Body Movement

[Anonymous]

I'm having trouble moving a body.  Whenever selected, parts of the sketch used to create the form don't move.  I've attached an image.  Is there some way of creating a single sketch from the many lines used to create it?  This way it will be treated as a single unit.  I can extrude and create a body, however when moved it isn't treated as single entity.

Thanks,

Tim

[Beyondforce]

Hi @Anonymous,

You should be aware of the difference between moving a body vs a component.

Watch this: https://www.youtube.com/watch?v=9DiwbQMQXNQ

Cheers / Ben
---------------------------------------------------------------------------------------------------------------------------
Did you find this reply helpful ? If so please use the Accept as Solution or Kudos button below.

Check out my YouTube channel: Fusion 360: Newbies+

[Anonymous]

Thanks Ben,

I watched and appreciate your sharing the video.  I'll be watching the others in the coming day (I have a lot to learn).  I'm back to my original question.

1) Is there something I am doing wrong when attempting to move the many lines that make up my sketch?  I've created multiple sketch's that make up a single entity to extrude to create a Body.  Should I be somehow binding them together before creating a body?

2) When I extrude to create a body, is it common to move that body away from the sketch or keep it unified as a single entity?  It looks like I can extrude multiple bodies from a single sketch enabling me to draw a single table leg and create 4 bodies of the same measurements.  I know I can create them individually and constrain them to match dimensions, butthat looks like a lot of work.

Thanks again for all the help,

Tim

[Beyondforce]

When I look at the attached image, I can see more than 1 sketch. Is it because you are going to extrude each sketch separately in order to create different bodies?

[ToddHarris7556]

@Anonymous - 

It looks like you're probably modeling several separate pieces in the same sketch. This might be viewed as a 'bottom-up' approach. Your sketches all appear to be pretty independent of each other, but after you've turned them into solids (more on this in a second), your intention is to stick them all together. All's good so far.

A good rule of thumb when you're modeling like this is to use one sketch for each feature/part. Not that you couldn't conceivably do it the way you're doing it, but things will get wonky and unreliable fast. So in short - one sketch for the leg. One for the apron, one for the stretcher, etc. Don't combine them. You'll drive yourself batty.

UNLESS - 

You start to get into 'top-down' modeling (aka skeletal modeling). In this case, you often combine several master sketches - say, a plan, a side elevation and end elevation - that show how all (or some) of your parts relate to each other. Then you use those sketches usually with workplanes to create solids. It takes a bit of work up front, but ends up creating very robust models.

NOW - 

I've only referred to 'solids' so far. 

In reality, you're creating bodies. Which may or may not be contained in components. The easiest rule of thumb I can offer here is that usually if it's a separate physical piece, you'll want it to be a component. Think of your Fusion file as a master component. (Or assembly, if you prefer) It might consist of 4 leg components, a top component, a couple of long stretcher components, and a couple of short ones. Etc. Within each of these components, you'll have one or more bodies. Think of bodies as geometric pieces that you use to stick together to make your component. 

It takes a little to wrap your head around it, but it sounds harder than it is, once you get a workflow going. 

[Anonymous]

Todd,

Am I understanding this correctly?

I've created a sketch using multiple types of lines (Curve, Rectangle, and Spline).

Extruded the enclosed sketch area to create a body (leg).

I then sketched small boxes (mounts) onto the extruded leg then extruded the sketch box.

I used pattern to create a series of blocks (mounting points) down the leg.

The result looks good but I see several complexities/issues with annotation. 

Question:

Am I following good technique extruding multiple bodies from a single source sketch? 

- Where should the sketch source for the leg body go?  I'm going to create multiple iterations of the same sketch.  With Multiple legs, do you keep a single master that all others follow when changed?

It seems that adding extruded bodies (mounts) to an existing extruded body (leg) without reference to the sketch would be problematic. 

In the end, I'm looking to understand the relationship between the sketch and model environment.  Any reading or video training would be greatly appreciated.

Thanks!

Tim

[ToddHarris7556]

Good morning, Tim, 

As @Beyondforce mentioned, there are several sketches. There's nothing inherently wrong with that. 

The clue that suggests where you might be running into trouble is "should I be binding them together" coupled with the fact that it sounds like you're actually trying to move sketch entities. 

THAT may be where your problem is.

Try this:

- Create a single sketch with one enclosed form in it. Extrude it. This body serves as the master form that everything else gets built off of. 

Now, there are a couple (or probably eight) ways to proceed - 

a) you can go back into that original sketch and use geometric constraints and dimensions to 'bind the bits together'. i.e. if you're going to sketch a mounting block, then it needs to be sketched in the right spot, up against the master profile. Then when you extrude the master form, you simply select these block boundaries as well, and the whole thing gets built in one extrusion. OR

b) start a new sketch ON THE FACE OF THE MASTER BODY. Use 'P' to project one side of the body into your new sketch. You can either leave it as a solid line, or turn it into construction geometry. Sketch your new feature (mounting block) constrained to this line. Stop sketch, and extrude/join. Now you have two sketches, but one body (because the new extrude JOINED the first one)

Sorry - I'd do a quick screencast, but I need to run to a meeting. I can get one later if the description's not enough. 

In short, the 'best practice' that you're searching for has, I think, to do with completely constraining sketches, and not trying to move them around. Yes, you *may* be able to do this by moving bodies around, but I'd see that as 'fraught with peril'. 

[TrippyLighting]

---

@Anonymous wrote:

1) Is there something I am doing wrong when attempting to move the many lines that make up my sketch?  I've created multiple sketch's that make up a single entity to extrude to create a Body.  Should I be somehow binding them together before creating a body?

2) When I extrude to create a body, is it common to move that body away from the sketch or keep it unified as a single entity?

---

The very first thing as @Beyondforce has already mentiond is that you really ned to understand the differnce between a component and a body whichis described here.

In the end for all your discrete pieces for the table you should end up as components.

All "objects" that were used to create the body of a component should "live" in that component. the sketches, construction planes, construction axis, joit origins, etc.

Most sketches really serve as a starting point to create geometry and if a sketch is used to create a single discrete piece of a table leg, the sketch sould be part of the table leg component as well as the body that represens the 3D geometry of the table. A body does not have it's own origin, a componet, however does.

As such most of the time you want to move components around in your design, not bodies.

Moving a component will keep the sketch and the body together. You should not move sketch entities to move your 3D geometry into place.

To assemble your components into the final functional table you would usse the joints inthe Assemble menu.

To work with components, you should review Fusion 360's R.U.L.E #1