Would like to understand Dissolve Features better

[Oceanconcepts]

I kind of get it, but may be missing something...  

I would like to get an explanation of what Dissolve Features is intended to do- it seems that when I create an array or mirror, I can use this on one body therein if I want to be able to edit the duplicated bodies independently.  But I don't find anything in the Command Reference about Dissolve Features.  

The bodies still stay as part of the Mirror Group, or pattern in the browser. Is there a way to create an array when you want a lot of duplicate bodies, then dissolve the array feature, so you have a set of independent bodies not under an array folder? Is the solution to just drag the bodies to the Bodies folder of the component, then delete the Array or Mirror folder?

Ron

[innovatenate]

Ron,

The Dissolve Features option will remove any features listed in the browser and leave only solid bodies for a given component. I believe the intent is to provide this option so that the browser can be simplified. I suspect this feature will have more impact after parametrics are added to Fusion.

Here's what I tested.

1. I made a cube primitive via the Solid ribbon

2. I then created a pattern of this body

3. Last I right click on the part and choose dissolve features.

Here's a short video of the last step

http://screencast.com/t/ZSmilF18NYU

The result is that I'm left with independent bodies with no pattern feature in the browser. This sounds like what you are describing, but I'm not sure. I'm betting you're design is more complex than this simplified example and I'm overlooking something. Any light you could shed would be a big help.

Thanks,

[Oceanconcepts]

Nathan,

That's about what I was guessing, but I had applied this action by right clicking on a single body in the browser (i.e. one of the boxes in the pattern), rather than a higher level folder. This seems to leave the browser looking exactly the same- still showing the pattern folder, or mirror folder, but it does appear to dissolve the relationship for the entire group. My confusion was that the browser appearance did not seem to reflect this change. 

What is the distinction between this and Make Independent, and in what contexts would each be used?

Ron

[innovatenate · Accepted solution]

Within an assembly you can have multiple instances of a component. By instances, I mean that the component is exactly the same, if you change one component, the others will update with the same modifications. Usually, you see that components instances are marked by a colon and a number to note that they are same. For example in the browser you will see the names  BoxComponent:1, BoxComponent:2, BoxComponent:3, etc...

Make Independent breaks that link between the components. After you make independent fusion will automatically add a (#) to the name of the component. Following the Example, you will see BoxComponent (1):1. At this point, I generally rename the component to avoid confusion, but that may just be my own compulsions.

Here's a video that demonstrates.

http://screencast.com/t/PrYIGSHQ9Yq

Dissolve features happens at a component level, removing any features that make up a component: Extrudes, Shells, patterns, mirror etc. One last thing I'd like to add is that when patterning or mirror a component vs. a body/feature, the browser is populated differently. Patterning bodies or features places feature pattern in the component where as patterning a component will not add any features to the design, only more components.

Hope that helps. Please let me know if I can clarify anything.

[Oceanconcepts]

It's very clear, thanks.  Make independent is straightforward, and the name describes what it does.  Dissolve Features is a bit more obscure. What I'm getting is that the dissolve features is something analogous to clearing the history in a parametric system.  I've wondered why Fusion gives such a prominent place in the browser structure to the Features- extrude, shell, etc.  They can't be collapsed, take up a lot of room, and I'm not sure what I can do with them- maybe I'm missing something. It would be one thing if you could open and edit a feature- change a shell thickness, etc.  Is this looking ahead to parametrics?

Ron

[innovatenate]

Features will stay grouped with the bodies they are associated with. So for example, if you create a multi-body design with a handful of features, then convert one of the bodies to a new component, the associated features will move with the body to the new component. In this way, you can compartmentalize features with components can be used to condense the feature list in the browser. Or.. the "nuclear option"... choose to use the dissolve features if you don't feel like dealing with them. Or given the social aspect of Fusion, it might be nice to dissolve features to "discourage" collaborators from editing a specific feature. Kind of a way of saying this is done, don't touch it without having to state it. I'm getting off topic....

Here's a quick video to demo the features following a body to a new component.

http://screencast.com/t/AcCgCzXjts

I should note that some of the features are currently editable and some are not. I'm usually able to edit a fillet, chamfer or a pattern feature. Other features in the browser are not currently editable (i.e. extrude). However, sometimes they are nice to have around in the browser since they may be used in patternsand mirror features.

Components present one option for grouping features in the browser and dissolve features an option for disposing of them.  As far as the future I believe Fusion 360 will add more and more features that are editable post-creation (like the chamfer feature is now). Currently, the direct edit tools like push/pull, move, and delete face tools are available as the safety net if you find yourself needing to modify what is already in canvas.

Hope this is helpful. Let me know if there's anything I can help with.

[lure23]

Very nice explanation of the "component instances" way of thinking. Thanks.

I presume there is no "inheritance" concept in Fusion 360. Ability to i.e. make a prototype pipe somewhere, then vary individual properties in particular components. I.e. material choices could be coming centrally whereas thickness would be individual.

It'd be very akin to object inheritance in programming. I think it makes sense also in CAD - are there any products that do this?

To me, the development of CAD products is somewhat following developments in the software world, only with huge delay in time. In the early times (late 1960's) they went hand in hand. Engelbart's video comes to mind (programming and CAD seem interrelated in it): http://sloan.stanford.edu/mousesite/1968Demo.html

Then again, Inventor feels to me like programming. Partly the reason why learning to utilize it well takes so much effort.

Any thoughts on this?

[pfbreton]

In other products, this is called "collapse" or "flatten history"  Maybe the term disolve in Fusion need to be changed to something more obvious?

[jsejcksn]

I can't find "Make Independent" anywhere in the UI. How can I make a copied component independent? I have already placed it and created joints, joint limits, etc., so I don't want to re-do all of those things after creating a new copy using "Paste New".

I can't view your screencast because it requires Flash.

[Scoox]

"Dissolve" seems an unfortunate naming choice, all it seems to do is clear features from the browser. I don't get why features even appear in the browser at all, since they can't be edited. Also, certain features (e.g. moving a face) don't show up in the browser.