Fusion 360 Copy & Paste Components Locked Together

[Anonymous]

I'm trying to learn Fusion 360 and one thing really has me stumped.  I've created a component.  Then I right-clicked on the component in the object browser and selected "copy" and then "pasted" the object into the top level of the browser so that I now two identical components in the same level of the hierarchy.  However, I need to be able to move each object independently in order to position them.  When I use "move" on one object to try and position it, the other object also moves.  I can't figure out how to break this relationship.  I'm sure there's some simple thing I need to uncheck but its not jumping out at me.  Why would this be default behavior for a copy of a component?  It seems odd.

Thanks!

Ian

[Anonymous]

Thanks for the solution Jole, this was driving me crazy.

[alex8RFDS]

Hí,

I am totally new to 3D design and Fusion 360. Watched a few Webcasts and things start to go. But this one is driving me crazy. I just don't get the principle behind it.

Here is what I do:

1. Start a new and empty design
2. Add new component
3. Create a box as part of the component
4. The body is clearly within "Component 1:1"
5. Right click on component
6. Choose copy 
7. Right click on "(unsaved)"
8. Paste New
9. In the upcoming "Move" dialog click component
10. Move it by 100mm in X direction
11. Activate "Component 2:1"
12. Right click on the copy and choos "Edit Feature"
13. The copy disappears and I can edit the shape at its original position
14. After I'm done it seems to work

I had several attempts where actually both shapes were changes. It seems that I have some major misconception of what Fusion 360 is all about. I would have expected that I can change the copy.

Any help highly appreciated.

Cheers Alexander

[Anonymous]

I'm having the same problem.  Copy one component, paste into the parent component and Make Independent doesn't exist.  All copies from Paste or Paste New just replicate any change to the original component or any copy.  Paste or Paste New is grossly misnamed.  Paste should be called "Clone and Link".  And a basic Paste function does not exist.

From reading the thread above it seems like the Fusion team intended the Paste New to mimic the functionality of what normal users would expect from a Copy/Paste operation.  But there's a serious bug in Paste New and it just does the same function as Paste.  It's the same as if Excel had a bug in "Paste Data" and it functioned the same as Paste without any way to just copy data across 1000 cells.

Why doesn't Autodesk just fix the Bug in Paste New?  Surely they can see the benefit of having a working Paste New function?  This thread is 2+ years old and the bug still exits.  Why?

Normal Non-Autodesk developers usually expect "Paste" to function similar to how Copy/Paste would work in MS Word or Excel or SolidWorks.  Just a data copy, unlinked in any way.  But the linking causes all kinds of confusion and making unlinked copies is basically unattainable for non Autodesk developer users.  100 of 100 users would never expect to go into Excel, copy and paste a cell 10 times and have the 10 cell copies linked to the original cell formula without any way to break the link.  It's just creates frustration and wasted time.

As a user, the effect is any potential powerful benefit to having linked copies is more than negated by the current behavior of Fusion 360.

If I make a table with 4 legs, I have to make 4 separate components and draw each of the features 4 times on 4 independent legs.  What a pain in the back side.

For stuff that has repetitive components I end up using Solid Works - all because Copy Paste doesn't work in Fusion 360.  I would also use Word Perfect 6.0 if MS Word Copy/Paste didn't work.

I understand there is some power behind how Fusion does this Copy /Paste business, but if users can't figure it out and there is no instruction - it effectively cripples the product.

Maybe if there was some tutorial or video on how this Copy-Paste/Paste New/Make Independent complexity is supposed to work.

As it stands right now, regular, non-Autodesk developers have to just draw the same component over and over.  Or use Solid Works.

IMO It's crazy that a product as good as Fusion can make it to 2017 and Copy/Paste doesn't work intuitively like every other application on the desktop.

This may be a textbook case of developers creating "features" that they dream up and noone else can use and it ends up sinking the product - kinda like Pandora and their crazy rules vs. the simplicity of Spotify.

