The project source is lost. Need help!

[CGPM]

I have a model with a sketch that is now missing the project source, after I deleted some things, and I can't figure out which entites it is missing.  I have been doing this with several sketches but have one that doesn't highlight the geometry so I can figure out what to fix.  What is the correct procedure to do this?

[innovatenate]

It sounds like you performed a hard delete on a body or component. Now, a sketch that contains sketch entities, projected from the deleted body, are now missing their reference geometry. Is this breaking downstream features in your timeline?

What is the first item that is highlighted in yellow or red in the timeline? Is it a sketch or another feature? If it is a sketch, you may edit this sketch and use the break link command (right click on projected geometry and select break link) to remove the reference to external geometry. 

If this suggestion does not help, could you share the design? Feel free to send me a public link (nathan.chandler@autodesk.com). I'm happy to take a look at it. 

Thanks,

[CGPM]

Yes it was a hard delete and there were a few sketches and extrusions involved.  I have fixed everything except for the one sketch left.  It has a lot of projected geometry and I do not want to break the links since I will most likely be modifying the model in the future, and want the model to change as I change referenced geometry.  I just can't figure out what is wrong with this one sketch.  I have sent you a public link to this file, hope I did it right.

Thanks for your help!

[Anonymous]

Besides the great points Nathan made, just wanted to mention some things I remember doing. 

First being turn off visibility of all sketches.  A systematic way is to turn on and off each component visibility, until a sketch turns off, then expand that component to turn off its sketches visibility, and after that collapse the component branch again. 

Then a procedure to view each sketch (or other feature) involves going through the timeline, hovering or clicking on each sketch, causing it to appear in the model space.  If hover over a sketch in timeline and then move just above it, repeating this cycle, can help detect where it is in model space.  If cant find can also right click and choose find in window.  Furthermore, clicking on a sketch in the timeline will cause the corresponding component and sketch to be underlined in browser. 

If have a broken dependency, go to yellow or red feature and timeline, right click it and choose Review Warning. Besides a description of the problem being given, the trouble reference, say in this example a missing line reference projected into another sketch, will be shown in red in the model space.  Once this is feature is identified, use undo until warning goes away, and hover each sketch in the timeline to find which one has that referenced feature, that was subsequently deleted. When find it, in the timeline note its info given (name and component in), and perform necessary actions to resolve the issue. 

Just some thoughts 😉

Jesse

[innovatenate]

If you have deleted the source geometry, the sketch entities will not update anymore because there is no longer a parent geometry to update!

You don't necessarily need to break the link for every projected sketch entity. As long as the source geometry the is still in the design, the reference between the 2D geometry and the 2D sketch entities can be maintained. Any healthy projected sketch entity that still has its source geometry intact can stay linked in the sketch. 

Taking a closer look at this, I see that the root of the issue is not that the projected geometry has disappeared, but that a construction plane has updated in an adverse fasion.

It seems that the real issue is that the sketch has lost connection with the base plane. Please try the following solution.

1. Activate Drive Plate component (this greatly simplifies the timeline)

2. Make Construction Plane 1 visible in the Browser and workspace

2. Right click on the sketch with the warning in the timeline (sketch 5), then select Redefine Sketch Plane

3. Select Plane 1

The problem is resolved with no further timeline computation issues. I note that if I activate the top level and perform a Modify > Compute All command, all features appear to be healthy.

If I Edit Plane 1, I note that it appears to be based on the face of another component (Body:1). I suspect this component was recently edited in a way that may have caused the plane to flip or to change in someway. This forced the sketch to loose it's references.

I hope this helps. Let me know if you have any questions or would like a copy of the file. 

Thanks!

[CGPM]

Yep, that did it, but when I try to project the hole of the slider component onto the Drive Plate I get "the project source is lost" error and the yellow warning comes back.  Redefining the sketch to the construction plane again removes the yellow warning.  This 3" vise is a "save copy as" of a 2" vise I first designed that I simply made the Body1 sketch 1" wider and 1/8" taller, all other components automatically adjusted.  I deleted the same component in the 2" vise assembly and I was able to rebuild all of the sketches that were affected.  Any chance I could get you to look at this again???

This project is me making my own aluminum double acting vises.  2", 3", and 4" that I can pattern into 4 sided tombstones to mount on my 4th axis, then mirror end to end for up to 16 stations per cycle on my vertical cnc mill.  I would really like to get this figured out, if it's not too much work.  I have tried a few things to fix this and nothing has worked.

What I did to cause the problems in the first place!

I moved the slider to it's own file since it is steel and needs different tools than the rest of the assembly, which is aluminum.  When I deleted it I lost all the reference geometry.  Some of it created the t-slot in the Body1 component.  This is the only sketch that I haven't been able to fix.

