Sketches, Bodies, Components, Oh My!

[george]

I'm struggling to wrap my head around the relationship between all of these when working with a timeline. I'm putting together a model of a doll house and I started by making individual sketches for each of the partitions. My general workflow was to create the sketch, add appropriate dimensions, push/pull to create a body, and then create a component from that body.

As I progress in the model I find that I might want to change the size of something or move it. If I select a sketch to edit any of the changes in the time line AFTER the sketch was first created are greyed out and I assume disabled.

What I'd like to do is to create a piece of the model and then be able to move or change the dimension easily later on if I want.

Please help me train my brain to think like F360 does!

Thanks,

George

[jeff_strater]

Thanks for posting this question.  I believe that you can do exactly what it sounds like you want to do.

Your design methodology sounds good.  Sketches -> Bodies -> Components is a perfectly valid workflow.

Think of the timeline as a form of time travel.  When you edit a sketch that was created earlier in time, Fusion will take you to back to that time in history.  That's why later features in the timeline are grayed out (they are in the future).  When you are finished, just click the "Stop Sketch" button, and your whole design will recompute from the edited sketch onward.  So, edit the sketch, make your change, "stop sketch", and everything should update correctly.

Hopefully this makes some sense and can help you get your brain around Fusion parametric modeling...

Jeff Strater (Fusion development)

[george]

OK, thanks for letting me know I'm at least on the right path. I think the trouble is when I create the component, decide to move it, and then go back to edit the sketch because the dimension is wrong. If I view the sketch it shows in the original compoent location so I think I need that first sketch moved into the compoent so if I change a dimension it moves with the component?

An example might help. Picture building an interior wall. So you have an outside wall on the left and right and then this interior wall. You then have floors and ceilings in the 2 rooms you just created. If I deicde the change the placement of the interior wall (changing the size of the 2 rooms) everything gets somewhat messed up. I've worked a little with parameters and I'm trying to use them but this whole process seems like a lot more work than it should be.

As a side note, I've created mid planes in the center of the walls. My thought was that this would make it easy to sketch rectangles that snap to the center of the wall (I plan on using dado cuts in the wood so the floors and ceilings should extend into the walls). It seems like construction planes work nice to use for measurements but only construction lines are available to snap to?

[jeff_strater]

Hi George,

Yes, you are right - if you move a component, and the component is defined after the sketch that created it, the sketch will not move with it.  You can still make this work, however.  In your example, if you are just changing the size of the rooms, then it should be OK that the rooms "move back" when you edit the sketch.  So, if you have a room that is, say, 10 cm, and then you move it later in the history, but decide that it should be 12 cm instead, you can still edit the sketch, change the 10 cm dimension to 12 cm, and stop sketch.  The move will still take effect on the new sized room.  That method can be a bit iterative, however.

Another choice is, as you say, to have the sketch be part of the component, so that it moves with the sketch.  To do this, though, requires a slightly different (but still valid) workflow.  In this workflow, you define your components first (as empty components), then "activate" them using the "activate" command on the right mouse context menu.  Then, create the sketches for that component, and they will be owned by the sketch.

A third choice is a "pure top/down" approach, where your entire design is driven by a few sketches.  This sounds close to what you are doing, with the twist that you are positioning components after they have been created.  In a pure top/down approach, the size and position of all the components are completely determined by that sketch.  So, to move a component, you would just edit that sketch.

I thought about creating a screencast to illustrate, but I'm afraid I would send you down the wrong path unless I have a better idea of exactly what you are doing.  Can you share your model, or even a screen shot of it?  If so, I can probably direct you more accurately.

Thanks,

Jeff

[george]

Sounds like in this case it might have been better to start with a component and then add the sketch to it. Here's a link to what I'm working on, http://a360.co/1JIZqi9.

I don't have everything in their final positions (like the the apex at the roof is not correct) but most of the bones are in place and once they are fixed I can start to add features (like windows and doors).

[TrippyLighting]

When working with Fusion 360, the first rule of designing discrete components ( not modeling/sculpting in the Sculpt environment) should be this:

1. Create an empty component by right clicking on the root of the browser and select "New Component"
2. Activate the component by enabling the little radio button to the right of its name in the browser or by right clocking on the name and selecting "Activate"
3. Then sketch and extrude whatever.

Whenever editing the component re-activate it before editing. If you just want to modify sketches this is not necessary.

As the timeline gets longer it will become hard to manage. Activating a component created with the workflow above will only show the timeline items pertaining to that component.

Another benefit of the above is that you can export such a component to use in another design. On export everything in that compoent gets exported including sketches, bodies, joint origins etc. If your sketch is outside of the component it does not get exported with it and you use an important part of it's parametrization.