[Oceanconcepts]

Can you be more specific about how you are trying to trying to paste new? That would help us to understand where the issue is. From where are you selecting the component you want to copy? Are you selecting the whole component by double clicking on a body in the drawing or by selecting the component from the browser at the left of the screen? Lots of confusion to those new to Fusion stems from the logic of components vs. bodies, activating components, and other such interface elements that are unique to Fusion. This is all very powerful but it differs from how other programs are organized. A screencast or even some screen shots would help. 

There should not be any reason you would need to draw four table legs as individual components. Paste New should create a non-linked copy if that is your goal, or a simple Paste would create a copy that is linked to the others but can be moved independently, so you could do edits to one and it would alter all of the others. Fusion’s developers could have chosen to call the commands “Paste Linked” and “Paste”, but as is the Paste command gives a linked component and Paste New a copy that can be edited independently. 

I assume you are in the history based mode? Paste Independent doesn’t exist in the history based workspace, only in Direct Modeling. In direct modeling you can un-link a component after the fact, that isn’t possible in History based modeling. 

[Anonymous]

I am also new to F360 but have a lot of experience(30+ years) with many other windows apps.  and, I find this cut and paste behavior very baffling.  I understand there are lots of complexities here that most apps don't have.  and, there is a need for multiple choices of behavior.  but, the *default* behaviors for cut and paste, ctl-c,ctl-v, have semantics that are utterly different then common windows UI design guidelines or any other windows app on the planet that i'm aware of.  I think this is a real source of confusion. I would like to see paste be normal windows paste and F360 special behavior get a new name.  but, perhaps F360 has been around long enough that it's too late to change this? or perhaps a preference setting could be added?

I started with 1 simple 2-d sketch and 1 simple extrusion body.  what I really want is the ability to copy a sketch and make a variation of it. but, I understand that doesn't exist 😞

so, I made a new component 1 and moved the top level sketch and body into it.  I then copied that component into component 2 using 'paste new' after finding this thread.  I can now rename the body and sketch design tree nodes in component 2 without affecting component 1 which I couldn't do before with regular 'paste'.

the problem comes when I try to delete the body in component 2 so that I can edit the sketch and recreate the body differently.  if I right click on the design tree node for the body in component 2 and choose 'delete' from the context menu or select it and press the delete key from the keyboard, then I get an error dialog saying this component is referenced by other parts of the design. am I sure I want to do this? and, if I say yes. it will delete the body out of both components.  this really seems like a bug to me.

I believe this because, if I undo the unwanted delete and get both bodies back and then click on the component 2 body in the 3d graphic view(as opposed to the design tree) so that it's highlighted in color and then right click on that and select 'remove' from the context menu there then it deletes the body from component 2 without affecting component 1 just like I wanted.

but, maybe this isn't a bug and there's some 'zen of design tree' that i'm not understanding yet?

thanks

[Oceanconcepts]

I don’t think you are going to get the “normal Windows paste” behavior you are expecting, except sort of in direct modeling. The parametric environment needs to keep track of relationships in copied and pasted components, and it’s necessary to specify how you want that done.  When, where, and how you create the original sketches and bodies has a lot of bearing on how they behave later in the process. 

In general it’s best practice very strongly recommended (it will help keep you sane) to first create a component, activate it (automatic when first created), and only then create your sketch and extrusion or other added features within the component. Copy and "paste new" at the component level. You will then be able to delete the body in the 2nd component without warnings or effecting the body in component 1. Moving a previously created sketch or body into a component is not necessarily the same thing re. the timeline. 

This class Peter and Jeff put on at AU has some great insights into managing parametric workflows. Towards the end is a section on error messages. 

http://au.autodesk.com/au-online/classes-on-demand/class-catalog/classes/year-2016/fusion-360/pd2070...