Thank you for all of your help so far and if this is more than you wish to help with then I will call it solved.

[innovatenate]

A great way to document issues and communicate them is to use the Autodesk Screencast recording utlity. You can get this utility for free from the below link.

https://screencast.autodesk.com

I'm trying to follow along, but I do not understand what is meant by "slider component." I didn't find a component named that in the browser. Can you clarify? 

If you activate "Drive Plate:1" component, and redefine the sketch base plane to be the default origin planes of "Drive Plate:1" (instead of being based on a face from Component "Body:1"), this may help. 

When creating cross-component references (using the project sketch), it can be difficult to determine how model changes will impact the model. Especially, if you are deleting a component/body that is being referenced elsewhere. This will cause failures in the timeline. The design's timeline will have to be cleaned-up every time.

There's a pretty helpful post below, that dicusses a few best practices and this concept in detail. It may be helpful to review this post. 

http://forums.autodesk.com/t5/design-differently/fusion-360-modeling-best-practices/ba-p/5502252

I hope this helps. Let me know if you have any questions.

Thanks,

[CGPM]

Here is the screencast of what I am trying to do, which works fine with the 2" vise model.  http://autode.sk/1gXOEZX

I am trying to project the hole through the Slider component onto the Drive Plate sketch so if/ when this hole changes it will update the Drive Plate.

I am clueless about "redefine the sketch base plane to be the default origin planes" and couldn't find any information on this after a few searches.  More info please.

I am familiar with the Modeling Best Practices post and have watched the videos several times.  All of the other repairs went fine, this is the only sketch that I am having problems with.

I would like to keep the components in my model as closely associated with each other as possible so as I change something in one component the others automatically adjust as well as I refine the design.  The body and slider components are the base components of the whole model.

[innovatenate]

Wow! Good find! I have reported this to develpment via report ID (FUS-19681). I'm not sure what is causing that, but I suspect this is not intentional. Development will investigate the issue for possible cause and resolution. I or a member of devlopement will provide an update here as information becomes available. 

To get moving forward, have you tried deleting and re-creating this one component from scratch?

Thank you for reporting this issue! 

[CGPM]

Glad to hear that behaviour is abnormal.  I did just try to project to a new construction plane and sketch but the problem repeated.  I could project from the Body component but not the inserted Slider component.  http://autode.sk/1LjKUfD

My current workaround is to just sketch the hole in.  Not a big problem, I just couldn't figure out why project would not work on this sketch.  It seems that the inserted Slider component may be at fault.  I will try inserting a new Slider component as a fix.

Ok, this is what happened, below is the error.  http://autode.sk/1LjM1vX

This insertion operation, along with undo or redo of previously committed commands, will result in a cyclic dependency between Slider v48 and 3in Double v7. To prevent that, the insertion operation was cancelled!!

[Fusion360Hodad]

I am having difficulty troubleshooting a similar issue. See screenshots below. I tried selecting the red dots without success. Any ideas on how to troubleshoot and resolve these errors?

PLAN/TOP VIEW

 RIGHT SIDE VIEW

RIGHT SIDE ISOMETRIC VIEW

Error message on Extrude

[Fusion360Hodad]

Additional screenshot of error message on the sketch with extruded body visible.

[Fusion360Hodad]

Resolved the error on the extrude by editing the feature and changing the Extent to All and then selecting Flip to reset the extrude in the correct direction and through the thickness of the body.

[Fusion360Hodad]

Finally resolved this problem (warning messages) with the following steps:

1) Rolled the timeline back to the original sketch.

2) Edit sketch.

3) Toggled show points in the sketch pallet to identify the problem points as yellow circles.

4) Problem appeared as the vertices not being coincident, but also suspected that there was an offset plane issue that was more difficult to identify because the circles indicating the coincident point problem were at the exact same points on the sketch as the yellow circles indicating the offset plane problem

5) Identified the offset plane issue by first determining which end of the vertices I could move and moving it away from the vertex of the perpendicular line so that there was clear separation between the two vertices.

6) Selecting the 1 key to right drag a box to select just the yellow circle (lower right) that enabled identifying it as an offset plane that I could delete. Deleted the offset plane.

7) Repeated the steps for the other yellow circle (upper left).

8) Reconnected the vertices and verified coincidence.

9) Reapplied the dimensional constraints.

10) Lastly performed a Comput All to verify resolution of the problem.

11) Moved the timeline back to the end to check for any other warning or errors resulting from the changes. No warnings or errors.

Problem solved!

Credit to Tyer Beck of TECH & ESPRESSO. Watching some of his videos on Youtube helped me figure out how to solve the problem.