Surfaces don't convert into solid
Sure. The dog that ate your homework probably also ran away with the sketches ?
I'll look at it later 😕
I took a look at this model (sorry if I stepped on toes, @TrippyLighting).
I can't say much about missing sketches, but there are a lot of sketches in this model:
Some are invisible. You can make them visible by just turning on the light bulb by the sketch.
About converting to solid: The problem here is really that your geometry is a bit messy near the top. If you zoom in close, you can see the problems. This is near the "top" of your model:
It's a bit hard to tell, but these surfaces do not line up well with each other. That's why they do not stitch together.
The root cause of this is the Boundary Patch features. With complex geometry (multi-curved surfaces), this feature generates pretty bad edges sometimes, that don't stitch together well.
You can get these to stitch together, if you specify a really big tolerance. But, this is a really bad idea. You might get it to work, but downstream operations (such as that fillet you want to do) will likely fail.
I did some experimentation with this, unstitching the solid, and hiding a few surfaces. With a big tolerance of 1 mm (again, not recommended), you can get all but a couple of edges to stitch (the red edges are not stitched):
So, unfortunately, I think you are going to have to take a different approach.
You might be able to make this geometry with a Loft feature. Or, create a Form feature and modify it to fit your shape. It depends on what your requirements are. How closely do you need to follow these curves?
Maybe @TrippyLighting has some additional suggestions?
Jeff
Jeff Strater
Engineering Director
He he. A little stressed are we ? Sorry for throwing a littel oil on the fire!
Don't worry, we've all been in in situations like that and have survived, and so will you.
The object you are attempting to design is really not at all a beginner object.
As Jeff has suggested, my first attempt would be to create one, or two solid lofts (Mode environment) as it is is easier to deal with. Let me see where I get with this tonight.
Tip 1. Try to avoid to leave sketches un-, or undefined. MAke sure everything is locked down either by a constraint or dimensions. YOu may not start that way, but you should end with fully defined sketches.
Tip 2. Try to avoid duplicate lines/arcs etc. ins skeches, particularly in these profiles used for surfacing, or lofting (which is what I am going to try). Again, make sure all the line/spline/curce end poins are snapped/constrained together.
More later.
Accepted solution
Yes, @Anonymous, you can make this work.
What I did was to stitch all the surfaces together, using a pretty high tolerance (.1 mm), but that's not too bad. Then, you can thicken this surface into a thin solid. If you are OK with making the top piece separate, you can use this workflow:
I was able to make this work for the top, but I was unable to use Combine to get the top and bottom into one piece.
Hope this helps
Jeff
Jeff Strater
Engineering Director
Accepted solution
No, Jeff has provided some temporay relieve, but if you ignore the advice I gave you in my last post you'll get into trouble again very fast!
If you make clean properly constrined and dimensioned sketches that will go a long way.
Some more tips, if you only need to have projected reference point, which I can see in some of your sketches, use project -> intersect. that will provide a projected reference point where a line/arc etc pierces throug a sketch plane. For lofts that is verry helpful.
I cleaned the file up some and create a loft. While lofting itself works fine, the surface it creates is rather ugly as sin. It has "smooth" transitions on the ridges of the pyramid, but I doubt overall it is what you're looking for.
Edit 1: Opps, forgot to attache the file 😉
Yes, you can do that. Just select fewer things to offset in the Thicken operation. Do it in two steps:
This ends up with separate bodies for the "handset" and the rest.
Jeff
Jeff Strater
Engineering Director
Here is another yet somewhat course approach just using a solid cutting away at it until it's a pyramid and then applied a G2 radius. It does not look too shabby for a first attempt.
Thats relly a very nice job on the foam prototypes.
For that model I believe that can be ver easily done with a split surface operation. Also, now that i've been thinking about it for a while I believe that mang this in the sculpt environment is the easiest and quickes way. I'll see if I can get a model and video up tonight.
Attached is the design entirely created from solids with split body based on the design sketches in your design. No need to do this with surfaces!
Glad it worked!
there are two folks that have helped you here. One is @jeff_strater and the other one is me @TrippyLighting and my name is actually Peter 😉
It would be great if one day you could help other users. I personally enjoy this as I get to solve problems theat I would not encounter in my own work.
A recommendation from my side for you would be to really review the training videos in the learn section. Then talk a look,at your initial design and see. How to improve it an learn how to use the different tools ink A Fusion 360 to your advantage. You mentioned that your sketches were stolen. If this is your own original design then continue to develop it to the point of a photorealistic rendering and use it to start a portfolio. That is something you cannot start early enough.
The design idea is very intriguing and has potential!