Trying to elongate a body (part of it stays the same size)

[Anonymous]

I have a Fusion 360 file that someone else made. I'm trying to elongate a body in the file by moving one end but only part of it elongates and z-fighting becomes visible when I do this. How can I elongate the whole thing? Thanks.

[etfrench]

Pretty hard to say without the file or any pictures.

[Anonymous]

I uploaded a screencast. I don't know why it isn't displaying in the OP:

https://knowledge.autodesk.com/community/screencast/51acf6e9-8f52-462d-9289-cfdc841f7bf2

[g-andresen]

Hi,

To do this, you would have to look at the origin in the timeline in order to intervene at the appropriate point.
Or you can create a new construction > Screencast.
That takes max 2 min.

günther

Also pay attention to the number of elements in the timeline!

[TheCADWhisperer]

Are there any unresolved issues highlighted in your Timeline?

File>Export and then Attach your *.f3d file here.

[chrisplyler]

Possibly the flat piece was made with an extrusion in the short direction, from a sketch profile that was constrained at least with a defined length. So when you "move" one end of it, the other end must follow to maintain that defined length.

This is just a guess, since you have not posted the file for us to examine.

As a general rule of thumb, don't just "Move" stuff.

[Anonymous]

Thanks. The file is available here: https://myhub.autodesk360.com/ue29f5e7b1/g/shares/SH7f1edQT22b515c761ed4937902b0947df1

I'm looking at the timeline but I'm not used to navigating it and it's pretty big.

[laughingcreek · Accepted solution]

Ideally a model is made in such a way that the steps are well organized, and changing the size is just a mater of editing a sketch dimension.  This model is pretty hopeless.  The irony is that it probably would have taken less time to model with solid modeling practices, and resulted in a model that takes no time at all to make size changes.

moving on

at this point direct modeling is going to be your best bet, so using the move is fine.  as you have found there is something about the geometry that interferes with moving faces.  here is a screen cast of  a heavy handed method of splitting the body, moving it, and connecting it back up.

https://knowledge.autodesk.com/community/screencast/372d15e6-8820-4a64-acce-46855a8737e8

I noticed the fillet around the edge when all the way across the vertical face and consumed it, so I tried editin that fillet in the timeline so it had a smaller radius.   After that, moving faces the way you were trying to do worked as expected.  here is a screen cast of that-

https://knowledge.autodesk.com/community/screencast/696d38db-f0fa-4886-9217-032dcdf02c09

@jeff_strater -is the way the filleted edge interferes with moving  a bug or limitation? definitely weird.

[Anonymous]

Thanks very much, LaughingCreek. I went for your second solution in the end. 🙂

[jeff_strater]

@laughingcreek - the issue here is that fillet face.  Internally, Fusion does what we call "reblend" during these kinds of geometry moving operations.  Basically, Fusion tries to remove all fillet faces, then move the geometry, then re-apply the fillets to preserve the shape.  In this case, because, I think, that fillet face completely removes the adjacent planar face, Fusion gets confused.  Usually, what fixes this kind of thing is the right selection of faces - just select the minimum number of faces necessary to get the result.  In this case, I found that 3 faces were enough:

[laughingcreek]

well now that's interesting.