Flatten rectangular box onto horizontal body

[chapmarm]

Imagine you have a rectangular box, without the top. You have two sides, a front, back, and bottom. My goal is to take this box and flatten it onto a horizontal surface, giving space between each body of the rectangular box. The purpose of all of this is so a CNC plasma can cut all the parts, which I can then weld together.

As a first pass, I went the parametric route, and for each side of the rectangle, I would draw a separate sketch onto the horizontal surface using the appropriate variables to scale. This worked fine using the simple rectangle, but it became a maintenance burden as I added more complex parts. Another downside is that for each body, I must create a separate sketch, which increases the margin for error.

I am very new to this, but I believe what I want to do is to project the bodies mentioned above onto a horizontal surface. In the case of the rectangle example, the sides are vertical, yet the surface I am project to is horizontal on a different axis. I tried "project to surface" but no luck. Any ideas?

Thanks!

[jasonhomrighaus]

So once you have everything the way you want it, there is a pretty straight forward way you can proceed.

First, determine how you want the panels to face up to each other then use a split body command and choose the inner face of the panel you want to separate as the cut plane.  This will cleave off the panel from the main body.  Repeat that process for each panel you want to make till you have them all where you want them and the right shape.  if you want to have tabs or different overlaps you use a combination of splits and combines to build up the flat pieces you want.

once you have them fully formed then use the create sketch command on the face of each of the panels.  Then use the Project command to project the body profile onto this new sketch.

then you can right click on that sketch in the browser and select the Make DXF command.  This will output a DXF version of the sketch that you can import directly into your cutting system.

Repeat for each of the panels.

The nice part about doing it like this in parametric model is that if you later tweak the panel sizes the sketch will automatically update without having to jump back to an earlier sketch.

[lichtzeichenanlage]

Two examples how to do it. Both are based on components. So the first step is equal to both variations

Example 1:

• Create all sides as components
• Create plate
• Run Nester to lay things out (semi automatic)

Example 2:

• Create all sides as components
• Create new document for production
• Insert all components via Insert -> Insert Derived.  Be sure not to select the bodies but the components.
• Lay all things out like you want. Might be possible to do this with Nester, too. Not sure because this tool was created before derived components exists. 

This video is not exactly what you're doing, but shows the idea:

[davebYYPCU · Accepted solution]

@jasonhomrighaus that was my old workflow, 

There is a lot simpler method now, 

an addin called Dxfer, on GitHub. (From the author of the Nester Addin)

creates a dxf File by clicking on any / each face of body.  

Many faces - many bodies, one dxf File.  

Dream come true for laser / plasma cutters that don’t use Fusion CAM.

Thanks again @prainsberry 

[prainsberry · Accepted solution]

Thank you! Glad it is helping out!