[Anonymous]

Fusion 360 is completely baffling to me as a new user.  Normal computer commands are baffling and non-intuitive, not just copy/paste, but moving items or copying from one drawing to place in another.  I created a model and have a extruded part.  Now even when I select the part I cannot move it or copy/paste.  I can delete it and start all over.  I can't seem to figure out re-sizing either or moving one side of the extrusion. 

I am super new on this, but not new to PC or programming.  The program seems counter intuitive.  I am sure there are lots of people with an answer to these commands or issues, like the vide above, but geez a simple select/copy/paste using standardized PC/Mac commands would be so much easier.  This is likely not so much features but limits on how the program was designed and perhaps not wanting to alienate the users.  I may only give this a bit more time, but honestly I don't want to have to do 12 commands to do something fairly easy.  There should be no reason in 2017 to have to re-learn and re-think PC processes and commands to get to do simple tasks. 

I may get flamed here, and that's okay.  If Autodesk really wants to grow their user base they really need to re-think how their system acts.  I understand that there are some things built in that have to function a certain way, but I just don't see how you would need 4 years training to get going on the most basic designs. 

[Oceanconcepts]

There are (generally very good) reasons that Fusion’s interface works the way it does.  If you are new to 3D CAD and parametric modeling, you can expect to have a significant learning curve getting started, regardless of the program. Fusion is, in my experience, far easier than most powerful CAD applications for new users. But if you are used to working with other types of applications you may find old habits need to undergo some reeducation.  Think of it not so much like learning yet another PC application, but like learning an entirely new language. 

Copy-Paste is possible using standard keyboard commands, I do it all the time- but it matters where you copy from, component or body or feature, if you want to have the copies linked, and if so  in what way. It can’t be as simple as in a “normal” PC/ Mac application, or as in graphic apps like Photoshop or Illustrator.  Parametric modeling- the timeline- introduces yet another level of power, and also requires greater understanding of workflow options and their implications.

You may find if you are new to 3D CAD that working in the direct modeling environment will ease the learning curve. Right click on the root component and select “Do Not Capture Design History”. Many simple designs don’t really need to be done in a parametric environment. 

The video above is really for intermediate users, working through some of the tutorials and getting started exercises would be better if you are new to CAD. If you have specific questions or examples, post them here and you will get help. This community is incredibly supportive. 

[Anonymous]

I wrote a lengthy response with additional questions and info, but not seeing that now. 

Anyway, if it does post, I wanted to add that why is it when making a hole the program doesn't detect the thickness of the item you are making a hole into?  The hole should be made to the thickness as a default IMO, instead of trying to resize it, and only need to resize if the hole does not go all the way through.  For example I have a part t hat is 2 inches thick and need a 1/4" inch thick hole, it should make it exactly 2inches thick and not some other size that has to be resized.  Maybe there is a preference check for this, I could not find it, and found it cumbersome to have to do extra clicking to get the hole the right length. 

[Oceanconcepts]

I don’t see you longer response here (moderated? it was kind a rant), but I did receive it in an email so I will try to quote parts and address some of your questions. 

I Came to 3D CAD many years ago with a design background, but not so long ago that I can’t remember the frustration in dealing with a new environment. While I appreciate the level of hair pulling this can engender, seeking to understand WHY things are done the way they are, and HOW you can accomplish your goals, will be more productive than ranting about how Fusion has it wrong. Ask specific questions, and ask for help, before you condemn the program.  There are reasons, generally very good ones, for why Fusion, including the UI, works the way it does. There are things that could be done better to help new users, and questions help identify some pain points. Working through some of the getting started tutorials, particularly if you have no previous CAD experience, will shorten the learning curve. Jumping into a specific design and expecting things to work the way 2D design applications do will create frustration. 

It’s my experience that the biggest stumbling blocks for new users is failing to understand the distinction between components, faces, features,  and bodies. I expect this is at the root of your copy-paste questions. Work on understanding this and many quirks will start to become clear. 