[george]

Thanks, that confirms that I've started this design a little off track. In many of the instructions I've always seen starting with sketches first so that has been my default behavior so far.

I think my project is a good one to learn the proper design flow. If you create all the walls/dividers and floors/ceilings as components you can then easily handle changes later. But what is the best way to place and work with the parts? Should I create a master sketch and then use parameters to adjust positions or is that overcomplicating things?

[Anonymous]

I'll mention the "quick and dirty" way I'd probably do this instance, is to just draw single lines for everything in a single sketch (these lines represent the centerlines of the walls, floors, ceiling etc) then once you get that sketch done, exit it, go to the Patch environment, and extrude the sketch a desired amount (it will be a "surface" without any thickness).  Then go to Create > Thicken and do a drag selection box to select all these surfaces, and choose a desired thicken value, which will then create a body.  If you want, you can then define a sketch on the top or bottom face of this body, and add driven dimensions, by selecting an edge that you would like to know the length of (say for cutting boards), dimension it, right click and choose Aligned (dimension will orient with the line), and viola. 

Just a thought.

Jesse

[Anonymous]

Of course in the first sketch I mentioned, you can add vertical and horizontal constraints and angle dimensions (say for the roof), and dimension all the single line sides, and if you want to change a dimension, just re-edit the sketch to change, and everything should update parametrically.

I tend to not use components for smaller projects unless I know they will be necessary, such as for joints.  You can normally also move bodies, and sketches and construction geometry into a component after the fact, but of course if you know ahead of time you'll need components, then is really best to create them first and use component activation as TrippyLighting mentioned.

Jesse

[george]

Hmmm, the Patch environment is unchartered territory for me! But, using the centerline of the elements for the sketch actually makes the most sense. Since plywood thicknesses can vary I've set that value as a parameter but I struggled a bit on how to use that when I fix my final location of parts and need to make the dado cuts in the wood. Since I want the dados and rabitt cuts to be 1/2 the thickness this makes sense to make that a parameter and enter the value when I have the plywood in hand and can measure it.

That's the part that has me scratching my head a bit because the tickness dictates every position of the elements/parts. Of course I'm over analyzing the crap out of this but coming up with a good solution for this can yield a methodology that can be used over and over again in future projects. 

Thanks for all of your suggestions and help, it's pushing me down the right path I think and I hope that this can help others later on as well.

[Anonymous]

Hmm, to maintain constant room sizes for adjustments to wall/floor/ceiling thickness, when dimensioning my driving sketch (with centerlines), I would type a dimension as something like say '5 + thickness', where 'thickness' would be a user defined parameter (go to Modify > Change Parameters), which would accomodate for the 'thickness/2' removed from the room from each wall side.  When you do the thicken operation, for the thicken value you would type the same user defined parameter (in my case 'thickness'). 

Jesse

[Anonymous]

I need to correct a statement I made a little bit ago about the thicken operation creating a body.  A surface is already classified as a body, but I guess the terminology is that the ticken operation would take a surface body and create a solid body from it.

Got to keep terminology clear 😉

Jesse

[Anonymous]

I should also mention if taking this approach, that you can add trigonometric functions into the dimension expressions, such as for accommodating 'thickness' for your angled roof.  In this case you could dimension the angle of your roof with respect to horizontal, identify the name of that dimension, let's say it's labeled d11.  Then for your roof height, it might be '6.5 +thickness/2 +thickness*cos(d11)/2'

Be sure to let us know if you run into any trouble.

Jesse

[TrippyLighting]

I've created a screencast of how I would approach it. You don't sacrifice anything as you still work with components that you can later create a drawing from for the shop or have laser cut or cnc routed. For an initial design where you still may explore proportions it is more flexible than working with construction planes, even though these can be constrined to a non-dimensioned sketch as well. 

The trick is to constrain your sketches well. That provides you with the functionality.

[Anonymous]

Nice step by step screencast!

[NicolasXu]

Good sample to show the parametric modeling process as well.

BTW, the Preferences setting can be accessed from the account drop-down at the top-right corner. 🙂

Regards,

[george]

Yes, once again you've gone above and beyond expectations. This is exactly the type of model I was thinking could be achieved yet I couldn't figure out quite how to do it myself. I need to apply what you've done to roof.That's a little more complicated but I'll give it try!

[Anonymous]

Hi Trippy,

Thanks for clearing this up, I had no idea this was how it worked. Any idea why the behavior you describe above isn't the default for creating geometry in F360? I can't think of a time when I wouldn't want my sketch to be unit contained within my geometry? Seems like another very curious decision on the part of AudtoDesk . . .