Drawings won't update after design changes

[Muzzerboy]

I created a set of compt drawings from my assembly for checking just now. Having spotted a couple of minor errors, I corrected them in the design space. Back in the drawing environment, I can't get the changes to come through. The design is now at v79 but the drawings are stuck at v76. How can I get the drawings to reflect the latest changes? I've attached a screenshot showing the different versions coexisting.

I've made sure the design changes are saved before going back to the drawings. I've even closed Fusion down and reopened both the design and the drawings. Still no cigar.

This happened a few days ago and so this is a recreation of those original drawings, as I assumed I was being dumb somehow.

Hopefully this is something simple I've not done! Can anyone point out what I'm doing wrong here?

[g-andresen]

Hi,

is it possible to recreate this behaviour or share the design?

günther

[Muzzerboy]

I'm happy to share the file. How do I do that - there is one for the design and one for the drgs presumably?

[g-andresen]

Hi,

 Datapanel > rightclick > share pulic link:

günther

[Muzzerboy]

Here's the assembly  https://a360.co/2zWuqPV 

And the associated drawings https://a360.co/2UeEESw 

Presumably they have to reside in the same folder so they can find each other? The dia 3.78mm dimension shown is corrected to dia 3.33mm in the latest assembly but refuses to come through to the drawing.

[g-andresen]

Hi,

I tried.
1. I had the described behavior in some operations.
2. Then I removed the dimensioning, zoomed a little and put it back. I repeated this procedure several times and could not find any error.
Just try it once.

günther

[Muzzerboy]

Hi Guenter - I've tried that, both before (many times) and again just now. But no matter what I do, the dimensions stay unchanged and the model referred to in the drawing remains R76.4, while the model is now at R83. Did you actually manage to get the drawing base model to update to the correct revision?

So basically, the drawing is correct at the time I create it but if I change the model, the drawing goes out of date and has to be recreated. That's no good and it's surely not what the team planned.

I can't see anything I've done wrong - equally, I can't imagine how this could be usable in a professional environment. I have to wonder if it's some sort of functional issue (I hate to say "bug"), yet I couldn't see anyone else reporting it.

Is there a central area for bug reports?

Thanks for your help!

[Anonymous]

@Muzzerboy 

I was curious and changed your threads from 4,5 mm (your value) to 3.5 (resulting diameter in model: 2.93) and the other thread from 4.0 mm (your value) to 3.0 (resulting diameter in model: 2.53).

Then I saved the model, updated the drawing and the results are ok, no problems (see screen shots).

You have to be patient with the drawing update and wait until the cloud storage of the model is complete.

[Anonymous]

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@Muzzerboy wrote:

........the model referred to in the drawing remains R76.4, while the model is now at R83......

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Wait a minute, did you copy the model and continued your work in the copy?

[Muzzerboy]

I'm beginning to think I must be living in some form of mind altering time warp!

When I download those files (the same ones as you, presumably), without changing anything at all, the hole diameters in the model are both 3.33mm (tapping size for M4), yet the drawing still shows 3.78mm. 

I'm wondering where you got these odd hole dimensions from (4.5mm??). The hole dialog shows the M4 definition and when I measure the result, it's what I'd expect. Meanwhile, the drawing stays the same (3.78mm) no matter what I do.

The 4.5mm holes that DO exist are the clearance holes in the mating plates. Could that be what you modified?

I'm tempted to consider marking the holes out and drilling them by hand at this rate. Placing the holes in a sketch seemed the sensible approach and the resulting arrays of holes are hardly complex.

[Anonymous]

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@Muzzerboy wrote:
...
....

I'm wondering where you got these odd hole dimensions from (4.5mm??). The hole dialog shows the M4 definition and when I measure the result, it's what I'd expect. Meanwhile, the drawing stays the same (3.78mm) no matter what I do.

.....

....

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To answer your question, this is what I did:

1) downloaded the drawing you published - the file: 4th axis assembly Drawing June.f3z contains the referenced model, that was all I needed

2) uploaded 4th axis assembly Drawing June.f3z into my Fusion 360

3) opened the model

4) selected the thread hole in the component Motor side plate , then mouse right-click to edit feature (see screenshot)

5) then I got the dialog-box with the 4.5 mm (see screenshot)

6) measured the hole diameter => 3.783 ((see screenshot)

I guess you dont´t work in the model that is referenced by the drawing - please see my post #9. The model referenced by the drawing is shown in the data-panel (see last screenshot). Please see what´s shown on your computer.

[Muzzerboy]

No, I didn't create any copy. The whole point here is that the drawings didn't update after that time. I'm struggling to get that point across it seems....

[Muzzerboy]

Latest model https://a360.co/2zWuqPV 

Latest drawings https://a360.co/2UeEESw 

So when I look just now, the model on the webserver seems to be correct (hole dia ~3.3mm, although the measure tool doesn't seem able to report diameters???). 

But I can't open the drawings from the link. "Oops! Sorry. We have encountered some issues when preparing file for viewing. Please contact support for assistance." Obviously I'd like to see if the drawings on the web server are still wrong at this point. 

