Often times I run across a client that wants to convert their 2d sheet metal flat patterns into 3d models. These flat patterns are trusted and has been successfully manufactured year after year. Using Fusion 360 the designs could simply be recreate and flattened. But, the odds of getting the new Fusion 360 flat pattern to lay exactly on top of the trusted flat pattern would be a difficult and time consuming task.
The Fusion 360 Team has now added a "bend" command to sheet metal which allows us to successfully tackle the task described above and have faith that when we flatten the design it will lay exactly on top of our original flat pattern. So, moving forward the Fusion 360 file would become the official document of record. Where we can take full advantage of everything that 3d has to offer.
Before we jump into Fusion 360 lets first take a look at what the file looks like in AutoCAD. Make sure that the bend lines are not set to a continuous line type.
If the lines are set to a continuous line type then when we go to select the object in Fusion 360 incorrect areas will get selected. Also, please make sure that all of the actual edges of the sheet metal are on the same layer so, that when the profile is selected it recognizes all of the internal cutouts. If the internal cutouts are on layer "A" and the outside profile is on layer "B" the internal areas will not be detected. And would add more time in the converting the design to 3d because you would need to manually select the internal cut areas. Like the image below.
Now that we have some house cleaning out of the way let's get started. How do we get the 2d into Fusion 360?
If you are using Fusion Team which I hope you are. Then I would copy and paste the 2d files directly into your drive and the files will just show up in your Data Panel.
I will assume for now that you are not using Fusion Team and just want to get the file into Fusion and start working. Create a new sketch and go to Insert DXF. Select your DXF and choose what layers to bring in and make sure that the Insert Mode is set to "One Sketch per Layer" then hit OK.
Select the Flange command, choose the sketch and select the appropriate sheet metal rule and hit OK. When using the Bend command it is crucial that you work from the outside of the part to the center of the part. If you think about it, it just makes sense. If I started in the center of the part and bent the part up 90 degrees the sketch with the bend line is still laying flat. So, I wouldn’t be able to continue bending the part because the part is now up in the air and the bend lines are still on the original plane. There will be times, that no matter how careful you are you may need to create a new sketch on the part and draw in a new bend line. I will show you an example of that here soon.
Select the Bend command and choose the area of the sheet metal that you do not want to bent and then select the bend line.
Continue working from the outside to the center of the part.
Here is an example of when you still may need to create a new sketch and a new bend line. In the below image Fusion 360 will not allow me to bend the wings up 90 degrees because the model will self-intersect.
So, the body of the plane needs to be bent first.
The only problem is the part bends and the sketch that we inserted stays on the sketch plane. So to finish the wing a new sketch needs to be created on the part with a new bend line drawn in.
So, experiment with this workflow and I will get back to sweeping some mines.
Hope this helps you in some way!
P.S
Depending on how you bring in the 2d data the history may be turned off in your design and you may not see any sheet metal functionality. Simply right click on your timeline and select "Capture Design History".
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