I am trying to shell partially a part. The picture in attachment shows the section view of the part. I want to shell only what is below the red line. How can I achieve this ?
1. Model correctly from the start (always works).
2. Split the body into multiple bodies, shell the desired body and then Combine (sometimes works, if you can define a split line (surface).
I would probably start over from scratch using what I learned from the first attempt unless the split is easy.
I can try if you can attach your part file.
I can not attach file online for NDA reason.
Do you want to keep a wall thickness where your red line is? must the 2 chamfers in red remain as drawn also?
What I want is the shell function to shell surface which are below the red line. What is above the red line I don't want the shell function to shell.
Ok, that's a bit vague. But you might get what you are after but creating a surface (revolved perhaps) that isolates the geometry you do not want shelled. Split the body. Shell the body you want shelled, then combine the bodies.
If the Shell thickness is bigger than the wall thickness then it will bypass the area above the red line. Not sure of the scale of your part or the wall tickness or the Shell thickness you need, see below.
Or you could change the order of your features, shell the part & have the thin section after the shell.
Currently the thickness of the shell I want to do is 5mm and the distance is 6mm....
It means I need to trick my geometry before passing with the shell function... then to enlarge the distance later..
A multi-thickness shell might work also.
I tired already but seems it didn't work.
Not sure if this will work or not, but I would try to use an offset surface, then thicken it and delete the body..
My current shape to shell is much too complex to use off set surface option I think. We have many face and I can not trim them all...
2./ is what I was thinking to do. Based on my initiall understading, the shell feature should have been applied at the end when finally all my part is designed. Thinking about it more, I understand now that I should apply the shell function when the shape is still enough simple so the feature can pass on the body, then start to add all the detail manually on the top of the shell...
I forgot Option #3.
If the part was otherwise modeled correctly - drag the rollup bar up the feature tree to where the Shell feature should have been added.
Add the Shell and then drag the rollup bar back down.
why not try the cut extrude, to cut revolve?
Then again there is nothing wrong with starting over with a thin revolve or some other modeling techniques mentioned above.
many times it takes getting to the drawing stage to get a clean idea on a 2 feature part that took 85 features to design.
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