The reason they are different files(?) is because "create drawing" opens a new tab in the Fusion space. There needs to be some clever trickery to ensure they remain synchronised. Seems the drawings contain a copy of the model but I'm getting the feeling that may be an outdated version that isn't getting updated.

What happens if somebody else tries to view the drawings from the second link above and check the hole dimension? Is it 3.33mm or 3.78mm? I'm guessing the latter but naturally I can't check myself....

[Anonymous]

@Muzzerboy 

"...Seems the drawings contain a copy of the model..."

No. The drawing file contains a pointer/reference to a model file. Just check if the correct model file is referenced by the drawing file.

How? See my previous post => data panel, "uses" => if the version of the model file is not the one you think it should be then something is wrong. For whatever reason.

[Muzzerboy]

Well, that's very much been the problem from the beginning. The drawing is STILL stuck at v76 and in the meantime the design is (now) at v87, which is pretty much what I said at the top of the post. All of the revisions in the interim have been me pulling my hair out with this. I have done almost nothing to get the design closer to metal.

You might argue that I don't need the drawings if I simply go to CAM now but I find them helpful for setting up the stock, identifying which piece is which and checking the dimensions before scrapping any of the expensive stock. However, I have a life to live, so that may be the pragmatic route on this occasion.

And given that the drawing file has now become inaccessible ("file failed to download" - that just had to happen), I will just move on and let somebody else figure it out. I don't imagine this is a one-off, as that's not the way software works.

[Muzzerboy]

Recreated a one sheet drawing just now, then made a trivial change to the design and it appeared to update (the yellow triangle disappeared), then changed it back. The data panel says it's still at the original version 87 but there is a newer version 89 available. Well yes, I know that - so how do I get it to update??? I've tried the obvious(?) stuff. I can see the v89 on the server. This is doing my cake in.

[HughesTooling]

Something that could be a problem for anyone downloading the 2d drawing as an F3Z file is it will probably still be linked to the old 3d design. I fell into this trap a while ago where I downloaded a 2d drawing that had not been updated so got an older version of the 3d model.

Here's an example of what I mean. The 2d drawing is still linked to V5 so if I download the 2d drawing I'll get V5 of the 3d design not the latest V6.0

@Muzzerboy  One thing you could try is clearing the user cache to see if that forces the 2d drawing to update to the latest version. @Phil.E  Can you help.

Thanks Mark

[HughesTooling]

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@Muzzerboy wrote:

Recreated a one sheet drawing just now, then made a trivial change to the design and it appeared to update (the yellow triangle disappeared), then changed it back. The data panel says it's still at the original version 87 but there is a newer version 89 available. Well yes, I know that - so how do I get it to update??? I've tried the obvious(?) stuff. I can see the v89 on the server. This is doing my cake in.

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The images above are from the online hub? What happens when you open the 2d drawing in Fusion, is there no option to get latest?

Mark

[Phil.E · Accepted solution]

You have saved v76 of the 3D model as a milestone.

The drawing references this milestone and will not update until you save a new milestone. That is seen in your "Uses" image. The drawing uses v76, the milestone version.

Milestones are the way to add release management (in rudimentary form) to your designs. It also prevents version churn in production.

The help section has much more detail:

http://help.autodesk.com/view/fusion360/ENU/?guid=Fusion_Import_designs_milestones_versions_html

It works like this, an example scenario:

1. You are ready to make a prototype of your design. In release world, this is typically Rev1.
2. You save Rev1 as a milestone, make drawings of it, and now it can be machined in your shop using your model and drawing.
3. Meanwhile your design engineers begin working towards a first commercial release, typically Rev A. 
4. You make changes to the 3D model, change minor details for whatever reason, start rendering, begin doing more Simulation, making more drawings, animations, etc. (all of which forces saves)
5. But the shop is still working with a milestone version Rev1 drawing, undisturbed by all this activity.

In other words, you begin doing the "rev A" work that requires many saved versions and you don't want to disturb the milestone Rev1 which is actively referred to by Fusion users in your machine shop. Until you save a new milestone "Rev A" for example, the drawing will not update. It refers to a milestone at v76.

Regards,

[Muzzerboy]

Hi Phil - phew - that makes perfect sense! I was hoping there was a simple explanation and fix but nothing seemed to be forthcoming. I guess that's the downside of working over the weekend when the Fusion team is away.

I foolishly made a milestone save a few days ago, as I thought I should be making more note of major design stages along the way. I probably thought I was being clever.

I understand the importance of version control in a professional environment, having been caught out myself in various workplaces by uncontrolled documents. 

Having created a milestone, I can't see any way of "uncreating" it. There may be a reason why you shouldn't be able to delete a milestone but it seems that from now on, I will need to create another milestone each time I want to bring design changes into a drawing. Previously, I only had to click the yellow triangle. I will let this be a lesson for the duration of this particular activity!

Many thanks for pointing out the simple misunderstanding on my part. Hopefully others will learn from this experience.