I’m not sure what you are referring to specifically re non-standard UI, some menu items are in different spots than might be expected- I think this might be  more a reflection of the cloud and eventually browser interface than anything else-  but standard keyboard commands work within the bounds of maybe having to understand additional context to get the expected results. Nothing about those interface elements inherent to C programming, they are conventions of the Mac or Windows OS, adhered to with greater or lesser fidelity by developers. 

Specific to some of the issues I had was first in importing a basic 2D design from CorelDraw that I saved into dxf and dxg extensions.  Neither could be "inserted" (why it is not called imported also baffles me) properly, and I finally had to insert the drawing from an SVG save, which then somehow made it 10 times larger (not sure why).  

re. import vs. insert, I think the general use in Fusion is that Import means getting an outside file into the Fusion environment, into a project, so it can be utilized in a Fusion design. Insert means to take a component and insert an instance of that component into a particular Fusion design. In many cases designers will reuse components in different designs. The terms are distinct, I suppose somewhat arbitrary, but I think clear when you understand the distinction. 

re. Corel Draw importing, again, looking at the file here could help. DXF should import into Fusion just fine, as a sketch, but some particular designs, particularly if they use types of splines, will not be CAD friendly and may fail. That’s a case where looking at the file will probably yield an answer. Not all design applications will provide good data for CAD import. SVG is tolerant, but less useful in some ways on import. 

I found a similar item part that I wanted to design as a 3D model, and was able to bring into Fusion 360.  I had my 2d design, which I extruded easily, and made some changes.  I wanted design and the imported item design and though it would be great to "select" a part from the 3D model, do a simple copy/paste, and bring the part into my drawing that way I don't have to design it by hand.  Can't do it.  Just doesn't.  I can select the part, but no real way to copy.  I RMB and click the move/copy but nowhere do I find a past and CRT+V (again simple C++ programming commands) will do nothing, so I'm guessing there is no paste, at least in my sketch view.  I am in MODEL BTW.  

I’m not clear here if you are trying to copy-paste into another Fusion drawing or some other application.  Move/Copy is not the right command for this, that is for moving features, faces, bodies, or components depending on what you specify in the dialog. There is a distinct Copy command if you select something where that is an option, such as a component.  If another Fusion drawing, I suspect the issue is in knowing what you are selecting to copy. Is it a face, a body, a component, and are you selecting it directly in the drawing or in the browser tree? All of these options can yield differing results. But yes, you can copy-paste components between Fusion designs. It's best to do that from the browser tree.  If the component is something you want to reuse again or reference, it’s probably best to RMB on it in the browser tree and select “Save Copy As…”, then import into the 2nd design. If you are talking about copy-paste in reference to copying a sketch, that is not possible in the parametric/ history based environment but you can do it in the Direct Modeling environment. In the parametric environment sketches are much more tightly bound, of necessity. 

Similarly frustrating is the lack of being able to copy/paste simple items.  My design required several holes.  Easily found the hole selector and made a hole and adjusted the length of the hole so it goes through my part - easy.  Wanted to copy/paste the hole 3 more times since I need a total of 4.  Can't do it.  Had to design each hole manually. 

This is a difference between CAD and visual design programs. A hole is a feature that contains a lot of information. If you want to create more of any such feature, Fusion provides a specific tool- Pattern- to duplicate holes or other features while preserving the data integrity. There is no need to recreate individually. In the modeling environment and you want holes that are not in a regular pattern or regular sized, the best path might be to create what you want in a sketch and use extrude. You can pattern sketch elements as well. There are many ways to do things in Fusion, the best path will depend on your goals. But Fusion, nor any other CAD application, is not going to work from a UI perspective just like a 2D drawing or design application. 

The direct modeling environment gives a somewhat greater degree of freedom in moving around elements freely- It’s where I usually develop ideas. You may find it easier to get started with.   

Anyway, if it does post, I wanted to add that why is it when making a hole the program doesn't detect the thickness of the item you are making a hole into?  

