Sheet Metal Workflow

[colinNJB25]

Greetings, I picked up a job that purchased a Fusion 360 license. I more usually post under my hobby account. I am drawing some sheetmetal parts and mistakenly drew a box and a lid onto one document. That put limitations into getting drawings produced so I am needing to move the lid to a new document but cut and paste is not supported in sheetmetal. Is there a way to move the body to a new document or do I just copy the sketch and start over? Also, I would like to link the screw holes that attach the lid to the body to update parametrically, how do I link the two documents? 

[HughesTooling]

What limitations are there creating the drawings? You should be able to add sheets of the individual components.

Mark

[HughesTooling]

Just in case you're unsure how to add a second unfolded component.

From the model space right click the component and select Create Drawing,

For representation select Flat Pattern.

Drawing, select your existing drawing.

Sheet, either select New or one of the existing sheets.

Mark

[colinNJB25]

When I try to create a component from a sheetmetal body I get an error: This operation is not supported for sheet metal bodies. If I make a flat pattern of one body I have to delete it before I can make a flat pattern of the other body. I am not sure how you were able to work with more than one sheetmetal component in a single design. 😕

[HughesTooling]

The first thing you should have done was create a sheet metal component you shouldn't have created the parts in the main component. I think I can convert what you have, I get back with it later.

Mark

[HughesTooling · Accepted solution]

I saved your design to my hub then inserted it into a new design and broke the link giving me your design as a component.

The way you were constructing your box and lid side by side is not the best\easiest way so I deleted your lid. I recreated it in a new component in place on top of the box. I've created a sketch that is constrained to the top of the box with 1mm clearance, edit the sketch in the second component if you want to change that. The dimensions are linked so you only need change one.

As the parts are in place you can create the holes and project between components. Probably best to roll the timeline back before the second component add the holes then roll to the end of the timeline and project into a sketch in the second component.

Model is attached.

Mark

[colinNJB25]

Thank you @HughesTooling! That is exactly what I needed to learn. I have a bunch of these to draw in the coming weeks. I didn't want to not start off without understanding the workflow.

[50079515]

Not sure if anyone is still following such problem. But I found an easier way to extract sheet metal into components. 

1. use "Boundary Fill" to convert sheet metal into new component as body.

2. Use "Sheet Metal>create>convert to sheet metal" to convert back to sheet metal under new component.

I learned this from this smart guy! see YOUTUBE link below: 

https://www.youtube.com/watch?v=FqVVNVN8gV4&ab_channel=JohnHackney