Project/include not working with external component

[Anonymous]

Hi -

A simple workflow: I designed a component (A), then inserted an external component (B) into the model and added a fixed joint to position B relative to A. Component B has four holes in it and I want to add aligned holes to A. So I created a sketch on a surface of A and tried to project/include the features in B on to that sketch.

Result - I get the message "The project source is lost. Cache is used!" I checked - both models are saved and I have inserted the latest version of the B model. Everything seems to be up-to-date.

If I break the external link for B then project/include starts to work correctly. If I undo "break external link" then it stops working again. So there seems to be some problem with the external reference, but I have no idea how to fix it. I do want the B component to remain external.

Any thoughts appreciated!

- MWoll

[davebYYPCU]

Project > Include 3....

is generally for 3d Sketches

Try Project > Project, or

if the holes penetrate the sketch then Project > Intersect

Might help....

[Anonymous]

Thanks for reply. My mistake - I wrote "project/include" because that is what is says on the menu and I wanted to distinguish it from "project" (As in "I use project in my F360 project.").

So I should have said "the project tool" or "I pressed the P key". But the problem remains - It does not work to reference features on the external component, but it does work if I break the external link first.  I want to keep the component external so I hope this is not normal behavior.

- MWoll

[HughesTooling]

It works OK for me so not sure why you have a problem. Can you make a screencast of what you're seeing?

Mark

[Anonymous]

Thanks for reply. I made a screencast of the problem using some simple components. Here is the link:

https://autode.sk/2BEDPJy

Not sure if you can see it - it is shown as "pending" on my screencast page, but a screencast I made a year ago is also shown as pending, so who knows. Sorry it is a little rough, but you can see what is happening.

Have I just run into an F360 limitation? It seems very evident that you would want to be able to insert standard components with holes - say brackets or hinges - and then make aligned holes in other components. And why would you want to break the link to a standard component that will not be modified in the new design?

[HughesTooling]

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@Anonymous wrote:

Have I just run into an F360 limitation? It seems very evident that you would want to be able to insert standard components with holes - say brackets or hinges - and then make aligned holes in other components. And why would you want to break the link to a standard component that will not be modified in the new design?

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No you haven't run into a limitation as it works perfectly for me, can't see anything wrong with what you're doing. Have you tried closing and restarting Fusion, maybe even reboot your computer.

Mark

[Anonymous]

I tried restarting F360 with no change. Haven't tried rebooting yet but I see exactly the same problem on two different computers, one with a fresh install of F360.  Happens with my original model, where I ran into the problem, and with the simple model I created to test it.

Any other ideas? Thanks!

[HughesTooling]

@jeff_strater  Have you got any ideas why this isn't working? I've tried a few different ideas like importing non Fusion files and with and without components in the destination file and all work fine.

Mark

[Anonymous]

OK - I have a clue. In both models that I tried there was some kind of connection between the two components.

In the first case I had removed a boss from a component and made it into a separate, independent component with an added mounting flange. I then inserted it back into the model from which I started. I was mounting it on the component that it had originally been part of.

In the second case I made a simple plate, saved it (as part A) and then did a save-as (as part B). I then opened B, added some holes, re-saved it, and then inserted B as an external component into the model with part A.

I just tried instead to create A and B completely separately and the problem no longer occurred. My guess is that when the parts were created from the same "root" then F360 had some problem resolving references, maybe because both parts had some identical internal "names" even though they had different top-level names. If this is correct I would call it a bug.

It seems a common enough workflow to decide that some sub-part of a component will get reused in multiple places and would better be kept as an external "standard" component. This is the kind of gotcha that seems minor until you lose a hours of work time because of it.

[HughesTooling]

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@Anonymous wrote:

I just tried instead to create A and B completely separately and the problem no longer occurred. My guess is that when the parts were created from the same "root" then F360 had some problem resolving references, maybe because both parts had some identical internal "names" even though they had different top-level names. If this is correct I would call it a bug.

It seems a common enough workflow to decide that some sub-part of a component will get reused in multiple places and would better be kept as an external "standard" component. This is the kind of gotcha that seems minor until you lose a hours of work time because of it.

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Seem to remember this bug has been reported before. @karina.harper  Seem to remember you helped someone with a similar problem.

Mark

[karina.harper · Accepted solution]

Hi all,

Yes I logged this a few weeks ago. This is on the radar of the dev team and we're working on a fix. 

It looks like you all pinpointed the problem - the "save as" command creates an identical underlying ID # that then confuses Fusion, particularly if the two files are derived into a new assembly together. The workaround is to right click the top level component and select "save copy as". That should work as a workaround for "Save as".

(FUS-45957)

[Anonymous]

Thanks all - greatly appreciate the support. And the work-around looks easy enough.

It is a little worrisome though - a year after I first tried F360 I came back to it, started a new project, and within hours ran into a bug that stopped me dead. Hope this isn't a trend....