Multiple component, parametric design and origins .. how?

[Anonymous]

Coming from SW I really start to like working with 1 file, multiple components in Fusion 360. However I can't seem to understand how to create a parametric design with multiple component, where each component has a suitable origin placement for that component.

My question is better explained with this tutorial of Lars Christensen: https://www.youtube.com/watch?v=nZ2ymIljiWk

He first creates mulitple empty components and start drawing the front panel on the front plane of the origin. The frist (right) side panel is created on the side of the front-panel. The origin of the side-panel is therefore the same as the front-panel. Coming from SW this is very unintuitive because each part has it's own origin. But so do Fusion 360 components. So how do I properly create a parametric design where the other panel are actually based on the front-panel but where each component has a properly placed origin.

I have looked through many tutorial but haven't found the one touching on this subject. So am I maybe looking for something completly unnecessary (due to different workflows in Fusion) of am I missing something really obvious?

[davebYYPCU]

You have modelling experience, you are aware of the uses of the origin, but I am not aware how that relates to the question, 

Are you asking about Assembly verses in situ modelling? not sure.  

[jeff_strater]

not sure what you mean by "a properly placed origin" here.  What is "properly placed"?  Do you mean that the geometry for that component is located around its own origin?  You can certainly model that way in Fusion, even with local components.  The workflow would probably require you turning off the rest of your design in order to do so, because, as you point out, all local components' origins are initially at the same XYZ location and orientation, and there would be a lot of geometry at that origin.  But, you can definitely do that.  Then, when you are finished with that component, you can use Joints to put it into the right orientation with respect to the rest of the design.

However, working that way is probably less efficient.  The power of local components is the ability to build things in place.  This allows you to easily use geometry from other components to build a new one (you can project geometry from side panels to build the front panel).  This technique is not without its downsides, as those cross-component relationships can be points of failure in the model, when updates happen.

If this explanation is not clear, I can record a quick screencast to illustrate.

[kb9ydn]

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@Anonymous wrote:

Coming from SW I really start to like working with 1 file, multiple components in Fusion 360. However I can't seem to understand how to create a parametric design with multiple component, where each component has a suitable origin placement for that component.

My question is better explained with this tutorial of Lars Christensen: https://www.youtube.com/watch?v=nZ2ymIljiWk

He first creates mulitple empty components and start drawing the front panel on the front plane of the origin. The frist (right) side panel is created on the side of the front-panel. The origin of the side-panel is therefore the same as the front-panel. Coming from SW this is very unintuitive because each part has it's own origin. But so do Fusion 360 components. So how do I properly create a parametric design where the other panel are actually based on the front-panel but where each component has a properly placed origin.

I have looked through many tutorial but haven't found the one touching on this subject. So am I maybe looking for something completly unnecessary (due to different workflows in Fusion) of am I missing something really obvious?

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In fact Solidworks works very much the same way Fusion does; if you create new parts from directly within an assembly (Insert Components->New Part) instead of creating them outside of the assembly and inserting them afterwards.  When done this way (insert then edit) the origin of a new part corresponds to the origin of the parent assembly, regardless of where you actual start modeling from.  I suspect the create part then insert method is the way most Solidworks users do things, which is kind of unfortunate because it really enforces the one-part-per-file paradigm where you completely miss out on the flexibility of virtual components.  With virtual components you can create as complex an assembly as you like, all in a single assembly file.

So my question is, how are you doing it in Solidworks?  Do you create a new part outside of the assembly and then insert and mate it into place?  One way to do the same in Fusion is to create each part as a new design and then insert into another design (assembly) as an externally linked design.  It's pretty much the same as you would do in Solidworks, except for the clunky data panel in Fusion (sorry, just really hate the data panel in Fusion).

Another way in Fusion would be to isolate the component you're working on so it's easier to see the origin entities.  Then add joints for positioning later.

C|

[Anonymous]

I agree with you @jeff_strater that 'properly placed' is very ambiguous 😀. Something along the long of 'the geometry of each component is located around each individual origin' does indeed make more sense.

Using the workflow like you suggested will probably limit me in making paramtric designs in more complex design (I will probably get around with this simple drawer example, but not with more complex designs).

Pretty much every tutorial, no matter which 3D moddeling software, starts with: "It's very important to think about the orientation of your first sketch in relation to the origin because it defines the entire future workflow or that part/component". I myself use the origin and its planes regularly for features like mirroring and symmetric sketches. Also, the origin defines the orientation that's used in drawings for example.

Now let's say I have a (assembly) component as in the file attached. It's a 3 panel component (front-panel, a panel placed at an angle referencing an angled face of the front-panel, and a side panel 90 degrees to the front-panel). I created this example based on the workflow as shown in the turorial of Lars. The result is a parametric component, but with origins all in the same location.

From what I understand from your comments I either chose the 'parametric design'-workflow or the 'origin'-workflow based on my future needs. So, if I have to make drawings of my 3 panel component it would be better to sketching each component based on its own origin, than use joints to join the components together. If not, I could chose to let go of the position of the origin and start sketching components based on other components' faces. As with many things in life, I'd like to have the best of both world but I have to make a decision in which path I chose 😋.

