Does Fusion 360 allow you to edit a component in an assembly?

[Anonymous]

Hi Everyone,

I'm a student who is just getting into CAD modeling. I've been using Inventor to model parts for a robotics project and I wanted to edit a component in assembly mode. However, while Inventor does allow you to edit a component, those changes don't get saved to the part, so the changes won't appear on every identical piece. 

Does Fusion 360 allow you to edit a component in an assembly and save the changes to that component? 

Thanks

[sanjay_jayabal · Accepted solution]

Hi smh3005,

In Fusion 360, you can build assemblies with two different approaches,

1. All the components of your assembly created in the context of your assembly, so they are contained in your assembly - in this scenario, you can activate components and make changes to them directly in the context of the assembly.  You also have the ability to apply features to one ore more components in the assembly.

2. Components of your assembly are external to your assembly, so they are referenced in your assembly.  That is, if you "Inserted" components into an assembly from the Data Panel, you would have built them with this approach.  In this scenario,

    a) You have to open the component (that you want to edit) from the Data Panel, make your changes and save it.  

    b) Now, when you come back to the assembly, it will show you that your assembly needs to be updated for the change(s) you made (see below).

    c) Click on the drop down and choose "Get All Latest".

NOTE: in the second scenario, if all your components are external references, then you cannot apply features in the context of the assembly to them.

BTW, regarding Inventor, you may be creating assembly features instead of editing the individual components.  Assembly features are isolated to the assembly only and can apply to many components.  So, in Inventor, if you want to edit a component, activate the component in place in the assembly or Open it in a separate window to edit.

Hope this helps.

best regards,

[MACABItech]

What about, if in scenario (1), I want to make the component within the assembly a stand alone component. do i need to export the part and then insert this part that i've exported? Is there no way to convert an assembly component into a stand alone part?

Thanks

[TrippyLighting]

Yes, there is! "Save copy as" will export an individual componet or a subassembly as a standalone part into the data panel

That standalone part currentyl is not linked back to the originating assembly.

Before you start desinging you may want to chack out Fusion 360 R.U.L.E #1.

[MACABItech]

Thanks for the answer. I've been over rule #1 and adhere to it vehemently when I do create components inside of a design. However, what I've found myself doing is mimicking the workflow that I became accustomed to in NX. Let me explain:

I need components that are created in one design to be applicable to multiple other designs. This is because, sometimes, I need changes made to a specific component to be standardized across a family of designs in which that component is used. So for example, lets say I've designed a specific socket head cap screw with a slot in the tip to be used in design #1 and design #2, design #3, etc. If I modify the thickness of the slot in the screw that is used in design #1, maybe I need it to be updated across the range of assemblies in which that socket head cap screw is being used. In this case, I need the socket head cap screw to be a stand alone component in fusion360. In NX, no matter where I create a component (inside of an assembly, as a new file, etc), it can be inserted as a part (what in fusion is called a stand-alone component) in any other file. Any change made to that part will propagate across all designs that use that part. 

This works fine in fusion; if i know i am going to be using a part in multiple assemblies, I make it a stand-alone component. However, it is then impossible to modify that stand alone component from inside of its parent design. If I am making a unique set of parts that assemble to one another, then I keep them as components inside of a design, and I can make modifications to any of the components of that design. What I don't understand is why have this differentiation, why not make it so I can modify a component from within a design or by itself? Is it too calculation intensive or resource intensive to have this in what can be a free software?

I realize NX and Fusion are completely different softwares, and there are obvious limitations associated with the cost of the software you choose, but this one doesn't make sense to me because Fusion is so close to already doing what NX does. The only change would be to make it so that creating new components in a design also generated new designs in the folders, that could then be dragged and dropped into other designs to act as sub components in those other designs.

[TrippyLighting]

There are many current limitations that render the work with external components as not very efficient or effective. However, the functionality you are describing is being worked on and it's not a matter of the Fusion 360 team not wanting to integrate it. It's simply functionality that has yet to be implemented. 

