Configurations of model with and without shrinkage/sprues/supports

[fsergent3M8YQ]

Hi,

I am new to Fusion 360 (potentially switching from SolidWorks) so forgive me if I'm missing something obvious. I know Fusion 360 doesn't do configurations the way SolidWorks does. That's OK. Here's my problem. In Solidworks I typically use multiple configurations that track the item through the manufacturing process. That usually starts with a 3D print. The 3D Print is then used as a pattern for investment casting. Then the investment casting is post machined for dimensionally critical surfaces. So I start with the "final part" configuration and work back through the manufacturing process. The "final part" configuration is used in assembly files that use the final part. The "as-cast" configuration gets a little extra meat in areas that will be cleaned up by the final machining operation. The "pattern" configuration builds on the "as-cast" configuration by scaling up to account for shrinkage, gets sprues added, and maybe duplicates copies of the part on the same sprue that will get cast at the same time. The "print" configuration builds on the "pattern" configuration (maybe even more multiple copies) to add supports necessary for reliable 3D printing that will be torn away after the item comes off the printer.

Now, if I'm working with an assembly with the "final part" configuration and discover that I need a slight modification there, I just edit the part there (only once). That change automatically propagates all the way back to the "print" configuration which typically has multiple copies plus miscellaneous features to account for the full manufacturing process.

At this point, I see no way to do anything close to this in Fusion 360. Initially, I thought I could just create individual Fusion 360 files that each represent one of those Solidworks configurations and each include a linked component representing the previous step in the chain. Problem is I can't add features to these linked components without changing the item I'm linking to. For example, I want the "pattern" version to be scale up to account for shrinkage. How do I do that without also scaling up the "as-cast" version? I could make an unlinked copy, but then if I add a fillet (etc) to the "final" version, I will need to add that same fillet in every unlinked copy. So once I decided that wasn't going to work, I figured I could use the nifty branch/merge feature for this. Turns out that whole system is going away.

Is there anyway to accomplish what I need here? Am I missing something?

Thanks,

Frank

[TrippyLighting]

I believe that can be done with a method I call "Configurations (really) light". 

I described the workflow in this hand out for a Autodesk University class. Lok for the season called "Configurations light"

I'd very closely examine Fusion 360's abilities and limitations before switching from SW! 

This youtube video explains the effects of copying and pasting bodies and components in Fuiosn 360 in more detail:

[fsergent3M8YQ]

Thanks! The Autodesk University handout link was very useful in sending me on the right path. I have done enough experimentation to have confidence I can do what I need to do now as far as configurations and linked components. I have uncovered what seem to be two bugs in the software though. Maybe they are features so I'll call them features for now. Everything I do is timeline based, so please keep that in mind.

FEATURE 1: This is related to implementation of the configurations light structure described in the handout. The idea is that I start with an empty file and create a base body that I would like to branch off in several different directions. So I create a new empty component in the file to receive a copy of that base body and activate it. Then I right click in the viewing area and select Move/Copy which brings up the Move/Copy Panel which is set to the "Free Move" move type by default. I select the base body (only body in this case). So far so good. Now I want to just press OK because I'm not interested in moving the copied body - but the OK button is DISABLED. So I figure perhaps I need to check the "Create Copy" box in the Move/Copy Panel. OK button still not enabled. So I switch from the Move Type from "Free Move" to "Point to Point" and back. Now the OK button is ENABLED for some reason so I click it and I now have a copy of the base body in my new component. Then I can add any features in that component to "customize" the base component. So this component is essentially as configuration. Not following this sequence exactly has caused Fusion 360 to CRASH a couple of times (crash reports sent to Autodesk), but following the sequence gives me what I need. Cntrl-Drag body in to the component seems to work as well and is perhaps not as prone to crashing the software. My question was going to be "Is there a better way to do this?" I think I answered it myself. Cntrl-Drag seems to be the "correct" way to do it. This nice thing about this methodology is that I can go back in the timeline and change the base body and all configurations are automatically updated (this was a "must have" for me).

FEATURE 2: So using the method outlined in the FEATURE 1 description, I can create a single file with lots of components with bodies that each represent a state of a part through the manufacturing process. FEATURE 2 relates to using those components and bodies in my "base" file in other files. The base file has lots of components in it and I would like to make a component in my new file where I extract one of those base bodies that I'm interested in AND I would to maintain the link back to the original design so I get updates if they occur. So, I insert the "base" file into my new design as a component which maintains the link to the original file. Now I create a new empty component and activate it. I can find no simple way to copy a body in the linked file into my new component. Nothing seems to work. If you can figure out how to do this easily, let me know. The software seems to actively try to prevent me from doing that. Here's the trick I use: I create a body in my new component that intersects the body I really want from the linked-in component.  Then I can use the "Combine" operation to join the body in the linked-in file with the body in my new component. If I make my "anchor body" small such that it is completely encapsulated by the linked-in body, then my new component is exactly the linked-in body which is what I needed in the first place. Now I have a copy of the linked-in component body and I can do what ever I wish with it that is tied all the way back to the original design. Is there an easier way to do this? 

Thanks for looking!

[HughesTooling]

@TrippyLighting Does copying a body still break at times leaving you unable to fix the design? I've moved away from Copy\Paste and use Boundary Fill set to new component. If you make a change that breaks the design you can reselect the new body by editing the Boundary Fill.

@fsergent3M8YQ If you want to use Copy\Paste. Select the body, right click and select Copy from the menu, not Move\Copy from the marking menu. Then just select Paste, or just use Ctrl+C, Ctrl+V.

Mark

[HughesTooling]

@fsergent3M8YQ One more tip, Boundary Fill works on linked designs so it's possible to roll the timeline back, import a different design then select the body from the new design and continue the design using a different body.

Mark

[TheCADWhisperer · Accepted solution]

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@fsergent3M8YQ wrote:

... with bodies that each represent a state of a part through the manufacturing process. 

...AND I would to maintain the link back to the original design so I get updates if they occur

... Is there an easier way to do this?  

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Sounds like Autodesk Inventor Professional tooling and Derived Components.  By the time you figure out a robust technique in Fusion - should pay for itself....

[fsergent3M8YQ]

Thanks to everyone for the help here. I think this is going to work out just fine!

Frank