topic Re: Component Workflow in Fusion Design, Validate & Document Forum

Component Workflow

Anonymous — Wed, 23 May 2018 19:08:11 GMT

I have two parts. Each are their own component. Number (#1) was my first component with the round hole (diameter). I then created a second component (#2). I sketched (#2) on the top surface of part (#1). Both parts are their own component.

I want to increase the round opening (#3). When I do, it closes the whole gap on at (#4). This entire perimeter are closes when I change the diameter of (#3).

I'm confused because if I made each part as a separate component, why does it effect the geometry of part (#2)? Is there a way to edit the round opening without effecting any other geometry?

My out loud thoughts:

I'm thinking I should not have sketched part (#2) on the top surface of part (#1)? How else would I have done it otherwise?

Re: Component Workflow

chrisplyler — Wed, 23 May 2018 19:06:13 GMT

It's difficult to understand your problem based on your description and the picture. What is a "round hold?" Why do you call #3 a round opening but the #3 in your picture seems to be calling out the outside diameter?

If you can attached an f3d file, or provide a link to your project, I'm happy to take a look at it.

Re: Component Workflow

Anonymous — Wed, 23 May 2018 19:10:33 GMT

My apologies for the typo. I corrected this; hold to "Hole" (diameter) to help synchronize terminology. I can't share the model with you at this time.

Re: Component Workflow

lichtzeichenanlage — Wed, 23 May 2018 19:45:40 GMT

Have you projected profiles from one component into the other?

Re: Component Workflow

chrisplyler — Wed, 23 May 2018 19:58:44 GMT

If you did not intentionally set up a relationship, then you MUST have accidentally auto-projected from one the sketch or geometry of Component#1 into the sketch of Component#2.

Re: Component Workflow

Anonymous — Wed, 23 May 2018 20:57:03 GMT

Not that I'm aware of. I simply created a new component, and then started a new sketch. When asked to select a plane to sketch on, I selected the the top planar surface of the part #1 because I wanted to build the new component on that level.

Re: Component Workflow

Anonymous — Wed, 23 May 2018 20:58:23 GMT

I'll have to double check if I did project accidentally. If I did, what options do I have to break this relationship, but still keep the component at the desired surface level?

Re: Component Workflow

lichtzeichenanlage — Wed, 23 May 2018 21:11:55 GMT

Edit the sketch with the projection and:

Re: Component Workflow

Anonymous — Wed, 23 May 2018 21:48:38 GMT

Thank you! Unfortunately, I do not have that symbol. I've gone ahead and attached the model for reference. Here are my thoughts.

1. I have three main components. Aluminum, Plastic and Steel.

2. I want all three to be individual components, but the steel part needs to be copied in a circular array 4 times.

3. I need to edit and modify the Aluminum, Plastic and Steel individually.

4. At some point, I need to extrude the Steel part through the Plastic part.

This is my workflow issue overall. The materials I mentioned are listed in my browser. Generally speaking, I need all components to align properly, but have individual control to sketch, extrude, rotate and array as I choose.

Re: Component Workflow

chrisplyler — Thu, 24 May 2018 03:14:44 GMT

Re: Component Workflow

lichtzeichenanlage — Thu, 24 May 2018 06:04:27 GMT

@BillyRaygun wrote:
...
This is my workflow issue overall. The materials I mentioned are listed in my browser. Generally speaking, I need all components to align properly, but have individual control to sketch, extrude, rotate and array as I choose.

As @chrisplyler already mentioned, you can disable the default projection. That's what I did in my setup, too.

For the workflow you should have to things in mind:

Follow Rule #1
Prefer joints for assembling (positioning) parts
Try to always include the origin in your sketches

The screencast shows one way of doing it and could be summarized like this

Create a component
(Rigit) Join the origin of the origin to the center of destination
Sketch by including the origin (in this simple example an extruded rectangle)

This is just one way to work with joints, but would do the trick for you in this case.

Re: Component Workflow

TrippyLighting — Thu, 24 May 2018 10:40:20 GMT

There are two things I look at right at the beginning when analyzing a users file:

1. Where are the component origins. That's OK in your design.

2. How do the sketches look like. Not OK!

3. The component structure looks OK

Why:

1. Your sketch is not fully defined, meaning it is not fully constrained and dimensioned. It isn't hard to imagine that things break or unexpected results occur with under defined sketches.

2. The fillets do not belong in the sketch. Use solid modeling fillets. Not only is this faster to model, it also faster in performance and more stable in behavior.

