Splitting objects

[Anonymous]

How can I split a simple box (when sculpting) down the middle so it becomes two seperate parts? Say I have a box that is 10mm wide and I want to split it at around 3mm , so I will have one half 3mm wide and the other half 7mm etc. Also I would like them to flush / fit together

How can I do this in Fusion360?

[jeff_strater · Accepted solution]

This is pretty easy.  The main commands to use are Split Body and Create Components From Bodies.

Start with your block (my examples are not dimensionally accurate to yours), then use an Offset Workplane to create a plane at the distance you want:

Then, use Split Body to split your block into two, selecting the block as the body to split and the plane as a splitting tool:

Now, you have two bodies in the browser.  Assuming that you want components instead of bodies, use the Create Components From Bodies command by right-clicking on the root of the design:

And that's it!  Now you have two components from your one block:

Hope this helps,

Jeff Strater (Fusion development)

[Anonymous]

Where is that offset workplane tool?

[James.Youmatz]

Hi @Anonymous,

If you go to the construction menu, you should see Offset Plane as an option. 

Thanks,

[HughesTooling]

Another simple option is to use Split Body with just a line or curve.

Mark

[Anonymous]

Ah, thank you. This helps a lot with a project of mine!

[chris.e.robison]

Unfortunately, splitting a body with a sketch geometry doesn't work reliably, beyond the simplest cases. If the curve comprises more than one segment, you may or may not be successful, and in my limited experiments so far the limit seems arbitrary and inconsistent between attempts. At some point it will just stop accepting more segments in your selection for no apparent reason. So this puzzle-piece split for example, isn't allowing me to select more than seven segments along the curve:

[Anonymous]

I am having the same issue. Is there an answer to how that puzzle was split? 

I am having trouble splitting these 2 curved surfaces apart. I have been using project 3d geometry and split body, but alas to no use. Any and all advice would be great? 

[HughesTooling]

---

@chris.e.robison wrote:

Unfortunately, splitting a body with a sketch geometry doesn't work reliably, beyond the simplest cases. If the curve comprises more than one segment, you may or may not be successful, and in my limited experiments so far the limit seems arbitrary and inconsistent between attempts. At some point it will just stop accepting more segments in your selection for no apparent reason. So this puzzle-piece split for example, isn't allowing me to select more than seven segments along the curve:

---

The problem above is down to a bad unjoined sketch, note all the points, these indicate open chains. If coincident constraints are added it will work fine.

In the image below note there are no points at the ends of the lines\arcs and I have no trouble selecting the continuous chain.

Mark

[HughesTooling]

@Anonymous A 3d part is going to be a bit more difficult as the split tools from curves will not work. You might be able to make a curved surface to use as a splitting tool but it might not work if there are place where the inter section is almost tangent.

You might find it easier to make a copy of the body in a new component then switch to the patch workspace and delete surfaces you don't want then patch any opening left. I'd suggest making the copy using Boundary Fill and set the operation to New Component. 

If you can share the part I'll take a look, export as an f3d and attach.

Thanks Mark

[Anonymous]

Here is the attachment. Let me know if you have received it. 

[HughesTooling]

@Anonymous Got your file OK. Next question is what are you trying to achieve? What's the reason for splitting do you just want 2 parts or is there more to it.

Mark

[Anonymous]

Yes. I want just two parts cut at the  vertical T-pipe. All of the other Y-part fillet stuff and pipe should be left as a separate entity or body.

[HughesTooling]

Here what I came up with, I've enabled history so you can step through the timeline to see what I've done. Basics are moved part to the origin to make sketches easier, remove fillets or split will probably fail then created a revolve surface as a splitting tool.

Mark

[Anonymous]

Just confirming. so you deleted the fillets and used revolve. This created a surface body that could be used to split the y piece body into 2 parts?

[HughesTooling]

I've attached the file to my previous post, "temp.f3d". Just save to your computer and use New Design from file to import.

Mark

Edit. The revolve was created in the patch workspace so is an open body. If you enable it's visibility while stepping along the timeline it should all make sense.

[Anonymous]

Thank you very much Mark! Great Help!