Moving a component results in ghosts. Yikes

[7milesup]

When I move a component (or body for that matter) I end up with "artifacts" that are left behind.  I am sure that I am missing something super simple but it is driving me nuts.  Nuts are bad.  Calm is good.

[chrisplyler]

A ghost? That's your Sketch10 in the assembly.

Why are you moving bodies away from their sketches? And why are you making so many sketches? And why are you starting the second tray off to the side away from its origin? Please take a look at my file.

You should have TWO components. ONE sketch per component will do everything you need in this case. The two components are JOINTED into position properly...no body moves. Actually only made the first component, then just did a copy/paste new to generate the second one and modified it's width. Made the joinery bits last on both of them.

[7milesup]

Thank you for your response.

Why am I moving bodies away from their sketches?  Well, I think that that is the crux of my problem.  Why, if I draw on the face of a body (or component), does the sketch not stay with that component/body. Why is it not grounded to that? I am obviously doing something fundamentally wrong. 

Also, as far as moving bodies, I would consider that as being a necessary part of CAD.  I would think that one would not draw everything exactly in its final position.

The drawing I uploaded is only a small part of a design, and it needs to be in multiple sections to fit on my 3D printer, should that be the route I go.  I may develop this on my large CNC but I wanted the option to print it.

Last question.... Let's say that I want to draw multiple "boxes" that are different sizes with the "tab & socket" that you see in my drawing (for alignment purposes).  There will be at least 10 of those boxes.  Do I draw each one in a seperate file and then assemble it in another file?  Or do I draw all of them in one file and then assemble them in another file. 

I did watch a very good video from Autodesk last night concerning components and bodies.   BUT, I apparently suck at learning stuff on line, even though I don't think I am exactly the dumbest person around.

[laughingcreek]

everything he said is spot on and should be heeded.

but to answer the specific question, what your seeing is a profile created when you placed a sketch on the surface of geometry.  by default, a selection in preferences called "auto project geometry on active sketch plane" is selected.  This creates invisible lines at the edges of the geometry, which of coarse creates a closed profile.  Why does it do it this way?  Somebody at AD thought it would be  good idea.  I find it annoying and not useful. Here is a screen cast showing what I mean...

[chrisplyler · Accepted solution]

It's a Component world, my friend. You can certainly sketch on the side of an existing body, but HOW you establish that sketch is important. If you have the Component active when you create the sketch, it will be inside that Component, and it's position will be related to the origin of that Component. If the body is also inside that Component, and thus its position is also related to the origin of that Component, then if you move the Component, the sketches and bodies inside it all move together as one.

If, however, you make a Component and make a body inside that Component, but then you start your sketch while the Component is not active, the sketch will be placed somewhere else in the Browser hierarchy, and will NOT have a location related to the origin of that Component. So if you move the Component, it will take the body with it but not the sketch. In the case of your file, you've got Sketch10 (and nine others) under the main assembly in the Browser hierarchy. So they are positioned relative to the main origin, not the origin of any Component. So when you move the body, or even the Component the body is in like you should, those sketches won't move regardless.

Now, if you move a BODY, you are effectively moving it inside its parent Component, RELATIVE to its origin. Even if you have located the sketch properly within the Component, the sketch is still in the same location. You're moving the body away from the sketch. Don't do that.

[TrippyLighting]

@7milesup 

as @laughingcreek has posted out these "ghosts" are sketch outlines that are auto projected. I also find this an utterly useless feature that can be turned off in the preferences and IMHO should be turned off by default.

Then you'll have to project things manually but have precise control over what you are projecting and you won't have projected rubbish in your sketch that you did not ask for.

There is written documentation that explains the difference between a component and a body. In most mechanical designs you don't want to move bodies, but components. The move command for bodies is mostly a modeling tool. It shouldn't be used to locate components in reference to each other, that is the purpose of the joints in the assemble menu.

As far as designing components in place in their final locations, that is very much part of CAD and is called top-down design.

In fact that is Fusion 360's best suit.

The other way around, designing parts at the global origin and then moving them into place (mind you, with joints, not with the move command!) is called bottom up design.

Most mechanical designs are more bottom up, because as soon as you start importing parts that you might have downloaded that's a bottom-up workflow.

Much of product design is more top-down. But in general most designs are a mixture of both.

After reading about bodies vs. components hop over to Fusion 360 R.U.L.E #1. 

This link above actually leads to a whole list of links to educational resources. Watch some of the Autodesk University lectures. These are created by those people that design Fusion 360. 

[chrisplyler]

Now as to the preferred method when multiple different parts will have some bits in common...

It's up to you how you organize stuff. I personally much prefer to build it all in one file. I take advantage of the fact that sketches in the main assembly won't move with other stuff by putting a sketch there of the common bits, and using it over and over to generate those common bits for each Component that otherwise has its own sketch(s).

Here is an example of using one common sketch (outside of any of the four Components) to generate the bodies and control the relative position and sizing of all four components at once.

https://knowledge.autodesk.com/community/screencast/8fe69d54-bd1b-4c20-ab46-447f62b4586b

Here is one where I put three common sketches into a different component by themselves, but they create/control bodies in other components.

https://knowledge.autodesk.com/community/screencast/05c8dafd-d809-4b3b-89b8-88ba07f676d1

Here is one where I use a "jig" of common sketches to create several differen't (but similar) components, like a production line. Keep in mind while you watch it that I just dragged the bodies out of the way as I made them, but I should have done a move on the whole Component each time instead.

https://knowledge.autodesk.com/community/screencast/4888c6c9-e532-4469-a858-4cd59cbfa829

So I'm taking advantage of all the stuff I explained in my previous post to suit my needs. You have to know the difference and decide when it's appropriate and when it isn't.

[7milesup]

Everyone, thank you so much for the replies.   I am away from the computer until this evening but I am taking all suggestions to heart. 

Getting the basics down is vital and I know that after reading these responses that I am missing some basic building blocks.  

[7milesup]

Did some reading and watched the videos.  Thought I had this figured out but apparently not. 

Watch my screencast please.   Why is the sketch still not "attached" to the component that I move? 

Times like this, with such a basic problem, I would like to throw the computer out the window. 

[laughingcreek]

Because you have the move command set to move bodies and not components.

[7milesup]

Thank you.