project cone geometry

[markreth]

I am creating a sheet metal cone with an access door. The original/main cone has a cutout in it for the door.  The cutout is then filled with a piece to create a relatively smooth continuous surface on the inside of the cone. 

Outside of the cone will be another portion of a cone (a couple inches bigger than the cutout) and will be made of rubber to act as a seal.  I have created the rubber on the outside of the cone, but am having trouble projecting geometry from the original cone and cutout to the rubber piece.  I created a work plane tangent to the cone surface in order to use the emboss function (which seems best suited for this application).  This is where I am stuck.

Outside of the rubber piece will be another piece of sheet metal to which clamps will be attached.

I have attached the file I am working on.  I tried using a work plane parallel to one of the origin XYZ planes.  The geometry projected better, but you can not use the emboss function, and the cut or extrude functions leave a beveled hole.  When I unfolded these to clean up the edges, the geometry got out of proportion quickly.

170905 is the assembly, 170906 is the rubber part I need to trim & put holes in.  Please let me know if these files work - I tried a pack & go, but it gave me a ipj file that didn't seem to do anything.  Pack & go and discussion forums are a bit new to me.

Thanks,

Mark

[johnsonshiue]

Hi! The assembly is incomplete. But, I think I still don't quite understand the design requirement here. Is 170906:1 the rubber part? Could you describe why you want to project the cone loop to XY plane here? For what purpose?

Thanks!

[markreth]

My apologies on the incompleteness; I guess I can only attach 3 files at a time.  Here are 3 more, the top ring is all that is missing, but probably insignificant to the problem.

170906 is the rubber piece.  170902 is a liner that goes on the inside of the rubber to make the surface of the inside of the cone as seamless as possible.  The goal here is to sandwich the rubber between two pieces of steel (170902 & another piece that has not been drawn yet).  The rubber piece and the outside steel piece will be cut 2.5" bigger than the opening on the main cone.  The "sandwhich" will be held together with some carraige bolts (the 5 holes on 170902).  Finally, the "sandwhich" assembly will be held to the cone with some clamps mounted to the outside of the cone.

My main problem has been effectively projecting the geometry from 170902 to 170906 so that I get the rubber (and eventually the outside steel piece) cut correctly to have a uniform overlap on the hole and get the bolt holes to line up.  I am open to suggestions; I am not sure that I am using the best plane or practices for this operation.

Thanks,  Mark

[johnsonshiue]

Hi! Please refrain from apologizing. You did not do anything wrong. I just want to get better understanding of the requirement and avoid any confusion. In terms of posting files here, you could zip up the files and post the zip instead of individual Inventor files.

I think I understand your requirement better now (at least than before). Have you considered creating each part as a solid body in a multi-solid body part. Then push each solid as a part using Make Components command. Are you familar with the workflow? Would it be easier than projecting edges from one part to another part.

Thanks!

[markreth]

Thanks for your input.  I am not familiar with multi solid body part path that you suggested.  I am going to look into that.

I actually had another suggestion come my way that I have been trying.  Part 170906 (rubber piece) was edited in place in the assembly.  I copied the face of the inside door (170902) with the copy object command (under modify).  Then the surface extend command was used to make the overall perimeter bigger.  Finally the thicken/offset command was used to cut the shape into the rubber (including the holes).

This appears to be successful; the flat patterns work out, holes line up, etc.  I am still working on finishing the design, but it appears to be going well and I am far enough into it, that a think it is going to work.

I have to give credit to Joanna from Imaginit for the input on this.

[markreth · Accepted solution]

I was out of the office for a few days - while working on this, I ran into a couple of issues with my previous solution.  I will attach the final layout I came up with. 

What I ended up doing was

1. Edit the part in place

2. use the copy object to copy the face of the door

3. then use the thicken command, but I only put in a small distance (0.1) to “engrave” the face

4. open the part up in its own window

5. unfold

6. project the geometry from the engraving, and sketch the geometry on that I needed and use the cut command

   1. note: when doing this, I had to leave a tab back to the original plane that was used to unfold in order to make the refold work correctly

7. sketch on the back side where the engraving was and extrude that to get the surface back to flat

8. refold

9. sketch on the surface (edge) where the tab was left for the refold, and trim it off with an extrusion

I think I caught all of the steps I did.  Part of the reason the previous method didn’t work was because the extend face did not extend the sides as they needed to be.  When working on a cone, the side cuts always have to form a straight line down to the theoretical point of the cone, otherwise they will be in a twist.  Sometimes that won’t matter, in this case, it was messing up the unfold operation and a couple other things I did later on.