Sometimes when I have designed a sheet metal part I need to have features added or removed in the flat pattern to produce it but these features I do not want to affect the 3D model which could affect the assembly and drawing.
I want to give the Fusion 360 team Kudos for allowing me to prep the flat pattern, in the flat pattern environment, while not affecting the 3D model.
Example:
I have a bracket. It has countersunk holes, and a flange that the edge is not parallel with it's bend line. Because the "2D cutting" CAM in Fusion 360 is still limited, (no nesting, the post for some laser/waterjet/plasma are still lacking and some don't work, don't have all the functionality of the native CAM for a machine) I would be creating a .dxf file to send to my CAM software. Typically I would prep the .dxf file manually by deleting bend lines, remove the outer counter sunk diameter and just have the through hole, and add features such as a break off tab to have an edge of a flange parallel to its bend line (If you have a press brake with an 8 axis back gauge you would not have to add this). The main issue I have with just preping a .dxf file is that it is not linked to the 3D model. If changes are made to the 3D model I have to add the preps again.
What's neat about Fusion 360 I can prep my flat pattern, not affect the folded portion of the model, and create a.dxf file ready for cutting and still have it linked to the 3D model so if future changes occur the prep is updated.
Here is my 3D model:
Here is the initial flat pattern generated:
First step I created a sketch and use the extrude option and added the break off tab. If you properly dimension and constrain your sketch this will stay intact and in place if changes are made to the model. The main tab gives me a parallel edge to the bend line for my press brake. The tabs holding the main portion are small and the main potion can be easily removed by "wiggling" the tab up and down until it breaks off. To keep the profile smooth a simple grinding of the leftover micro tabs are done.
The next step is to remove the outer diameter of a counter sink hole. I only need the through hole for laser, waterjet, and or plasma cutting of the part. The counter sunk portion will be done on a drill press, hand drill, or mill after the part is cut. To do this I made a sketch and included the outer diameter and inner diameter of the holes and used the extrude command to remove the counter sink holes. If I ever move the holes or change the size of the counter sunk holes, the prep will stay in tact.
Before making the .dxf of the flat pattern I need to remove the bend lines. All I want in my .dxf are the inner and outer contour geometry. You can show and hide the bend lines but if you make a .dxf of the flat patterns the bend lines still show up in the .dxf even though you hid them. To accomplish what I need I had to go one step further. I first hid the bend lines then I created a sketch and included all the geometry (to include all the geometry simply make a box around the entire part and select the include 3D geometry command). I made a .dxf from the sketch.
Here is the .dxf that was created and sent to the CAM software:
Prepping the flat pattern in the flat pattern environment keeps everything linked to the 3D model and if changes are made to the model, and the preps are properly constrained, they will update as well. The other benefit is that these preps do not show up in the 3D model so you won't have these features affect the drawings of the views of the 3D model or affect relationships to other parts in assemblies.
Hope this is of benefit to the Fusion 360 community.
Thank you
PS @lars.christensen what are your thoughts???? 😁
Bryan Lagrange
