How to extend parts in fusion 360

[68031B]

I am CADing my intake for this year and I need an axle that’s longer than the standard 3 inch one that comes with the library, How do I make it longer?
(I have tried using the extrude command along with every other modify tool in fusion 360)
I have seen other tutorials use the “Modify part” tool but Google has told me nothing about it and I believe it’s something you have to add to fusion 360.

[5062F_Adam]

Create a sketch, and then use project geometry on the sides of the axle, and then extrude the resulting face. (There might also be a push pull feature, but it has been a while since I have used fusion 360 for cad so i don’t remember if you can do that but I know for sure the first method would work)

[68031B]

Push pull only works on bodies, but thank you for your help

After messing around with the extrude tool more I found out you can extrude a new component. This works for axles but I still can’t modify c channels (not by length, but by width)

[u89djt]

You can select and move the end faces of a shaft.

Be more specific about what you want to do to which channel and I’ll show you how to do that.

[68031B]

You are using move copy…That doesn’t extend the shaft…It just moves it (You seem to know what your talking about so maybe you just clicked the wrong tool).
I want to be able to cut the “C” part of the c channel that sticks out (I’ll add a picture, it’s hard to explain.

[u89djt]

Ah, no, I got it right, and it’s very good that you lean into learning something new. Just those selected faces move, and the sides of the shaft are extended or retracted to match up. If you could see the other end, you would see that it doesn’t move. Try it I should have thought to shorten into the window first to make this more obvious.
OK, to your C channel. There are lots of ways of doing it. The quickest one would be to select the internal face - the one you can see lying horizontally in your image - and extrude that downward and use the intersect operation.

That will create a new body in the active component and delete the original channel body from its component. To keep the original body, create a new body from the extrusion instead of immediately intersecting, then perform a separate intersection and select “keep tools” so it isn’t deleted.
Another way would be to use the split body command and use the vertical inner faces of the sides to perform cuts.

That will cut the original channel body into three parts; centre, side, side.

[68031B]

I will test this when I get home, Thank you so much for your help

[u89djt]

You’re very welcome. Experiment boldly in CAD - you’re not wasting metal

[68031B]

Which library are you using? Clicking on all sides of the axle doesn’t select that side of the axle (suggesting there are no faces on the axle)

As for the C channel, following the steps you gave me I get the “No target body found to intersect!”

I’m thinking we are using different libraries.

[u89djt]

I’m using the original CAD models from the vex website in this instance, but that’s not relevant to solving your difficulty. You can definitely achieve what you need with the library you are using.
“No target body found to intersect” is happening because the thing you’re trying to edit is still linked back to the source.
https://www.autodesk.com/support/technical/article/caas/sfdcarticles/sfdcarticles/No-target-body-found-to-cut-or-intersect-when-extruding-in-Fusion-360.html
Right-click the component and select “break link” and you can go ahead and intersect or cut it.
For the axle, I don’t understand yet. Can you post a screenshot of the axle and its entries in the browser list? Like this

[68031B]

My axle is a component, not a body. That’s why your able to use the extrude command the way you are.
I will test the c channel method tomorrow.
Thank you for your help!

[u89djt]

Here is what happens when you don’t break the link, and then what happens when you do.

Break the link to the original component if you want to edit it.

[68031B]

This worked perfectly, thank you so much.
The only thing is I get 20+ errors when I do this. Do those matter?

The error: Implicit Join fail
Then there are couple revolute joints that failed

[u89djt]

Heh, yes the errors matter. Don’t leave errors sitting around in a CAD file if you’re going to use it.
Coaching mode: you know that joints are made between components located and oriented according to features on the bodies within the components. Think about what you just did to one of the components. What do the failed joints connect to? You have some remedial work to do that I think you can work out for yourself. Tedious, perhaps, but you took away one component and replaced it with another that looks the same to you, but is not the same data to the software. The software has absolutely no idea what you’re trying to achieve, so if you pull out a part, it’s your job to reconfigure it.

[68031B]

It really weird though, the errors are there but nothing actually changed.
My dr4b still moved like normal, same with my mogo mech.

[u89djt]

Yes, it caches the joint relationships (or whatever it needs to) when you make a breaking change and tries to work with those, and you’ve been kind of lucky. You should rebuild them. If you double click on the yellow highlighted step in the timeline, you’ll get the opportunity to reselect stuff.