Fusion
If I understand what you are trying to do, I suspect that part of the problem is that you are missing a coincident constraint here:
Anywhere you see a white dot like that, it usually means that those points are not constrained together. That's why they "come apart" when you move them.
If you want the entire thing on the right to move together, you will have to add lots more constraints and dimensions, too.
Can you describe what you'd like the final result to look like? Also, if you share your model, we can show you on your own model.
Jeff Strater
Engineering Director
@rebeccah_luttrell - here is a start. The technique I usually use is drag. Just drag a sketch line/arc, and see what comes with it. If you hit ESC, it will cancel the drag (or, if you forget, you can use undo). So, find out what moves, and lock that down using dimensions or constraints. In this screencast, I used only dimensions (except for the upper left corner, with the missing coincident constraint). I tend to like Aligned dimensions, but others will work as well.
Once you can drag the entire shape, then you can dimension it to something else, and it will move as a group. Hope this gets you started...
Jeff Strater
Engineering Director
OK, I think I know what is going on here, after looking at your design again. I just got lucky, and the part of the design that I modified did not have this problem. But, everywhere else, you seem to have MANY copies of the geometry on top of each other. You can tell this in two ways:
- you'll notice that the lines, and especially the profiles, are a little bit darker
- if you use Select Other (hold down left mouse button for 1/2 second) you can see the list of things under the cursor. I counted 6 lines on this part of the sketch:
So, when you are dimensioning, you are really only getting one of those 6 lines.
I understand how this probably came to be, and it is really a bad bit of UI in Fusion (one I have been trying to get elevated for a fix for years...). If you use Copy/Paste, it is a two-step process when you Paste. First, the sketch geometry is pasted, then the Move command is invoked on the copy. Normally, you move the copy away. But... If you cancel at this point, you are only canceling the Move - the Paste has already happened. So if you Copy/Paste/Cancel, each time that will leave another copy on top of the original. Like I say... bad. In the screencast below I demonstrate on a simple rectangle. The first Paste, I move the geometry away. On the second, I Cancel, and show that I now have 2 rectangles on top of each other...
as to what to do - you can either try to clean up the copies, or just get rid of all but one set (in the design you shared, the upper most copy has only one set of geometry), fully dimension that, and copy/paste that (without cancel), 3 or however many times you want for each copy
Jeff Strater
Engineering Director
