Replace component with another component

[schengnz]

In large assemblies, it is common to include one or more families of interchangable parts. It is very useful to be able to switch from one of these parts with another in the same family, for design experimentation or to create a product family.

Autodesk Inventor allows a component in an assembly to be replaced by another component, which serves this purpose very well.

Fusion 360 is sorely missing this feature, only allowing a component to be replaced by a different version of the same component. This effectiovely means it is impossible to try out a design using different parts in the same part family, and makes it far more difficult to test out different design variations, or to create product variants..

[lucasproko]

Hey all - I wanted to give an update on this issue because I understand it is an important one for all of you.

A Replace Component feature is a relatively straightforward operation in many bottom-up design softwares because it occurs in Assembly files where you only really have to worry about re-associating the joints/mates/whatever other assembly constraints you have in the design. However, since Fusion doesn't have the concept of an Assembly file, and all designs can be modeled top-down as well, it makes it much more difficult to replace a component because there are many more types of references we have to worry about. For instance, not only would we have to re-associate all joints, but we would have to re-associate all sketches which may have used a face on the old component as a sketch plane, all projections in other sketches throughout the design that may have referenced the old component, all construction geometry that was based off the old component, all commands that may have used part of that component as reference (Extrude To extents, etc), etc. 

Without the ability to re-associate all of those, a Replace Component command would blow up your timeline. The good news is that we've recently started a project to help you Re-associate sketch projections which is a step towards this path, but the bad news is this is still a very difficult problem to solve and it will take considerable time before it becomes a reality.

Thank you for your patience and your constant feedback.

[matt.soule]

I have worked out a solution to not being able to globally exchange a inserted component and it didn't seem to be posted here so at the risk of duplicating someone else's post, I guess I will submit mine. This is the solution I came up with to exchange identical inserted components in an assembly. Well it's not really a solution - it's more of a work around. It does require up front steps before you insert a component into the current design or download a component from mcmaster.com so you need to do this setup first if you think a component might be globally replaced later with a different component. You could just do it for all inserted external components just in case but it is a little extra work during the initial component insertion plus a few more steps to keep track of.

The general idea is to first create a parent component that the external component will be inserted into. All the geometry from the inserted component that is required for down stream model construction has to exist in the parent component. When the inserted component is replaced with another, some of the links will break or disappear and will have to be reestablished but you will only have to do this on one instance. You will not need a very large assembly or many instances of the component before this method will be a quicker alternative to rebuilding the model or replacing instances individually.

Here are the steps.

* Create the parent component. Modify the properties and material to match the component to be inserted as this will be what is displayed in the parts list.
* Insert or download the external component into the parent component. In most cases you do not want to move the inserted component as part of the insert command. This should be done to the parent component, if necessary, later.
* If the inserted part will have other parts jointed to it or geometry constructed from it's features construct the required planes/sketches/joint origins/geometry and make sure they are in the parent component, not the inserted component, even if they must reference the inserted part geometry. Note that by rolling the history back to this point more construction/jointing geometry can be added later if necessary.
* Create a rigid group of the parent component and include children.
* Use the move command on the parent component to position the parent and inserted component if necessary to aid visualization.
* If the inserted component is the first part in the assembly ground the parent component. If the component is to be jointed with another, joint the parent component using geometry in the parent component. Note this goes for the other component as well if it too is inserted.
* When you want to add another instance of the inserted component , copy and paste the parent component and joint it as desired using only the parent component geometry.
* If you want to replace the inserted component with another different inserted component, roll the history back to the insertion point and delete the inserted component. Insert the new component within the parent component. Replace the rigid group which disappeared.
* Reestablish the links from any planes/sketches in the parent component related to the inserted component geometry required for the downstream construction. Change the properties of the parent component to match the new inserted component.

All inserted components should now be updated with the new inserted component, all should be placed properly and all downstream geometry manipulation should conform to the new inserted component. Note once again how important it is to only use the parent component geometry for jointing and downstream construction in order for this to work.

I have up loaded a the file showing the construction process. Not sure how it is going to appear with the external references.
https://a360.co/2N3s9mb

I also made a screencast of the replacement steps.
https://autode.sk/2QXNS2c

Also a expanded view of the inserted component in the browser.
https://a360.co/2OSsjP4

Hope I did that correctly.

[Anonymous]

I can't even comprehend why this would not have been implemented from the get go. It's some basic functionality. Hopefully we'll be seeing a video of Lars showing us how cool the new replace component feature is soon.

[Anonymous]

ive just moved over from Inventor and this I’m really missing this functionality.

It makes the design development process so much simpler.

[dirk.leipold]

For the replacement feature it would be useful to have a common reference sketch (physical interface definition) used for all replaceable parts

[Anonymous]

Thanks for considering this feature. It would be incredibly useful. I use it often in SolidWorks and it is a huge time saver. In response to Lukasproko, I'd like to share a couple thoughts.

