topic Re: Assembly help for a SolidWorks User in Fusion Design, Validate & Document Forum

Assembly help for a SolidWorks User

chris.sutanto28 — Wed, 29 May 2019 03:44:34 GMT

Hello,

I have about two years of experience with SolidWorks, but I recently moved to a small company that uses Fusion 360. I've used Fusion for CAM as I built a CNC router at home, but I'm not that familiar with the CAD functionalities. I’m having trouble understanding how multi-part designs work, especially since Fusion doesn’t deal with assemblies like SolidWorks does. Here are a few questions I have:

Can I work with assemblies like how I did in SolidWorks by creating separate designs for each of the components and combining them in an “assembly” design?

What is the benefit of creating all separate components in one file? If I were to create all components in one file, how would version control work if I made edits to all components but then decided to revert only one component? Would I have to revert the entire design or can you rollback individual components?

Honestly, it feels like I’m having more trouble switching to Fusion 360 than I did learning SolidWorks in the first place (I’m probably just getting a bit frustrated). If anyone has switched over from SolidWorks and has any good resources or tips for the change, they would be greatly appreciated.

Thanks

Re: Assembly help for a SolidWorks User

johnswetz1982 — Wed, 29 May 2019 10:05:29 GMT

I dont think there is any advantage to having all parts in one design. I use a workflow like your used to with one component per file then having a separate assembly file with the components linked to it. You do so by creating a blank file then going to your data explorer, right click a component and >insert into current file.

Re: Assembly help for a SolidWorks User

TrippyLighting — Wed, 29 May 2019 10:34:23 GMT

@johnswetz1982 wrote:

I dont think there is any advantage to having all parts in one design.

I'd have to disagree with that assessment! There are a number of caveats even gotchas when designing with linked components and not working with linked components is a much smoother workflow as you don't constantly have to manually update the assemblies where you use these.

In Solid Works (I've worked with SW for 15 years professionally) you make changes to external components in context, so you don't have tp perform any extra actions to "update" the assembly after you edited a component. That in-context edit does not exist in Fusion 360 which makes a workflow exclusively with linked components very slow, clumsy and frustrating.

Also, many things that you use often in a design like hiding/unhiding sketches, construction plans, bodies require a change to the linked component with manual update of the assembly and cannot be made just on the fly as you can with internal components.

Fusion 360 from the beginning was designed with a top-down design workflow and the still is is strongest suit.

@chris.sutanto28 are you familiar with Fusion 360's R.U.L.E #1 ?

Re: Assembly help for a SolidWorks User

johnswetz1982 — Wed, 29 May 2019 16:39:40 GMT

Having used Autodesk product for many years I guess I am just used to working in separate "reference" files and reloading/updating them whenever I am done. I just find it easier to keep everything separate than having one file jammed full of stuff.

Re: Assembly help for a SolidWorks User

TrippyLighting — Wed, 29 May 2019 17:49:48 GMT

@johnswetz1982 wrote:

I just find it easier to keep everything separate than having one file jammed full of stuff.

This is indeed easier when you keep separate files for each of your components, but until in-context editing is part of Fusion 360 feature set I find it cumbersome. But it also depends on what sort of "stuff" you design.

I develop mostly prototype and conceptual designs and for that I find that internal components allow a fluid workflow.

Re: Assembly help for a SolidWorks User

Anonymous — Mon, 10 Jun 2019 22:07:13 GMT

I'd also like to contribute here and say that missing in-context editing of inserted components is cause me real headaches when approaching a model of anything other than basic complexity.

In Inventor I'm able to reference surfaces in other components to create bodies and extrusions etc, this all works parametrically. In Fusion I'm forced to do the Top Down design flow, which after you reach 20 or so components it gets too cumbersome to work with - nevermind when I want to export these for CAM, and I loose the ability to parametrically update the component!

This really should be priority Number 1, over UI updates like toolbars. I appreciate the work so far on Fusion but it is too simple really for a 'real' product.

Re: Assembly help for a SolidWorks User

HughesTooling — Mon, 10 Jun 2019 22:34:09 GMT

@Anonymous wrote:

- nevermind when I want to export these for CAM, and I loose the ability to parametrically update the component!

For CAM you can use Derive and keep the link back to the main design.

Mark

Re: Assembly help for a SolidWorks User

Anonymous — Mon, 10 Jun 2019 22:40:37 GMT

@HughesTooling Thanks Mark I'll look into Derive.

How do you handle larger assemblies? Especially parts that need derived positions from other components which can be modified parametrically?

I have an example of using a Linear Motor which needs to be positioned +28mm X and +1mm Y from a point on a magnetic track - at the moment I am doing this with a Joint which works fine. Issues compound when I have two linear guideway carriages that also need to be positioned, and all these need to be referenced in a saddle that at the moment I'm having to keep all these components in one file - meaning I can't share these components between files, its driving me nuts!

Re: Assembly help for a SolidWorks User

TrippyLighting — Tue, 11 Jun 2019 11:14:00 GMT

Can you post that file ?

You can simple share ht public link to it from the data panel.

Re: Assembly help for a SolidWorks User

Anonymous — Tue, 11 Jun 2019 11:39:27 GMT

Sure Peter you can find it here.

Any advice on how to structure assemblies would be appreciated - at the moment I'm thinking of abandoning Fusion 360 and going back to Inventor, despite Fusion being easier to use for sketching and general modelling, especially with the CAM.

https://a360.co/2I6R0GK

Re: Assembly help for a SolidWorks User

TrippyLighting — Tue, 11 Jun 2019 17:17:50 GMT

The structure of your assembly looks fine with the exception of several instances where you have body at the same structural level with another subassembly. Form an assembly standpoint his will work, but it might it difficult to create a proper BOM.

Carriage is an assembly so you'd create an assembly drawing with a BOM. That BOM would only include a subassembly called fasteners. It would not include the carriage as a part.

I'd need to understand what exactly the difficulties are you are encountering.

If you can create a narrated screencast that might help.

Re: Assembly help for a SolidWorks User

Anonymous — Wed, 12 Jun 2019 20:36:04 GMT

@TrippyLighting

Thanks Peter, I was attempting to keep the Body which I need to machine in the root of the Component for example Carriage.

Looking further into organising assemblies I've tried this Master Layout pattern which I have created a portion of my model in, as well as change the Body's to be their own components. I've included dependent components on each part in their file (fasteners for each component for example).

This is getting me closer to in-context editing, as at least I can reference geometry I need, at the moment I have to know I will need it later on. I can go and add it to the Master sketch afterwards, but this would be a pain. But now I'm thinking I should have created a Root type Master Layout Component that I can draw off, and make Sub Master Layouts Components that come off this.

For example, I have some 8020 extrusion which these assemblies are mounted on, I don't want to put these in the YAxisAssembly, as they are siblings rather than Parent/Childs of those components. Deciding how to structure this type of machinery is likely a one time task, that once a good pattern can be shared it will save a lot of headaches for people using Fusion.

Re: Assembly help for a SolidWorks User

Anonymous — Wed, 12 Jun 2019 20:40:18 GMT

Link: https://a360.co/2X9am6q

Re: Assembly help for a SolidWorks User

TrippyLighting — Thu, 13 Jun 2019 01:43:18 GMT

I only see 2 sketches. One in the assembly and one in the linked components. No geometry ? Is that it ?

What exactly do you want to do ?