Help me understand the design process

[Im1in260m]

I design things in wood. So I am always using 2X4's, 1X4's, etc. These are always assembled into something such as a workbench, cabinets, whatever. If I draw a 2X4X8 feet for a frame I should make a component from the body? If I need two of these for the same frame, should I use a copy of the first, or create a new body? Then assemble the two components to make the frame? I don't want to get finished with most of the workbench and find out I should have done one thing or the other. Using the example above, suppose I am making a box frame on which I will attach a sheet of plywood. I have two 2X4X42" and two 2X4X96" and one sheet of 3/4" plywood. Should all 4 of the 2x4s be individual components?

Thanks for the help.

[TheCADWhisperer]

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@Im1in260m wrote:

I design things in wood.

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Can you Attach prior designs that you have already completed in Fusion 360?

How many projects have you done with multi-body solids?

How many projects have you done with components?

Will any of your projects have moving components, example - drawers?

Are these projects for your use only - or do components get sent out to vendors (or even other users on the shop floor)?

Can you File>Export your *.f3d file to your local drive and then Attach it here to a Reply?

[jeff_strater]

@Im1in260m - these are good questions, and important to understand from the start.  A couple of rules I would recommend for this type of design:

• always use components from the start.  A 2x4 is a good example - you know this is something that you will buy as a unit, so it should be a component from the start.  Don't model these as bodies.
• always use component instances of any component where the geometry will be the same.  If you have two 2x4x8s in your design, they should be instances of the same component.  It probably is not a big deal in a design the size of a workbench, but if you get a larger design, the efficiency that results from sharing geometry will become noticeable.
• If you have a component that is a slight variation of another, use Paste New.  This creates an un-associated copy of the component that can be edited independently.  For example, say you have a 2x4x8 that has a different set of holes drilled in it from the main 2x4x8.

admittedly, Fusion is not great at managing these kind of "cut to length" components.  Because lumber comes in fixed lengths, if you end up having two 2x4x8s  and two 2x4x7s in your design, what you want for a shopping list is four 2x4x8s, because you cannot buy 2x4x7s.  Because of the shared geometry with components, these 4 cannot be the same component in Fusion.  So, that part of the bill of materials becomes a more manual process.

[laughingcreek]

another set of suggestions-

-flatwork wood working is frequently easiest to model using skeleton sketches at the top level, and producing components by extruding from them (setting the extrude type to new component reduces the number of steps to work this way)

-utilizing skeleton sketches allows for a top down design approach, which I find easier to manage conceptually. Also makes it easy to build most components in place, which makes joint creation easier.

-check as you go that your sketches are responding to dimension changes as expected

attached is an example model I did for someone a while back.  you'll note that everything is controlled from the first 2 sketches.  double click a dim to make changes to the model.when constructed like this, if the model blows up on you it's typically easy to trace the problem back to a sketch just by looking at it. 

also when constructed like this, components don't reference each other directly, but rather go back to the higher level skech.  so if you delete a component (vs using remove), you won't generally break the whole model from a cascade effect of referencing component to component.

p.s. turn on "componnet color cycling" under the inspect tab so you can see visually which components are reused instances.

[Im1in260m]

Thank you both very much for your responses. I am designing component by component. It seems a little more intuitive. I create a sketch, extrude it as needed, then create a component from the body. I did not use copy and paste in place. I am going to have to revisit that.

When you have 5 components that make up a drawer, can you just group them together to make a single "Drawer" component? Of course, I'll try this before any one has a chance to respond, but I expect there will be cautions and suggestions when doing this sort of thing. I look forward to those responses.

[g-andresen]

Hi,

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@Im1in260m wrote:

I create a sketch, extrude it as needed, then create a component from the body. 

1. create  component > sketch > body inside that (active) component

When you have 5 components that make up a drawer, can you just group them together to make a single "Drawer" component? 

1. create component „drawer“  > inside „drawer“ > (sub)components (left, right, back, front,bottom )

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Günther

[shahriarsifat1802164]

Hi,
If you are trying to make assembly, of course, you need to make them separate or what can I say individual components.
Thank you.

[shahriarsifat1802164]

Can you please share your project with us so that we can collaborate here.
Thank you.