It does, if you tell it to- but that's just one option. The Hole dialog that comes up allows you to specify a simple through hole as one of the options. There are many different types of holes. If you specify an "extents" hole it knows to stop at the extent of the body, even if another body is adjacent. If you are fastening several items together or want to drill through several in the same location, a common issue, the "distance' option will locate the hole on different bodies or components. 

I have several 2D designs in Corel that I want to bring to Fusion for the ONLY reason that I need to export files to someone with a CNC machine.  I don't do this for a living (CAD design) so I am not going to invest hundreds of hours to locate copy/paste or other simple functions, but was hoping that it would not be such a steep curve in learning the program's functions. 

Fusion is one of the easer applications to learn for someone wanting to do what you describe- get a precise model for CNC. Plenty of people here have picked it up rather quickly, and done amazing work. Rather than looking for the copy-paste command you are used to, ask here “how do I…”  and include screenshots or files. I think you will find things start to make sense.

[Anonymous]

Thank you Ron for the answers. 

One specific task I want to do is take a part from another drawing (let's call it drawing #1)  that I opened in Fusion 360 and copy it to my new drawing (drawing #2) because it is a common part/item for my type of drawing - a type of extruded hole for a guitar pickup. 

I do not know how that drawing #1 was created (program type) and I did import it into Fusion from the step file.  I'm not at my PC with Fusion but can provide screenshots if needed.  I guess the question lies in the following:

1.  Drawing #1 imported from a step export file

2.  Drawing #2 created from a CorelDraw file - it did have splines due to the curves.  This file could be opened in Fusion only from a SVG.  Actually the DXG version could be opened as well but would not extrude, but the SVG version worked. 

3.  Want to take a part of the Drawing #1 and copy/paste into Drawing #2. 

Ron I appreciate the comments, and will look at further resources online as well to learn the nuisances of the software and CAD in general. 

[daniel_lyall]

@Anonymous Up load your file that you are trying to use copy and past on and you will shown how to do it on your file and the file can be checked for problems at the same time.

Go to File -> Export and save as a .F3D Archive File and attach it to your next post

What you wont to do is quite easy once you know how to do it.

[Oceanconcepts]

Is the Part # 1 a solid? If it’s an .stp file I assume so? If it’s a hole would this be something you would subtract from your Fusion design to create the hole? A screenshot or design file would help clarify. Once you have it in Fusion just save the design and you would be able to import it as a component into any future designs. 

Your drawing #2 would be a sketch? Or have you made a solid from the sketch? Splines from some drawing programs frequently come into Fusion as many small segments, which may not be connected properly to form a closed profile. That’s very likely why the DXF would not extrude. Often the best thing is to bring in a picture of the object (or the SVG or DXF) and treat it as a canvas so you can sketch the splines from within Fusion’s sketch environment. 

At any rate, you can copy and paste components or bodies between drawings by selecting the component or body in the browser tree and the Copy command I pictured above, then Paste in the other design. Standard keyboard commands work for Copy, but not for Paste New if you want an unlinked copy in the same design.  Options are all hinted in the menus when you RMB. 

Or, if drawing #2 is saved as an independent design, select it in the Data Panel, RMB, and select insert into current design. Note that this will bring in a linked copy (chain links showing in the browser tree) that will not be editable within drawing #1 unless you RMB and select Break Link. You would then be free to delete unneeded parts. 

But if your drawing #2 is a sketch, and you are in the parametric environment, you can’t copy it by itself. You can, however copy the component in which it is located and paste that. Or use the import strategy above. 

Selecting parts in the drawing directly can be a bit confusing for a new user- it’s possible, but the options can be daunting.  For instance double clicking selects an entire component, while single clicking typically selects faces, edges, or vertices. In some tools where a particular selection is not possible it will default to body or component, and some tools require you to specify which level you want to use for an action in the tool dialog. For that reason I think getting used to selecting, bodies or components in the browser tree rather than the drawing will help to eliminate confusion and reenforce the distinctions between these parts of the design. 

