I am having a heck of a time creating a shell or swept cut for this piece, I have tried for hours, and have gained no progress could anyone lend a hand? The thickness is 3.25 mm.
Attached is the part file and pictures of the part
I am having a heck of a time creating a shell or swept cut for this piece, I have tried for hours, and have gained no progress could anyone lend a hand? The thickness is 3.25 mm.
Attached is the part file and pictures of the part
If you Split the model near the cross-rib, you can shell most of the part and Combine in later.
It is far from perfect and you need a lot more work. Especially at the tip.
One big tip:
Before you do any type of shell or thicken, check your minimum radius of curvature:
If the number you get is less than the amount you want to thicken or shell (and you are thickening toward the inside of the curvature) then you are going to run into problems.
You've got the multithickness faces selected wrong. You can't shell adjacent faces at different thicknesses if they are tangent to one another, so if you're going to use the multithickness shell, you have to have the fillet after the shell. Also, you've got to fillet the inside before you fillet the outside. The shell should be in the range of a couple of mm, not .2 and 10 where it was. Shell, Draft and Fillet are like Rock, Paper, Scissors. Silly game you can never really win without some luck.
Thomas Voetmann 's suggestion about splitting the body and shelling one side is perfect. It will enable you to use the cuts/ribs to shell the angular area. I've got the split body as a different color below.
I made it this one....but if I have a dim of reference maybe will be define it better....
A question, you will manufacture by injection of aluminum on a mould?
ömür tokman wrote:
he draws such interesting shapes beautifully.
I think that he is secretly a PJ Mask:
LoL
..close..
woooow.
this show was nice.
I was hoping you were going to do something...
OOoooo....
Weren't we going to say this?
Hi Chase,
You can't shell the main part like you want because as the error message states some of your current curves are already smaller than that as a radii.
Just a couple of observations.........
1) Your file size is very large considering the how basic the part is?
2) None of your sketches are fully defined which may lead to problems later.....
3) This model probably would have been done easier using surfacing features if you are familiar with those.
Totally up to you but I would consider re-creating this in a simpler fashion that yields more realistic identity to the real-life item.
Dave.