topic Re: Moving Lines Help in Fusion Design, Validate & Document Forum

Moving Lines Help

skypilot65 — Mon, 04 Sep 2023 00:20:28 GMT

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

Re: Moving Lines Help

davebYYPCU — Mon, 04 Sep 2023 00:51:38 GMT

Too many ways to get there, depends on what is actually in your file.

Re: Moving Lines Help

skypilot65 — Mon, 04 Sep 2023 00:59:20 GMT

Too many ways to get there? Depends on what's in the file? Cryptic responses like this are not at all helpful for a Fusion 360 newbie!

I will ask again. How do I move each line 15mm to the left? Thanks.

Re: Moving Lines Help

davebYYPCU — Mon, 04 Sep 2023 01:05:12 GMT

What can I say, I can't tell you what to do, only guess.

move this to 15mm left.

Is there a Sketch,

Change the dimension, if there is no dimension make one, if there is no sketch,

etc.

Re: Moving Lines Help

jeff_strater — Mon, 04 Sep 2023 01:24:24 GMT

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.

Re: Moving Lines Help

skypilot65 — Mon, 04 Sep 2023 02:14:21 GMT

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.

Re: Moving Lines Help

davebYYPCU — Mon, 04 Sep 2023 02:53:43 GMT

Hack bandaid is OK?

If there was a sketch, you should have edited the sketch.

Might help....

Re: Moving Lines Help

TrippyLighting — Mon, 04 Sep 2023 09:54:59 GMT

@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!

Re: Moving Lines Help

TheCADWhisperer — Mon, 04 Sep 2023 10:26:24 GMT

@skypilot65 wrote:
Any help would be greatly appreciated.
Kent

@skypilot65

After 3 years - it is time to learn how to do this correctly.

Attach your file here for demonstration of correct technique.

Re: Moving Lines Help

skypilot65 — Mon, 04 Sep 2023 14:25:45 GMT

Ok, I surrender. Here is the file.

I want to make something very clear. I am not a professional designer. I use F360 to do 3D printing as a hobby. I've never taken any professional training, but what I have learned over the years by "playing" around with a system teaches me more than reading from a manual or listening to a YouTube video. When I get stumped like this I ask for help. Typically, the community is very supportive, but in some of the responses in this thread its more of a beating, like I should know better to ask such a simple question. Maybe I should've, but as you can see I was working from the 2D view trying to move the line(s) to expand the hole size (most folks would think this would be a logical thing to do).

I apologize to all those experts out there for asking such stupid questions. I won't post here again.

Re: Moving Lines Help

skypilot65 — Mon, 04 Sep 2023 14:54:38 GMT

Here is the file.

Re: Moving Lines Help

TrippyLighting — Mon, 04 Sep 2023 16:11:02 GMT

@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 😉

Re: Moving Lines Help

TrippyLighting — Mon, 04 Sep 2023 16:40:12 GMT

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.

Re: Moving Lines Help

skypilot65 — Mon, 04 Sep 2023 17:29:23 GMT

Thank you. I have made the changes under the preferences and will from now on try to center up the design.

Re: Moving Lines Help

TrippyLighting — Mon, 04 Sep 2023 19:07:37 GMT

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 ).

Re: Moving Lines Help

skypilot65 — Mon, 04 Sep 2023 19:27:02 GMT

Will do. Thank you very much.

Re: Moving Lines Help

skypilot65 — Mon, 04 Sep 2023 20:11:28 GMT

@TrippyLighting Wow! You make it look down right easy. Clearly there are a lot of additional steps in my version that were unnecessary. So, by placing the origin were you did, it allowed you to split the overall design in half using "Sketch 2" to act as the mirror for the final step to transfer "Sketch4". Is that right? You also used the "Chamfer" feature to create the corner elements of the openings versus the "Line" tool like I did (lesson learned). I'm not quite sure why you used the "OffsetFaces1" ? Was it to project the "Sketch2" image on each side so that you could perform the extrude for the opening on the sides or am I missing something else? The "Hole Location" sketch was used as a guide where each corner was the center point for each hole (I like it, lesson learned). The "Sketch4" defined the location of the other openings from which you simply "Chamfered" the corners again and used the "Fillet" operation to round over the edges.

Let me know. Thanks again!

Re: Moving Lines Help

TrippyLighting — Mon, 04 Sep 2023 21:08:27 GMT

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.