Objects move after a copy

[JohnSays]

I have created an assembly and desire to change the shape of one of the parts. I decided to copy it and "Paste as New." As soon as I do this, the components of my assembly scatter and some of the sub-components also loose their relative position. What can I do that does not require realigning all these individual parts yet again.

Btw, I tried assembling these parts using joints and found it impossible to move an entire component intact. Each time the sub-components lost their positions. I found it easier in the end to use the "Align" function to move an entire component assembly into place. (I did watch the video on how to use joints.)

I executed a "Compute All" and got a host of errors and warnings. I tried to resolve some of them, but quickly saw that that was a lost cause. I just do not know how to fix them. How important is this to fix them? I seem to be able to create the 3D stl files I need.

Warning: Combine2 Tool Body Error Warning: Mirror1 1 Pattern Source Lost
The model is using cached geometry to solve. Please reselect reference geometry for failed features in the timeline. 1 Pattern Source Lost
Failed to get target occurrence transform Warning: Combine1 Tool Body Error Warning: Combine2 Tool Body Error Warning: Align1 2 Reference Failures
The model is using cached geometry to solve. Please reselect reference geometry for failed features in the timeline. Warning: Align2 2 Reference Failures
The model is using cached geometry to solve. Please reselect reference geometry for failed features in the timeline. Warning: Align3 1 Reference Failures
The model is using cached geometry to solve. Please reselect reference geometry for failed features in the timeline. 1 Reference Failures
Failed to get owner occurrence transform Warning: C-Pattern1 1 Pattern Source Lost
The model is using cached geometry to solve. Please reselect reference geometry for failed features in the timeline. 1 Pattern Source Lost
Failed to get owner occurrence transform Warning: Combine5 Tool Body Error Warning: Position8 Compute Failed Warning: CopyPasteBodies1 1 Reference Failures
The model is using cached geometry to solve. Please reselect reference geometry for failed features in the timeline. Warning: CutPasteBodies2 1 Reference Failures
The model is using cached geometry to solve. Please reselect reference geometry for failed features in the timeline. Warning: Combine9 Tool Body Error Warning: Combine10 Tool Body Error Warning: Combine1 Tool Body Error Warning: Combine2 Tool Body Error Warning: Align1 2 Reference Failures
The model is using cached geometry to solve. Please reselect reference geometry for failed features in the timeline. Warning: Align2 2 Reference Failures
The model is using cached geometry to solve. Please reselect reference geometry for failed features in the timeline. Warning: Align3 1 Reference Failures
The model is using cached geometry to solve. Please reselect reference geometry for failed features in the timeline. 1 Reference Failures
Failed to get owner occurrence transform Warning: C-Pattern1 1 Pattern Source Lost
The model is using cached geometry to solve. Please reselect reference geometry for failed features in the timeline. 1 Pattern Source Lost
Failed to get owner occurrence transform Warning: Combine5 Tool Body Error Warning: Position8 Compute Failed Warning: CopyPasteBodies1 1 Reference Failures
The model is using cached geometry to solve. Please reselect reference geometry for failed features in the timeline. Warning: CutPasteBodies2 1 Reference Failures
The model is using cached geometry to solve. Please reselect reference geometry for failed features in the timeline. Warning: Combine9 Tool Body Error Warning: Combine10 Tool Body Error Warning: Position32 Compute Failed Warning: Position49 Compute Failed

[TrippyLighting]

Can you share your design ?

If so, please export it as a .f3d and attach it to your next post.

You can also share a link to it using following the link in the data panel.

[JohnSays]

Sorry but I cannot. I cannot make it public until after the patent is filed... which is in progress as I type. I'll create a work-a-round.

[TrippyLighting]

You cannot find a workaround for these mistakes. You've clearly ignored warnings throughout the design process and the nature of these error messages also fairy clearly indicates that your are missing some basic essentials in working with Fusion 360.

As such I'll link one of the AD support people in here @innovatenate. Maybe you can share your design with them offline so it can get the urgent help it needs.

If you continue to work with it in this broken state, chances are it it'll become unresponsive or go totally haywire and you might have to start over rom scratch.

[JohnSays]

Thank you.

[innovatenate]

It sounds like there may be a few key things missing from your workflows that may be leading to what you're describing. It's really hard to say without having a look at the design but, let me share some pointers that may get you going in the correct direction.

When you use the Paste New command in the Parametric Timeline environment, it is also going to copy those features along with your components. If the features aren't "contained" in your component and there are a lot of externally referenced geometry, there could be warnings/errors introduced when you do a Paste New. 

Try testing out the below workflows.

Workflow 1:
1. create a sketch in the root of the design
2. create a body from the sketch with some feature (extrude, revolve, etc.)
3. create a component from this body
4. perform a Save Copy As with this component

Workflow 2:
1. Create a new component in the design
2. Activate the component
3. Create a sketch in this component (on the component’s default planes and not the root component’s planes)
4. Create body from the sketch
5. Activate root design
6. Perform save copy as of the component

When you compare the results, you’ll note that the sketch/feature/body will "stick together" with a component using workflow 2. Workflow 2 better preserves the parametric features for later use and helps keep the timeline error free. In workflow1, the parametric features are lost and substituted for a base feature (dumb solid). In a similar fashion, externally referenced geometry and cross-component dependencies can lend themselves to failure. In the above workflow Save Copy As and Paste New are similar.

