This is my first attempt at a more complex part, and am learning as I am going. I am attempting to shell the part, but am receiving errors (That I frankly don't fully understand):
The yellow highlighted portions--are these the areas giving me the potential issues?
Thanks for any help!
Oh Geeze! I meant to include this rather relevant info in my first post!
I am trying to go 1.5mm shell, and shelling the entire assembly, such that it is pretty much all hollow. From my little experience with the shell command, the through holes should have shelled bosses around them automatically. I would like to exclude the flat base portion (I hope this nomenclature of mine is clear).
This will take quite a bit of effort to make a 1.5 mm shell work. For a model like this it would be best to use the rollback bar and try shelling at different stages in the model. I found that it will shell above the Fillet4 feature in the tree, but not after.
Thank you. So moving forward, I will shell at the end of each major operation, and see where I get stuck, and potentially amend the feature until the shell works. I appreciate the help troubleshooting, and for helping me get better at CAD!
Shelling is actually pretty complicated. Behind the scenes it creates offset surface, trims and extends to form a watertight surface and then thickens into a solid body.
Once you learn, you can use the diagnostics tools that are available if shell fails. Check body/faces will give you callouts identifying the issue(s). Go to Offset Surfaces will launch the Offset Surface command to see what surfaces it could not create.
That's great, thank you. I wasn't aware of the Error Diagnostics drop down. This will prove handy, as I am rather adept at generating errors!
I have tried a different approach, based on the above suggestions--namely, I am shelling or creating thin features as I go. This seems like a much more intelligent approach.
By rolling back to an early state and creating a lofted boss with a thin feature, I was able to successfully make the first manifold conduit. This feature was a sketch from a flat plane to another sketch on a flat plane. Great!
The second manifold conduit is proving to be problematic. I projected a sketch to create a curve on the first manifold conduit surfaces, and am attempting to create a lofted base, but am getting an error:
I also attempted an alternative approach, which was to make a lofted surface (this was successful), and then thicken the surface, but alas this also generates errors.
Any suggestions would be fantastic! Thanks!
Uncheck the option to merge results when you try to thicken the surfaces. You can then work on the issue it has with merging the two solid bodies after it thickens the surfaces.
Ok! This definitely moved me in the right direction, thank you.
BTW, I added the current V5 model above to the original post (I didn't immediately see how to add an attachment to the last comment)
How thick of a wall and what faces are you trying to remove if any?