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@kb9ydnI never really liked virtual components in SW and primarily used them (occasionaly!) for some dimension referencing of the actual part I was creating where the virtual component is not part of the final assembly. Also making drawing of each individual virtual components is pretty much a no-go for me. So in SW I use the more traditional one-part one-file method, where each part is defined around it's own origin, but losing some flexibility in parametric designing. (I know I can perfectly achieve this in Fusion 360 as well 😉)

[chrisplyler]

Easy.

Lets suppose you are going to create a box. You're going to start with the front panel, and you figure you will model it with the Origin along the bottom edge, in the middle of the length (because you've decided to use side-to-side symmetry). Okay? Fine.

Now create a new Component for the first side. Take ITS origin and Joint it where you want it to be onto the body of the front panel, and then start modeling it from there. It doesn't even have to be ON the front panel body...you could click there to establish it, and then use the offset settings to put it half way down the intended side depth, or whatever, if you wanted to.

Notice how I still project an edge from the front panel, and use it in the sketch of the side panel, in order to create a dependency that I want (being the box height). Create dependencies like this, or be careful NOT to accidentally create dependencies like this, depending on how you want things to be set up.

Notice that I started to make a second side panel from scratch also, but then thought better of it and just Copy/Pasted the first side panel to create the second one, and Jointed it into position. I chose to do it this way because I know I always want those two side panels to be exactly the same. If I was to create a Bill of Materials now, those two side panels will show up as a single part, with a quantity of two. Now, if you were going to have a hole in one side, but not the other, they would NOT be exactly the same, and so you would want to model them separately/ individually.

https://knowledge.autodesk.com/community/screencast/f3f900bf-9a77-4c10-a591-3dc7c17049fc

[chrisplyler]

An alternative to the method I demonstrated above...

Just model each component as you desire on its own origin. Since component origins default to the main origin location whenever you create components, this will result in you have several components all stacked in the same space, with their bodies overlapping and sharing space. Not a problem...you just Ground one of them and then start Jointing the rest of them into their proper positions. It is wise, in this scenario, to use the visibility eyeballs to carefully control what you can see and what you are jointing to what, or else you may be likely to accidentally joint the wrong thing to the wrong thing, since they're all jumble in the same space before you get the jointing done.

[laughingcreek]

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@Anonymous wrote:

... So, if I have to make drawings of my 3 panel component it would be better to sketching each component based on its own origin, than use joints to join the components together. ..

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I don't understand this statement.  why would having to make a drawing matter for the origin placement?

[TrippyLighting]

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@Anonymous wrote:

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From what I understand from your comments I either chose the 'parametric design'-workflow or the 'origin'-workflow based on my future needs.

...

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The distinction that needs to be made is between a top-down design workflow and a bottom-up design workflow.

Top-down means you design the parts in place in an as-assembled state and is what Fusion 360 was originally designed to do. This is where the as-built joints can be very handy.

Bottom-up means that all parts are designed separately and then moved into place using "regular" joints.

These can be components designed in the same assembly file or external components that are linked or derived into a design.

Both can be done in Fusion 360 and as long as the timeline is enabled those designs are fully parametric.

[chrisplyler]

@TrippyLighting  Meh. Lame. Nothing lights up in your post.

[TrippyLighting]

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@chrisplyler wrote:

@TrippyLighting  Meh. Lame. Nothing lights up in your post.

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I had hoped the post itself would be somewhat illuminating 😉

[chrisplyler]

Yeah alright you get a pass for that. But you can't use it all the time!

[kb9ydn · Accepted solution]

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@TrippyLighting wrote:

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@Anonymous wrote:

...

From what I understand from your comments I either chose the 'parametric design'-workflow or the 'origin'-workflow based on my future needs.

...

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The distinction that needs to be made is between a top-down design workflow and a bottom-up design workflow.

Top-down means you design the parts in place in an as-assembled state and is what Fusion 360 was originally designed to do. This is where the as-built joints can be very handy.

Bottom-up means that all parts are designed separately and then moved into place using "regular" joints.

These can be components designed in the same assembly file or external components that are linked or derived into a design.

Both can be done in Fusion 360 and as long as the timeline is enabled those designs are fully parametric.

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Yes, I think that sums it up nicely.  If you're going to do a fully top down design the origins aren't really important.  For bottom up, you use the origins as the base reference for each part and then joint everything together.

You can still make a fully parametric design from the bottom up though, by using parameters to drive the critical dimensions instead of modeling in place.  It's more work to set everything up this way, but if you were doing cabinetry or such where you have lots of parts that are essentially the same, only differing in a few dimensions (length and width for example), it would make things easier when you need to adjust the design.

C|

[Anonymous]

Thanks all for the constructive answers. I do know the difference between top-down and bottom-up designing. I guess I was thrown off guard a bit by the "1-file"-workflow in Fusion thinking there was "magic mix" between the two 😀. My question is answered for now, again, thanks all