[ericbrowning]

This is the dumbest and worst part of an Autodesk UI.  We should be able to copy/paste bodies or components as new independent objects without having to jump through this weirdness of pasting in open space vs. not being able to do it with the move command.  Totally counterintuitive 😞  Yes,

---

@Oceanconcepts wrote:

You need to copy the component first, deselect it, then right click in the workspace to get the marking menu. You should see options to Paste or Paste New. If you had used Paste and therefore had a linked component, you  could RMB in the browser on the component and select Make Independent. 

---

this nonsense still exists still in version 2.0.2938

[Oceanconcepts]

You don’t need to paste in open space, you need to click in open space, i.e. not selecting anything, to access the marking menu.  The marking menu is the standard way in Fusion you access a contextual menu of commands- including Paste and Paste New. You can also use the standard keyboard shortcut to copy/paste, control / command- C or V, but Autodesk needs to be able to differentiate in the interface between pasting a linked copy- the default behavior you get with the keyboard shortcut or a simple paste- and pasting an un-linked copy, “paste new”.  The pasted component will appear in the same position as the copy-from component, with the move option active. 

Since linked copies are quite normal and useful in CAD work, this seems like a reasonable way to structure this set of commands, with preserving the linkage being the default. Once links are broken, putting them back is problematic. One way to copy, two options for paste. If you want to Paste New a series of items, just access the marking menu again and the option to repeat the command will be at 12 o’clock. And there is a way to un-link if you need to. 

Is what you are looking for the kind of Option-Drag to make an independent copy that exists in some graphics programs? 

[ericbrowning]

No, just the option to paste and paste new in one single menu (for bodies and components) instead of hiding this function into a totally obscure method of pasting.  There are commonalities in all programs, this is not one of them.  Autodesk has a bad habit of trying to outsmart the user with it's UI design and how it's programs work (123D had all sorts of weirdness) and it only causes extreme frustration for new users.

[Oceanconcepts]

I'm still not understanding- isn't this what we have here when you access the contextual menu? This appears any time you have copied something. 

[ericbrowning]

Do you see "Paste New" in either of these menus???  Because I don't and yes I copied first before trying to paste the body on the left picture and the component on the right picture.  It only appears if you copy and bring up the contextual menu in open space.  This is counter intuitive to every program I've ever used before.  Autodesk needs to fix this hot mess of a program.  There are so many weird things like this that give it a steep learning curve not because of the power of what it can do but because of the idiosyncrasies of its user interface.  It holds back new users and limits the reach of this program.

[Oceanconcepts]

OK, I think I see source of confusion. I have to admit this took me a while, because it wouldn’t have occurred to me to click on (select) a body or component in the browser when trying to paste or paste new- the RMB is just a way to access the menu, selecting anything is not necessary once you have already copied what you want to paste. And yes, if you do that it’s not easy to discern why you get the results you do- particularly if you are unfamiliar with the body/ component structure that underlies Fusion. 

It seems that when you do that Fusion is trying to assign a relationship between the component to be pasted and the component you are highlighting /clicking on. From what I can see:

When you try to paste into the same component that was copied, Paste is the only option. You will get another component that is identical and linked.  If you are in parametric mode you can’t break that linkage, you would need to edit from the timeline.

If you try to paste into another component then you have the option of both paste and paste new. Paste New will add an independent component as a subcomponent to the one you selected. Paste of course adds a subcomponent linked to the original.

If you RMB without selecting anything (what I always do), you have both options, and a new component will be created with or without linking, depending on which option you select. 

If you select a body only, then the paste operation is independent.

Maybe someone from Autodesk can more fully illuminate the reasons for these distinct behaviors.  

[TrippyLighting]

I created this video to explain the different behavior of components and bodies when copy/pasting them. This also highlights the different behavior of these operations between Direct modeling mode and Timeline mode.