While it's easy to verbalize it's not easy to implement properly 😉

[ToddHarris7556]

@MACABItech.... while on the surface, it's a simple thing to update linked components, it introduces a bunch of version control issues as well. 

To use your example - 

Say you use that socket head cap screw in several assemblies, and you went and modified the head diameter in one. Would that change break any features in any of your designs? i.e. hole sizes located next to the edge of a part, for example. In Inventor, when you insert a part from the Content Center, you have the option of either inserting as a 'standard' component (which can't be edited) or as a 'custom' component (which can be edited, but isn't linked to any other assembly). The intent is to prevent the issues described above. 

Having said that, I completely understand the usefulness of being able to link a part in, and activate it in place to edit without having to go out and edit it explicitly. I jump through this hoop probably 30 times a day and I wish it were a little more efficient - but there is a reason for it. 

[MrsOKeeffe]

Hi Peter

We have a file that is made in option 1 (everything seen as an assembly) and want to delete one screw.  But when we try to delete that screw - all screws that are the same delete as well.  How does this work with the process you have listed above as this looks like more to do with altering a piece not deleting it.

[jeff_strater]

@MrsOKeeffe - what are you deleting, a component or a body?  If you are deleting a component, only that instance of the component should get deleted.  However, if you are deleting a body, that will delete the one shared body in all instances, and all will appear to be deleted (the components will be there, but they will be empty of geometry).

Also, you can try Remove instead of Delete - this will put a Remove feature into the timeline that will remove that object for any later operations.

[MrsOKeeffe]

Hi Jeff

What I have is an assembly of a robot drivetrain (base) and we want to remove one screw from one area.  BUT - when we go to remove it deletes the screw from all locations not just that specific location.  We have the same issue when we are trying to modify one of the rails - modifying the front rail also does the same modification to the back rail.

Question - how do we delete a component over deleting a body (I am assuming this is what is happening at present)?

[MrsOKeeffe]

Ok.... we tried deleting it as a component and it deletes all of the pieces (the same). ... we also tried to remove on body and component - it deletes them all as well.

We do not have history on this file all the way to the start as it is an imported STEP file.

[jeff_strater]

If you can record a screencast of what you are doing, that would help.  Below is a screencast of a simple case that illustrates the difference.  The easiest way to delete a component is to select it in the browser.  If you select in the graphics area, you may be selecting the body (second delete in the screencast).  Because all component instance share the same geometry, deleting that body will delete it from every instance.

This is similar to what you are referring to here:  "We have the same issue when we are trying to modify one of the rails - modifying the front rail also does the same modification to the back rail."  Again, all instances of a component share the same geometry.  If you make a modification to one, it will affect all instances.  If you want a version of the component that is independent, you have to create it using "Paste New".  Select the component, Copy, then Paste New.  This will create an unassociated copy of the original component that can be modified independently

[MrsOKeeffe]

Hi Jeff

That does solve one problem of how to modify the piece but how do we delete a piece without deleting all of them?  

[jeff_strater]

I can't tell without more information.  Can you share the design and a screencast that shows me what you are doing when this happens?  In the screencast above I showed deleting an instance of a component.  Are you doing something different that that?  To share the design here, export the model as a Fusion Archive (F3D) and attach it to your post.

[jeff_strater]

ah, OK.  If a picture is worth 1000 words, a video is worth 10,000.  Did not realize that the component in question was one level down in the component hierarchy.  So, this delete is another flavor of the "all instances of a component share the same geometry".  In this case, "geometry" includes child components of a sub-assembly.  So, you have multiple instances of the same sub-assembly:

A sub-assembly is just like any other component - all the contents of this component is shared between all instances.

So, the solution here is the same as modifying geometry in a component - use Paste New to create a version of this sub-assembly that you want to be different from all the rest:

[MrsOKeeffe]

OMG - you have solved a two week battle to make this happen - THANK YOU 🙂

[TrippyLighting]

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@MrsOKeeffe wrote:

OMG - you have solved a two week battle to make this happen - THANK YOU 🙂

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Don't wait so long to post questions 😉