So whenever possible, avoid creating cross-component references and always Activate a component before you edit. To go one step further it may help to isolate the component you're working on (option is available from right click menu in the browser).

In the forum, @TrippyLighting has coined this suggestion RULE#1. There's lots of good content all over about it. See the forum discussion above for reference. 

There was a recent discussion below where I discuss some tips to consider when creating components in Fusion 360 I think may also be relevant here.

https://forums.autodesk.com/t5/support/scissor-problem/m-p/7086537#M2514

One trick you can use to get lose some of the parametric features is to right click on a feature in the timeline and select Convert to DM feature (Direct Modeling). 

As for the assembly/joints, behaving unexpectedly, I would really recommend watching the below class. I recently re-trained myself using this class and the instructors knocked it out of the park.

http://au.autodesk.com/au-online/classes-on-demand/class-catalog/classes/year-2016/fusion-360/pd1957...

Fusion 360 has a very open structure so joints can behave unexpectedly, especially if you treat Fusion 360 like an Inventor or a Solidworks. Here are some high level tips I gleamed from the class:

• Generally speaking you only need one joint between each component.
• Ground only fixes a component to the parent component and not across multiple levels or x-references.
• As-build Joints are awesome
• You can create Rigid Joints between components and origins

The bad news is that timeline errors and warnings should absolutely be fixed. However, if you understand the above points, they are easy to avoid. The last thing I'll add is that a regular Modify > Compute All is a good thing to get in the habit of. I like to do it before a save. These can reveal warning and errors that you may not be aware if you are doing some heavy editing in the Timeline. 

I hope that helps! If you have any quesitons, please let me know. 

Thanks,

[innovatenate]

Sorry I forgot to add.. if you would like to private message me a share link to the design, please feel free to reach out. 

Thanks,

[JohnSays]

Thank you for your post. I was unaware of way too much! I have been using Fusion 360 to design for about a year (off and on) and printing and machining 3D objects without being aware of the havok I was creating in my multi-part drawings. However, you hit the nail on the head with the whole, basically, incomplete copy from another drawing. I had been simply putting one object per drawing and that was working just great. Recently I thought, "Why not but the entire product in one drawing so that I can see it and see how the parts relate?" DUH! That is when the trouble started. Not enough trouble to stop me from producing. However, I suspect that that could come to grinding halt if I don't  pay heed now.

I have removed the patentable parts from my invention and would very much like to send you my botched-up drawing. I am messaging you after I write this.

I do not know how to get it back to a no-error condition. The thing is that -- and now I understand why -- there were only a couple of warnings and then after the copies, lots of errors and warnings. Even after I watched the videos on fixing them, I still had no idea how to fix them but II was still able to add and change features, so I just continued on.

The good news is that ev en if I cannot fix this drawing, I can recreate it and chalk up the time to learning. I want to do it right this next time.

[atherisinnovations]

I know this is an older thread, but I am not sure this issue has been fully resolved, at least not for me..

@innovatenate Basically, is there any way to repair the results of 'Workflow 1' in your example above? How does one 'reselect reference geometry'?

Ideally, being provided the option to pull all referenced constructions and sketches into a component when using 'Save Copy As' would be hugely beneficial, especially for those times that 'Workflow 1' is an unavoidable consequence of where one ends up in a "design exploration" (or if a client gives instructions that contradict previous parameters). Will something like that be possible for Fusion 360 in the near future?

Otherwise, yes, 'Workflow 2' should be the design aim at the outset..

[innovatenate]

Traditional CAD software forces you to follow a workflow very rigidly. In Fusion, the workflow is much more open, but there can be downstream consequences. There's not always a nice way to unpaint yourself out of a corner if that is where you ended up. Sometimes, rework is the only solution.

In some cases, if the parametric chain of features is simple and clean of externally (cross-component) references, you can shuffle things around. In the below screencast, I show how you can move a sketch to a new component after creating a series of features in the root of the design. By moving the sketch, you'll note that the entire parametric chain (which is dependent on the sketch) moves as well. 

http://autode.sk/2irDAaZ

You'll note at the end of the video above how the base plane for a sketch is a subtle and often overlooked cross component references.

Workflow 1 highlights that if you are thinking something should be a component, do it first and do it often. The other tips I mentioned help avoid the pitfalls that make it difficult to move around parametric chains.

"whenever possible, avoid creating cross-component references and always Activate a component before you edit. To go one step further it may help to isolate the component you're working on (option is available from right click menu in the browser)."

The below screencast is what I mean by re-selecting reference geometry. Basically to repair features that have lost association to the source geometry.

http://autode.sk/2AYqauX

With that said, Fusion 360 has extremely powerful direct modeling capabilities. Brad Tallis highlights a log of great tips and tricks in the below class.

http://au.autodesk.com/au-online/classes-on-demand/class-catalog/2016/fusion-360/pd16277#chapter=0

The timeline is not something must always be used. In some cases, it is actually easier to work in direct modeling.

I hope this information helps!

[Anonymous]

I am relatively new to Fusion but I would add that when my timeline beaks one (albeit labor intensive) solution is to delete all broken elements in the time line. For me this tends to reveal the required order for making things work (workflow). Sometimes I end up starting a new document and using the old document to supply sketches at the proper time.