I also feel that you are misunderstanding the component structure. If you create the sketch for component 2 on the geometry of component 1 then that creates a relationship between the two components (as @chrisplyler has pointed put in his screencast). So when you change component 1 it still might change component 2.

Having 2 separate component does not mean that there is no relationship between the two.

Re: Component Workflow

chrisplyler — Thu, 24 May 2018 12:56:22 GMT

@TrippyLighting wrote:
If you create the sketch for component 2 on the geometry of component 1 then that creates a relationship between the two components (as @chrisplyler has pointed put in his screencast). So when you change component 1 it still might change component 2.

Yes. I failed to mention this in my screencast, but EVEN IF you don't create any in-sketch relationships (intentionally or otherwise), you have still the relationship created by the fact that you began the sketch using a face of geometry instead of a stand-alone plane. Since you associated the sketch to a face of geometry, the sketch will MOVE with that face of geometry.

So in the case of this thread, the Steel component would move up and down if you change the thickness of the Aluminum component. It wouldn't get messed up, but it would always stay on that face.

Now sometimes that's what you want, so no problem. But sometimes it isn't what you want, so you should be aware of how that works. If you don't want that to happen, you make a new plane offset from the origin instead of based on a geometry face, and you start your sketch on that plane instead of on that face.

To TRULY keep components unrelated, I prefer to build each one on its OWN origin, and not necessarily "in place" where it belongs in the assembly. Build it completely unrelated to any other component. Then use an assembly Joint to put it in the right place/orientation. Now in this way, the component isn't dependent on anything else in the assembly. It could be exported out and used in a totally different assembly file, and only require a new Joint be defined. If you try that with your Steel component, with it's sketch location depending on a face of another component, then you can imagine that it would go screwy if you tried to export it out to exist on its own. It would be wondering where the heck its sketch belonged.

Re: Component Workflow

Anonymous — Thu, 24 May 2018 18:10:20 GMT

@chrisplyler Thank you for the video tutorial. This was very helpful. I confirmed my settings and I did in fact have auto project boxes checked. I immediately unchecked these. I think the culprit was in fact this setting as I was not anticipating or expecting this functionality.

I very much appreciate you taking the time to help me with this issue.

Re: Component Workflow

Anonymous — Thu, 24 May 2018 18:17:40 GMT

@lichtzeichenanlage - That was very cool. Thank you for sharing. I know the importance of joints, but just haven't practiced using them. Watching your workflow, I never realized how powerful joints can be. I'm going to have to practice this.

Re: Component Workflow

Anonymous — Thu, 24 May 2018 18:26:37 GMT

Thank you @TrippyLighting - Point number 2 - I debated with myself for a while on this. It's so easy to draw in Fusion 360, its easy to get into too much detail. What you say makes sense and I'll have to practice that.

As for two separate components, I was in fact assuming there was no relationship. Everyone who jumped in here to help has proven why things were not performing as expected. So much to learn!

Re: Component Workflow

Anonymous — Thu, 24 May 2018 18:33:18 GMT

Excellent information @chrisplyler - This workflow makes complete sense and seems to follows @lichtzeichenanlage thinking.

How you described sketching on the face of existing geometry is exactly what I was doing. Seemed logical but as a Rhino 3D user, I didn't have to think about the relationship the new part has with others.

Everyone's help here has been great now I just need to practice. I do want my parts to have a relationship with one another, but not totally. As I experiment more, I think I'll find a workflow that follows the advice here, but will allow me to achieve the results I need for this specific project.

Thank you @chrisplyler @TrippyLighting @lichtzeichenanlage !

Re: Component Workflow

lichtzeichenanlage — Thu, 24 May 2018 18:58:52 GMT

The first time I've seen that joints could be applied not only to bodies (inside of components) but also to sketches or origins my jaw dropped followed by dirty words I don't want to post again 😉

@Anonymous wrote:
@lichtzeichenanlage - That was very cool. Thank you for sharing. I know the importance of joints, but just haven't practiced using them. Watching your workflow, I never realized how powerful joints can be. I'm going to have to practice this.

Re: Component Workflow

lichtzeichenanlage — Thu, 24 May 2018 20:04:33 GMT

That's the post which blew my mind:

https://forums.autodesk.com/t5/fusion-360-design-validate/joint-to-create-a-truncated-icosahedron/m-p/7866963/highlight/true#M153533

Sry for the raw link, format options aren't available on my phone 😉

Re: Component Workflow

Anonymous — Thu, 24 May 2018 20:59:02 GMT

Excellent! Thank you for sharing!