when i try sketching on an angled offset plane, the sketch doesnt stay on that plane.

[quincyjacobs17]

I'm not sure if this is even the right place to ask this, its my first time actually interacting with the community. I'm relatively new to the program. But I've been having this issue where i set a 10 degree construction plane, and draw my sketch on it. then when editing that sketch, none of the lines seem to ever want to stay on that plane and will move about freely. its so slight that I never even notice until I'm a bunch of steps down the line, and am having issues because of it. (I know this is my fault for not realizing that none of the shapes turned blue to show a closed profile before moving on) if I view the design from the side and zoom in super far, I can see all the different lines are actually not all level with each other. making it so that the surface i create out of it doesn't register as a flat surface to draw sketches on, and wont register any closed shapes to extrude or anything because of it. 

I've been trying to find any kind of way to go back and edit the sketch to select all the lines and see if I could like snap them all to be flat on the construction plane again somehow but I haven't been able to find anything or figure anything out. I thought maybe there would be a command similar to the align feature where u can select 2 faces of separate solid bodies and make them flush with each other. does anything like that exist? or do I actually have to completely redo all of the steps I did after fixing the sketch? I noticed if all I do is adjust existing lines things will update down the line without a problem, but if I delete any of the lines I used for the patch commands and redraw them it requires me to edit all my features. which is completely understandable. I just don't see any possible way to fix all of those lines back down onto the plane that they were originally drawn on. I don't wanna have to completely redo it all. There's got to be a simple fix to this right? I feel like I'm missing something here.

Its not the end to the world if I have to redo it all again I guess but I'm curious if anyone has any ideas for how to either prevent this in the future or fix it in an easy way?

[jhackney1972]

Please attach your problem model.  Open in Fusion 360, select the File menu then the Export command and save to your hard drive.  Attach it to a reply post using the attachment section.

[TheCADWhisperer]

Do you have 3D sketching disabled?

Are there any unresolved issues highlighted in the Timeline?

[TheCADWhisperer · Accepted solution]

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@quincyjacobs17 wrote:

I just don't see any possible way to fix all of those lines back down onto the plane that they were originally drawn on.
There's got to be a simple fix to this right?

I feel like I'm missing something here.

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Right click and select Redefine Sketch Plane (or something like that, I am not at my Fusion machine at the moment).

[davebYYPCU]

With only that sketch visible, Edit sketch, 3d sketching turned off, 

window select all articles, right click, select Move to sketch Plane, 

Might help.....

[quincyjacobs17]

Okay i will have to try looking into that when i get home from work tonight thanks

[quincyjacobs17]

ah, okay I don't know how I missed that. I swear I've tried looking at all kinds of right click menus. lol

but, apparently that didn't solve my issue because it automatically says "failed to resolve" the second i try selecting any of the lines. 

[quincyjacobs17]

how do i check if 3d sketching is disabled?

edit: sorry, nevermind i found the option on the right side of the screen in the sketch palette

[quincyjacobs17]

thats the kind of option i was looking for, but it just instantly says failed to resolve the second i click move to sketch plane 

[davebYYPCU]

Visibility Eyeball turned on for just the single problem sketch.

All other eyeballs for other sketches and bodies and unrelated components turned off.

Now do you have all of the sketch articles that should be there?

Sounds to me like you have multiple sketches involved.

Might help....

[TheCADWhisperer]

Can you File>Export your *.f3d file to your local drive and then Attach it here to a Reply and end all doubt.

You didn’t answer my question about, “Are there any unresolved (and apparently ignored) issues highlighted (in yellow or red) in your Timeline?

Is this your first project? I would recommend starting with several more simple projects and mastering sketch techniques before tackling a design of this complexity.

[quincyjacobs17]

Sorry, I just figured it out now so there's no need at this point. I work long shifts at work and wasn't able to get back to my computer until now. I have a few issues in the timeline but on completely separate sketches involving the body design. so I doubt that had anything to do with it.  Ive done multiple complete 3d models of various guitar designs that designed. I've just never ran into this issue before. ill admit I don't know nearly as much as I should, but so far I've been able to create models and successfully generate CAM files for my CNC router to help me build. so I know just enough to be able to do what I intend to (for the most part anyway lol)

The Fix: for whatever reason, the fact that there were coincidences within the sketch is what was causing the error with the "move to sketch plane" command. I deleted all coincidences and then it worked just fine. now I have all closed profiles which is exactly what I needed. 

[quincyjacobs17]

I did have 3d sketch enabled. i figured it out now though, the "move to sketch plane" only worked after deleting all coincidences within the sketch. thanks anyway for trying to help i appreciate it

[TheCADWhisperer]

For future reference - if you want to improve your sketching/modeling techniques in an efficient way - whenever you get an issue highlighted in your Timeline you should immediately STOP, undo what you just did to cause the issue and ask questions here about best technique to avoid or resolve the issue.  I have seen these issues left unresolved result in “digging a deeper and deeper hole” not to mention loss of efficiency in modeling.