Fusion360 won't let me edit my extrusion

[kyle.kramer2]

I'm used to using inventor so I have no idea what I'm doing wrong here. But I have this part, and I'd like to edit it, but when I do the edits don't show up in that bottom timeline but in the side tree thing. When I try to edit them as well it doesn't let me reopen the feature to change anything about it. Am I in a different mode or something? I need this specific part to be changed as it's linked to other parts for machining so I can't create a new one from scratch. What am I missing here as this should not be this hard to change a part.

[kyle.kramer2]

It also won't let me extrude join for some reason, I can only extrude cut or extrude a new body.

[jeff_strater]

Your design is not parametric.  Only history-based (parametric, with the timeline enabled) designs allow feature editing.  Your design appears to be a Direct Modeling design.  Did you create this design from scratch, or import it?  Imported designs come in as Direct Modeling designs.  You can:  import a design, turn on history, then create parametric features on top of the base DM design.  But, unless you do that, you will not be able to edit features

[kyle.kramer2]

Not sure how it was brought into fusion as that was done before my time, I think it was made in Solidworks before and exported over from there. Do you have a recommendation to a good resource to how I can turn on history?

[jeff_strater · Accepted solution]

turning on history is easy.  Right click on the root browser node and choose "Capture Design History":

However, be aware that this will not result in a timeline for your imported Solidworks design.  It will only record history for features added after history is turned on.  There is no way in Fusion (or in any other CAD software that I am aware of) of importing parametric design history from one system into another.

[kyle.kramer2]

So I've added the history which does let me now edit my extrusion but I still cannot make an extrude join. (There is a grey cylinder being rendered but when I screenshot it disappears)

[TheCADWhisperer]

Looks like you have the top level of the assembly active rather than one of the Components.

Did you go through the Tutorials, or did you jump right in to the deep end of the pool?

Can you File>Export your *.f3d file to your local drive and then Attach it here to a Reply?

[kyle.kramer2]

I don't even think I realized there was a pool. Must've strapped some cement blocks to my feet and went right into the deep end. But I believe I tried activating the component I was working on earlier (like it had the black dot next to it) and still no go.

[jeff_strater]

CTRL or CMD will cause the preview to be suppressed, which is why it goes away when you capture the screen (on Mac, for instance, area screen capture is CMD/SHIFT/4, so the CMD will suppress the preview.

If your sketch plane is on a face of the existing body, and if that body is not in a component that is external to the design, then Join should be OK.

I think it's time to share your design here.  It will be easier to debug that way.  Export as a Fusion Archive, and attach it to the forum.  Thanks,

[kyle.kramer2]

will add the file in one sec too

[kyle.kramer2]

Here is the file. Not sure why I'm having so much trouble with something so simple, I've used Autodesk Inventor for maybe 8 years now so I figured this should be straight forward working with fusion360, though since I can't even figure out how to edit a part I guess there isn't as much overlap between the two programs as I thought. I very much appreciate the help! Didn't quite know the words I should punch into google to figure this out.

[jeff_strater · Accepted solution]

Thanks for the model.  See the screencast.  You don't have to activate the component to get the join to work.  I only did that so that the sketch I created was then owned by that component - it's a better design practice.  The join does work.  You'll notice, though, that the new extrusion is colored differently.  That is because the imported component has face-level colors applied, not body-level or component-level colors.  So, the new faces do not inherit that appearance.

Don't beat yourself up too much (or beat up Fusion, either, for that matter).  In some ways, learning Fusion after 8 years of Inventor can be harder than learning it without that CAD experience.  There is a lot of overlap between Inventor and Fusion, but there is also a lot that is different (local components, timeline, parametric assembly operations, a different sketcher, joints vs assembly constraints, etc).

[kyle.kramer2]

I've got no idea what changed but yeah now it works when I follow what you did! Just glad I was able to screenshot it not working so I didn't look like too much of a crazy person haha. Thank you so much for the help! I'm thinking I'll need to find a good class online that goes over all the basics as the last few days have been very slow going, nothing against Fusion of course, it has its strengths over Inventor, I just need to get used to the little differences.