hey,
So I'm trying to shell out this part, but its leaving a thickness is this side.. as you can see its not shelling up along the face but its just bridging across and leaving that thick piece. I've attached my file to this. can anyone help me with this please?
Kind regards,
Luke Brient
hey kelvin,
Thanks for the reply! i did indeed, but im not really sure what to do about that/ how to fix it?
regards,
luke brient
Hi Luke,
I think your problem starts up at Boundary surface 14. You've created a 3d sketch of the two edges, but this is giving you a surface where it doesn't meet the edges of the other surfaces. I'd rollback above the boundary, and trim the lower surface using an new sketch on plane 2 with an offset from your sketch 48.
Then edit boundary surface 14, hide sketches, delete the direction 2 selections, and use the selection manager to select the surface edges instead.
This will cause a few minor errors mainly in sketches you can easiliy fix.
however looking at boundary 15, you can use the same approach, trim the surface so you have a set of edges.
Change sketch 62 so its now coincident with the new edge
Tweek boundary 15 to reference edges
delete surface trim 21.
These surfaces will now knit nicely. You'll need to fix some of the other features though.
Do all symetrical geometry before mirror 6.
Thank you very much!! this has worked very well, very detailed feedback!!!
kind regards,
luke brient
No problem Luke, glad to help.
hi, sorry i didn't fully check when i replied saying it was fixed.
i did all of your above steps which trimmed it down and made it alot cleaner, but then again when i come to shell it i have the same issue with it not following that curvature. this is preventing me when splitting the part and adding groove/ lip through plane 2.
any ideas?
cheers,
Luke Brient
Can you attach the part again as it is now?
its attached here
It's not liking the sharp transition between boundary 1 to boundary 2. Rollback before the mirror and put a small rad on the edge.
After that life is sweet.
PS, that's not uncommon on an edge that transitions from going inward to outward.
brilliant thank u very much for all your help!
But now that i have this radius on the edge, the split tool wont cut the body in 2 through plane 2, how can i get round this?
Delete the rad. Delete Shell, use plane 2 to split the part (do not consume selected bodies). Isolate bottom body (RMB Isolate) Select top and bottom faces and shell. exit isolate. Shell top body. Combine bodies.
Did you not see this message when using the Shell feature?