Offset Face or Push pull not working

[danFL2NZ]

I would like to offset the faces of this assembly. Ideally i would like the three separate boundries to be different depths. I have created the splitting lines but cant get the offset face or the push pull command to do what i would like. 

[laughingcreek]

The surface quality of this is pretty bad.  I wouldn't expect to be able to do much off anything with it along the lines of offset faces.  You have to have pretty good surfaces to start with for those tools to work-

trouble seems to have started from in the second sketch from the offset of that projected sketch, probably went down hill from there.  Haven't checked the rest of the model-

[ritste20]

I 've tried to go through and clean up this model and I hate to say it but there is a lot going on here that could be causing problems. When I opened the modeled as downloaded, there were rebuild errors due to undefined or poorly defined sketch geometry. I tried to work with what the OP had for geometry. This isn't perfect by any means but maybe this is good enough for someone to answer the original question as to why you can't manipulate the individual faces.

[danFL2NZ]

Okay great, Thanks for looking. How did you get to analyze the sketch like that for future reference. So i know to check ahead of asking for help

[danFL2NZ]

Ill try this new file this morning. I appreciate you checkng it out. Very new to fusion and im working off a laser scan of the car. Big learning curve!!! But you dont learn if you dont ask for help...

[ritste20]

Laser scans can be great but they often give you way more data than you need. If this is something you plan to do on a regular basis I would concentrate very hard on cleaning up the mesh before you jump into modeling something from the scan. That will go a long way in avoiding pitfalls down the road with a lot of time invested in manipulating your model.

My advice would be to look at your scan mesh, pick out the relevant points (corners, mounting holes, basic form control points), and create construction geometry at those locations. Then turn off the mesh and build your model the right way from the ground up. This will give you better control over the geometry and the tools at your disposal will react the way you want them to, more often than not.

[ritste20]

https://forums.autodesk.com/t5/fusion-360-design-validate/geometry-101-geometry-is-geometry-even-on-...

Check out this post and video from @TheCADWhisperer. In parametric modeling software like Fusion or Inventor, literally everything hinges on how well you as the operator define your sketch geometry and construction geometry.

It takes practice and there is no magic formula for how to model your parts. Each tool offers different functionality and by learning how each one operates it will allow you to define your sketches in the most appropriate way for your specific scenario.

But there are very few circumstances where underdefined sketches should be the norm

[TrippyLighting]

I can see the thought process behind your workflow and in general, the concept is solid, but the techniques and tools used to create geometry are fraught with problems.

The key to good geometry, as others have mentioned already, is good curves. In Fusion 360 hat means sketches.

You re-meshed your triangulated scan data into a quad mesh.

Then that quad mesh was imported into Fusion 360 converted into a T-spline and then  NURBS surface.

The NURBS surface was used to create an intersection sketch, to get a base profile.

One problem is that the dense mesh is full of poles (star points in T-Spline lingo ) which creates curvature problems, particularly when a sketch intersection is created at such a point.

For surfacing projects, I stay almost completely away from sketch projections of any sort and almost completely work with surface edges.

A better workflow and with a bit experience likely less a laborious one is to simply import the triangulated mesh and create a mesh section sketch.

That sketch you then use as a visual guideline only to start building a nice smooth curve.

Start with a 3-degree one and see if that works. Then maybe upgrade to a 5-degree curve.
Does not work either? Maybe use a fit point spline. Always toggle on the curvature comb display when creating such spline curves.

I recently helped another user in with another tail light and demonstrated the technique for him in a screencast:

[danFL2NZ]

Okay, that was spectacular!! I think i learned more watching that video than hours of messing about by myself. Clearly i have alot to learn but that was excellent help. I didn't realize the mesh section sketch until this video. I was trying to use the mesh as essentially a cut tool to capture the profile.  I now understand how mush that actually complicates things. Im going to start over with this method and see what i can come up with. Could i create that surface as you demonstrated it than just use thicken to get my bezel thickness? Honestly the user community is an excellent resource. You guys are awesome!!