Workflow Question - Enclosure Panels

[Josh__]

Hi all,

I'm a beginner with Fusion 360, but I am learning! I am going through the self paced tutorials. I have a quick project that I'd like to attempt right now though, and I'm unsure of the best workflow. For reference, I come from AutoCAD, and this style of modelling is very different for me.

What I'm trying to do is create a small panel for an electronics enclosure. I've done it in a different CAD program, but I want to do it in Fusion now. This is what I'm looking at:

So, what's the preferred Fusion workflow for this? Start with a sketch of the overall shape, then extrude, then use the hole tool? Should I be creating the outline in the sketch and then extruding once the holes have been removed?

So many options, I'm just trying to avoid starting down the wrong path and banging my head against the wall later.

Thank you in advance for the help!

[Beyondforce]

Hey @Josh__ ,

It is fairly simple, just don't forget dimensions, constraints and to follow R.U.L.E #1

[davebYYPCU]

Short answer to get you going, 

if that exists in autocad, save it as dxf and import it to Fusion.

Place it so symmetry around the origin will work for you and not hinder you.

All goes well, you see the blue highlight of Bens pic, you can select that by clicking in the open area, and extrude a plate with holes - done.

There is an external rib boundary, select that as a second extrude because will be a different height to the first extrude.

Long answer - basic

One fully constrained sketch per function, until you learn to do it my short answer way.

Sketch patterns are not recommended, but for a small job like this will not break the system.  

Text in a separate sketch,

holes in a separate sketch, and

sketch for the plate itself, is the compromise between the two versions I have discribed.

there is no right or wrong, some things are better.

Might help.....

[Josh__]

Thank you @davebYYPCU  and @Beyondforce !

This particular one does exist in another CAD package so I could just import the DXF. I'm trying to avoid that for now as I'd like to use this fairly simple project to learn.

I'll start with sketches and extrude from there. Some of the holes are for countersunk screws, so I'm hoping to use the hole tool for them.

Why do you say no patterns? In this particular case I don't think I'd use them anyway, but I'm curious the thought behind it.

Is there a way to save a pattern of holes as a block or preset of some kind? The one larger hole with the two smaller holes off axis are for a panel mount connector I use frequently.

Thank you for the help!

[davebYYPCU]

Sure, teaching exercise in Fusion,

Countersunk holes, no need to extrude them, you will need a sketched centre point to make it easy, 

Extruded cut holes and chamfers,

which is better, it is design dependant.

Keep Sketches simple, this is a parametric system, every line and article in a sketch is driving Fusion (mad) in the background, establishing constraints, dimension limits and considering alternatives. 

So a few "layer" sketches in your example is the way to go. Solid, - holes and centre points - and text.

Fully constrained sketch has all black articles or a combo of black and purple.

Blue and Orange lines and most white points, in sketches will now keep you awake at night.  These are the source of most trouble when sketches break on parameter changes.

So reusable stuff, goes in it's own component, save the component out to a stand alone file, and it can be inserted into many files.  Can be just the sketch, or spaced bodies for Combine Cutting.  So many ways, need to see your file for best options, but we are not there yet.

So no sketch patterns for the constraining workload that brings, when a modelling pattern will do it quicker easier, some can't be avoided.  Same for sketch Fillet against model Fillet model fillets near the end of file - the better option.

Use centre plane origins when there is symmetry.

Might help...

[TrippyLighting]

Don’t import .dxf files. It will probably work, but you are just shortchanging your learning experience.

For people coming from traditional 2D CAD systems, sketching is often a big hurdle.

The sooner you’ll get that behind you, the better 😉

[Beyondforce]

@Josh__,
I 100% agree with @TrippyLighting!
There is no reason to import a dxf file for a few circles and squares. In general, a dxf file can reduce F360 performance (depends on the number of geometries). - KEEP IT SIMPLE 😉

[Josh__]

Thanks again for the advice! Here's what I came up with:

Here's the sketch for some of the holes:

Here's the sketch for the Text:

 And here's the shaded view!

 

So I seem to have done what I set out to do, thank you for all the help!

I do have some issues constraining the text where I want it, though it seems I am not the only one with that problem.

I was not entirely sure when to apply rule #1. I know this is a simple project, but I am hoping to someday build up to more complex ones.

Should I have converted to a component immediately on extruding the panel into 3d? Or after I cut holes?

Thank you!

[davebYYPCU]

First pic has too many duplicated dimensions,

horizontal hole centres - one dimension,

equal sized holes, dimension one.

Add dimensions as required to the text insert point.

Rule No 1.  Not required for this part, until you add another part to the file.

Test is, how many individual real world parts will the model have?

More than one, use Rule no.1, 

Make the Component first, activate it, then make one part in that component.

Repeat.

At any time You can work in other activated components,

always activate the component you are working on, after reloading the file you have to activate the right one.

Should avoid making components from features or bodies, because the sketches will not be included.

There are exceptions, but very much Design Dependant.

Might help....

[davebYYPCU]

You can fairly advanced pretty quick...

When you start thinking about reducing sketch patterns, you will have similar to this for the bottom set.

From the left or the right it was the same pattern...

plate's Solid fillets at the end of timeline, 

Rectangular pattern 26mm to the left then circular pattern the pair.

then making a component of that original set can be re utilised.

Might help....