Workflow for Structural Steel Shapes & Libraries

[Garret_H]

I think I've found a good hack for building steel structures in Fusion 360 and the lack of a steel shape library.

The first, unfortunate step is to build your own library by creating new files in a separate folder. The parametric features of sketches make this less painful for doing shapes like rectangular tubes, draw one and just change a few critical dimensions.

Another important step is to use some construction lines to capture the intersection points of face planes intersections (e.g theoretical corners) so you don't have to snap to radiuses or exclusively centerpoints.  Turn the sketch back on after you're done.

Now extrude that profile some short arbitrary length (say 1"). Save the file, then do a save as for each different profile, changing dimensions accordingly.  Don't forget to write the material description in the properties box, this will make for nice clean Bill of Materials later.

After creating your library this is the workflow to insert steel shapes:

1. Drag and drop selected shape into to your drawing. (Note: I really like to snap to sketch geometry points of my frames, so I can modify dimensions and positions later).
2. Break the link, rename the component.
3. Use the sketch features as snap points when moving your object to the correct point in your drawing.
4. Now just use extrude to extend your components profile to the correct length. This can be either by activating your steel component and editing the extrusion length, or by simply extruding the end face within your top level component.
5. When you are all done lock your components into a rigid group if applicable.

Now if you have multiple occurrences of that same length of steel you just created, you can simply copy the component around. This is great for your BOM showing multiple quantities of similar lengths, see the highlight example BOM below.

I didn't add a field for cut length, which would be a manual process unfortunately.

At first attempt this seems to work well for me, with the profile sketch as part of the individual component and not any of your top level components makes for a very nice clean workflow.

Here is an assembly I am in the process of. I used sketches to define my geometry based on measurements of an as-built frame, while I drew rectangles of the width's single line representations could have also been used.

If anyone has any feedback or ideas to improve on this please let me know!

[HughesTooling]

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@Garret_H wrote:

1. Drag and drop selected shape into to your drawing. (Note: I really like to snap to sketch geometry points of my frames, so I can modify dimensions and positions later).
2. Break the link, rename the component.
3. Use the sketch features as snap points when moving your object to the correct point in your drawing.

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Are you moving the sketch within the component or are you moving the component? If you're moving the component are you using a joint or the move command? Can't tell from your timeline but you don't want to end up with lots of save positions as they hit performans, best practice would be to position the imported components with rigid joints.

Mark

[Garret_H]

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@HughesTooling wrote:

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Are you moving the sketch within the component or are you moving the component? If you're moving the component are you using a joint or the move command? Can't tell from your timeline but you don't want to end up with lots of save positions as they hit performans, best practice would be to position the imported components with rigid joints.

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Good point.

When I initially insert my component (the steel shape) I use the move features to place it, using the component's profile sketch to position it where I want. I think this avoids an additional move command initially.

Additional copies of identical length/profiles are done with the move/copy command.

Using joints if I move that component later would be wise. I know I can use joints from sketch points, so that should let me use sketches to define material lengths and positions when needed.

[HughesTooling]

OK. Just for better performance with bigger assemblies it would be a good idea to ground the component if it's static or use a rigid joint.

Mark

[Garret_H]

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@HughesTooling wrote:

OK. Just for better performance with bigger assemblies it would be a good idea to ground the component if it's static or use a rigid joint.

Mark

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Thanks, I am finding that instead of placing everything and performing a rigid group at the end I am a lot better off applying joints to each member as I drop it in to my sketch. If I don't do this and then try to change the sketch later I lose positions which may also affect lengths etc. 

[HughesTooling]

I don't insert designs that often but I find even in an assembly file where all components are created in that design, after creating a component the first thing I do is either ground or use a joint to its origin to position it and lock it in place. The more you constrain everything the better performance you'll get. With sketches always try and fully constrain so the red pin is on the sketch in the browser as well.

Mark

[HughesTooling]

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@Garret_H wrote:

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@HughesTooling wrote:

OK. Just for better performance with bigger assemblies it would be a good idea to ground the component if it's static or use a rigid joint.

Mark

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Thanks, I am finding that instead of placing everything and performing a rigid group at the end I am a lot better off applying joints to each member as I drop it in to my sketch. If I don't do this and then try to change the sketch later I lose positions which may also affect lengths etc. 

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Not sure if this is what you're using but this is what I'd do, insert part, break link and roll timeline to start of new component and use a rigid joint to position. Screencast below to make it a bit more clear.

Mark

[Garret_H]

I haven't tried to roll the time line back after breaking the link, but yes using rigid joints now. 

My next task is to start creating a library of "box frames" that use just a couple sketches to drive the geometry. This is for four sided angle or tube frames where all four corners are mitred to each other. A time consuming activity otherwise.

[Garret_H]

@HughesTooling this video on capture position has a handy trick. Instead of rolling around the timeline just delete a capture position that occurs before placing your joint. 

Link to the portion of the video its shown.

https://youtu.be/SMrNkF5UcPw?t=2566

[HughesTooling]

Yes that's about the only time a capture position's useful. I see a lot of designs on the forum where someone drags a component near to where they want it or out into space to make adding the joint easier but they leave the capture position, in a big design these will waste a lot of resources and make Fusion very laggy.

Mark