marc

[Anonymous]

Thanks @etfrench, appreciate the response. I think I'll hit the same snag I just mentioned but it's very possible I am misinterpreting your suggestion!

[etfrench · Accepted solution]

By splitting it in half at 90 degrees to your desired split, the desired split will only cut one side of the model.  You'll need to create separate (desired) split paths for both halves. 

[Anonymous]

thanks @etfrench  I see what you mean, and that feels like a cleaner approach for sure. 

Attached..  Is that what you had in mind, lofting the line down the 3d edges? So since I had to extend the cutting tool (or fail), it obviously cuts both sides. Were you suggesting a clean flat cut across the whole piece first, then run each cut, essentially creating quarters. and combine them back after? Or is there an approach to cutting just one part of a body? I suspect Split Body fails because it's not technically splitting the entire body, yes?

Either way this method should work, much appreciated.

[etfrench]

This image is of one half after the double split and two quarters rejoined.

Obviously,  you'll want to pick a better path than I 😀

[etfrench]

p.s. There is no lofting required for the Split Body command.  Simply select the line as the Splitting Tool.

[Anonymous]

haha yeah just picking the path is half the battle.

My fault, I definitely didn't mean to say Loft. Sweep is what I used!! So you did split body and just chained those up the pot? Either way your breadcrumb got me there, and yup had to join up quarters all the same. Probably no way around that without cutting faces I think. ¯\_(ツ)_/¯

Thanks again @etfrench  & @TheCADWhisperer  Here's how she came out if you're curious. test print seems ok so far lol

Cheers

-Marc

[etfrench]

That looks good.  What material are you casting?

p.s. Sweep isn't needed for Split Body either, just the line.

[Anonymous]

Plaster/Cement etc. I just used the sweep to create the object that does the cutting, e.g 90 degree line is swept along the 3d line segments. Still not 100% sure which operation you used from your screen shot, but i will give that shot next time

[etfrench]

You don't have to create an object to do the cutting.  Just select the line as the Splitting Tool.