What seems to be simple task in most other CADs is apparently rock science with Fusion 360. All I want to do is move two lines (#1 & #2) left 15mm to create a larger opening (See picture). I cannot click and drag them. I've tried to move them with the MOVE/COPY command and have failed. Not sure how else to approach this. Any help would be greatly appreciated.
Thanks,
Kent
share the design. Export as F3D, and attach it to a forum post. It looks like maybe line 2 is fixed, but it is hard to tell from an image, that's why we need the design itself.
@skypilot65 wrote:
I was able to figure it out. I'm trying to move lines by selecting them, when I should've been selecting the faces. All good. Thanks.
No, you've not figured IT out. You found another way to accomplish the overall goal, but that is not a recommended workflow.
Also, I don't know what other CAD systems you are talking about. None of the parametric 3D CAD software I know (SolidWorks, ZW3D , Alibre Design, Autodesk Inventor) allows you to just drag constrained sketch elements around.
If you are able to drag other sketch elements around, then that means you did not properly dimension and constrain your sketch!
@skypilot65 wrote:
I apologize to all those experts out there for asking such stupid questions. I won't post here again.
I would not throw out the baby with the bathwater. The question you asked isn't stupid.
When you start your post here with:
"What seems to be simple task in most other CADs is apparently rock science with Fusion 360" then the issue is probably more how you asked the question 😉
Looking at some of your sketches, the first thing I would suggest is to turn off these two settings in the preferences.
These autoprojections are supposed to help people new to Fusion 360 but very quickly they become a nuisance. The main purpose of a sketch in a parametric 3D CAD application is to create simple base geometry to be refined further with 3D features. As such any clutter in sketches, including auto projected stuff that isn't needed is better kept out of a sketch.
You have much better control if you manually project only those objects (edges, or objects form other sketches) that you need.
The next thing to consider before sketching anything is if the object you are about to design has some form of symmetry, or patterns. The origin of a design should be in the center of the symmetry. In your design it's off to the side.
There's much more to learn on this design. Go through the timeline step by step. Edit every feature and every sketch to see how it was done.
Attached is an almost complete version (without the washers that are levitating in thin air ).
Firstly, my workflow isn't the only workflow. This can be created many ways. I just wanted to show some techniques that can be helpful. I uses the offset faces after the shell command to avoid having to use the offset tool in the first sketch.
My personal preference is to use 3D modeling features instead of sketches. It makes sketches simpler and more reliable. I spent much less time sketching and debugging sketches. While it is counterintuitive, it also creates computationally faster models.
The purpose of Sketch 2 is to create the outline for the openings in the sides. I created it on an origin plane rather than a face of the existing 3D geometry. Origin planes don't change and as such are a more stable reference then faces of 3D geometry.
I project/Intersected the body into the sketch. A body is a more stable reference than individual faces:
then I used constraints to make sure that the little rectangle for the cutout is always centered horizontally in the tab.
Sketch2 and Sketch4 are independent and have nothing to do with each other.
The way I created the holes is one way. I could also have only created and dimensioned one point, created one hole on that point and then rectangular patterned that hole. The nice thing with the sketch is that you can see the distances between the holes in one view without having to edit another feature.
Chamfers and fillets do not belong in sketches if the same effect can be achieved using 3D modeling features.
Again, keeps sketches simple etc.
Decorative chamfers and fillets are secondary or even tertiary features and should be applied as late in the timeline as possible. You never know ahead of time when you want to reference an edge of your model for example in another sketch for another feature. It helps if that edge doesn't have a fillet 😉
Generally mirroring and patterning (both should also be kept out of sketches) are powerful features, that when used wisely can significantly reduce the amount of modeling.
Fusion