1) Implement "replace component" only for components that don't reference any sketches in the component that is being replaced. Joints would be allowed, but nothing else. Once this feature is available, it would satisfy the needs of many users and you could then work on expanding the capability of this feature to include re-associating sketch projections etc. You often do incremental feature introductions and enhancements, so this model would fit will with your release history.

2) Solidworks has "replace component" capability even though you can use parts in-context like Fusion 360. Yes replace component sometimes causes problems, but the problems are usually not terribly difficult for the user to fix. Good explanations of the problems and guiding the user to re-select problem planes, sketches, etc. helps make it even easier.

[adamwoster]

One more user adding a comment...please implement soon. Simply replacing 2000+ pan head screws with flat head screws has suddenly become an onerous, possibly deal-breaking task.

As I've discovered from being a part of some user studies...I'm in the minority as a professional user of this software. However I hope it carries more weight when I comment, as Fusion's functionality directly effects my customer's and my bottom line.

[Anonymous]

This feature would be an absolutely great add, for so many reasons. I constantly run into a situation with the need to replace fasteners for different sizes (typically use McMaster to insert fasteners). Takes forever to replace a couple handful of screws compared to a couple clicks with the replace command many of the other CAD software's allow you to do.

[jwatte]

It's four years later and I still can't find the menu item.

I realize that sketch links will break, but now there's the "re-associate geometry" option, so that would be a reasonable workflow for me.

[Anonymous]

Don't know if meanwhile someone found an alternative solution, but to change multiple bolts at once for example from M4x5mm with M3x20mm, or add a nut for example, i found this solution:

multiple M4x5mm bolts1. select one of the components (in this example "short bolt:1") and make it active

2. while inside the "short bolt:1" component, insert the new wanted bolt (example M3x20mm), and hit OK

insert the new bolt

3. right click the "body:1" from the "long bolt:1" component and select cut

4. hit escape key; then right click on a empty space and select paste; click OK on the menu, without moving it. like this, we made the body of the long bolt part of the short bolt component.

5. delete the "long bolt:1" component inside the "short bolt:1", and hit OK on the warning message that appear.

6. align the new long bolt with the old short one as needed. If necessary, ground the old short bolt.

7. delete the "body:1" of the short bolt.

If needed, you can add additional parts (washer, nut), as long as they are bodies inside the multiplied component.

I didn't test this workaround to see the behavior when joints are involved, but i think it could be usefully.

Cheers!

[jboerhout]

The original request for this feature was 6-25-2015. Now more than 4 years later ... no implementation - just gathering votes. This is extreme!

Why implement new toolbar behavior, colors, buttons etc. but not have a fundamental feature such as component replace implemented?  Yes yes, I know all about your roadmaps and other features/functions taking priority (somehow), but 4 YEARS, come on!

[nshankins21]

Has this been implemented yet?  I take it from the last post that it has not.

[Anonymous]

This is needed !!!  How soon can we expect?

[Anonymous]

I have posted regarding this issue before.

The replace command or some type of work around is desperately needed.

I have a family of products that I am designing were the difference between assemblies within the family are minor.

Up until this point I would try to use save as and replace for when similar new details are to be added to the assembly. This seemed to work well but is limited. I need to be able to replace a detail in the assembly with a already created detail from another assembly while maintaining as many links as possible. The detail I want to replace with was originally created from another assembly using the save as and replace command.

Does anyone have a work around that will not loose the component links?

Can you also update us on the status for having something in the works?

[matej3TURY]

As for the others, this is a major missing feature for me...

I understand this can be problematic due to the top-down modeling possibility, but why not allowing the following?

• 1) create a copy of an assembly (already possible)
• 2) select a component within the assembly and use "Save as and replace all instances", or even better "Save as and replace selected instances" in case only some of the component instances should be replaced

We already have an option to "Save as and replace" a single instance of a component, so adding this feature cannot be too difficult...

Are we really asking that much?

[Anonymous]

I agree, this is an important feature

[Anonymous]

I am facing the same problem and dont know if this method helps.

Suppose you got an "assembly file" referencing Model A v.1, then you got a revised Model A v.2 on hand(not referenced by "assembly file").

1) Export the Model A v.2 as .f3d file

2) right click Model A v.1 and select "Import new version"

3) upload the Model A v.2.f3d just prepared.

4) Update files by clicking "Get all latest" command in the "assembly file"

This solution is OK for me(A rigid joint still remains as I replace the model in "assembly file") but it may bring file consistency problem(You can import totally unrelated model as new version of a model) and the model history is building up.

[Anonymous]

@lucasproko Like you said a year back, this is a complex task. Is there a rough timeline for this feature or is it still too early in the process to give an estimate? 

[mrm1018]

I just figured out this feature is missing...too bad.  4 years is a long time to wait for some of you.  I'm fairly new to using Fusion 360 consistently.

Solidworks sketches in an assembly referencing a replaced part would blow up too.  No way around it.

This seems like paralysis by analysis.  I say you let the sketches blow up.

[micromelt01]

I'm guessing there is another reason why this very basic feature that we have all used in other programmes has not been implemented after 5 years of requests. Perhaps it can't be done or they don't give a ****.