Lofting a Hollow Object

[apostM2K9B]

Hey Thrill Seekers,

From what I can tell, it looks like what I want to do can't be done in Fusion 360.  I'm trying to create a light weight propeller duct.  The end result is a section of cone, with hollow tubes cut through the wall of the cone to keep weight to a minimum.  As you can see in the sketch below, the tops and bottoms are two circles each with 100 smaller circles to create the voids/tubes.  When I select the bottom and tops (as though I was going to extrude) F360 shows my selections like we're on the same page.  But the loft operation creates one big solid.  

My work around would be to loft the solid, use the center circles to cut it out, then loft ONE of the voids, extrude a base for it, then create a circular pattern of it and use that as a tool to cut out.  

Is there an easier way?

[jeff_strater]

no, there is no easier way, unfortunately.  Loft cannot handle hollow profiles (even if they are hollow on both ends).  It's just a limitation of the loft geometry engine.

[apostM2K9B]

My work around isn't working either.  I created this tool and tried to combine/cut it with the cone shell and F360 started to whine about bodies being nearly coincident.  

Any brainstorms?

[apostM2K9B]

Can you share any parameters about how close the edges can be in order to work past the error message I get with my work around?  I'd rather compromise/change my concept than have to loft 100 voids one at a time.  

[TheCADWhisperer]

File >Export and then Attach your *.f3d file here.

[apostM2K9B]

I've attached the file as you suggested.  Before I scaled this up, I had created a small 3mm tall test ring that included all 100 circular voids to check my sizing.  It was a simple extrude and worked well.  

As it stands now, I'm just going to loft 1/4 of the voids then split the body into quarters and create a circular pattern out of the section to make a whole.  

I would of course welcome the opportunity to see that I've been exercising my God given right to be dead wrong and learn a better way.  

Share your thoughts,  

[TheCADWhisperer]

---

@apostM2K9B wrote:

 The end result is a section of cone, with hollow tubes cut through the wall of the cone to keep weight to a minimum. 

---

How will this part be manufactured in the real world - only by 3D printing?

The reason I ask is the method you have used to Loft the holes is not correct for drilled holes.

Also - use symmetry about the Origin, keep your sketches simple and fully define your sketches.

[apostM2K9B]

The funkyness continues.  I tried cutting 10 holes, split the body, created a circular pattern of 10, combined the bodies.  The resulting single body still displayed lines between sections instead of one smooth cone section.  

On printing the piece, something was hosed with the code as it displayed correctly, but printed a sort 5-ish degree section then half the cone.  I abandoned that.

I then tried cutting two more holes and splitting the piece into a wider section, then manually copied and rotated it 39.6 degrees each so that I was certain, the pieces overlapped.  Combining them still left the telltale joints and the print was the same.  

I tried a test on the uncut body and it seems to want to print the entire circle.  

Looks like I"m going to have to manually loft all 100 holes just to get a test print.  Unless there is something I don't know, it seems like a pretty serious short coming.  

[TheCADWhisperer · Accepted solution]

---

@apostM2K9B wrote:

...it seems like a pretty serious short coming.  

---

Examine the Attached file.

One simple sketch.

Four Three simple features.

Done!

You didn't answer my previous questions?

[apostM2K9B]

OMG...You da boss!  Features for crying out loud.  Thank you thank you thank you.   

[chrisplyler]

I've assumed you would like the overall wall thickness to taper with the holes, such that the amount of material AROUND the holes is constant. Adapt as necessary if you would rather the overall wall thickness remain constant.

Watch this video, which I've prepared especially for you. I know it's long. I went all the way through from the blank file to completion, so you can see everything. Watch it slowly. If at any point you don't understand something, rewind a bit and re-watch.

Please note:

1. I did not make a solid body that would then be used as a void. Instead I just loft/cut a hole, and then patterned that feature around.

2. The lines I used to set up an angle for the hole have that angle defined as 360deg/hole_quantity, so that I can later match the pattern quantity to that value, and the pattern holes will space around appropriately. Later on in the video, I go back and parameterize this.

3. My sketches are fully constrained, and control the desired thicknesses, height, and hole placement as desired, so I can just edit the dimension values (or parameter values) and change whatever I want.

4. I decided to drive it via the two outside diameters, the number of holes, and the amount of meat between the holes. The two inside diameters and the hole sizes themselves are handled automatically based on those driving conditions. If you want to control the hole sizes instead or whatever, adapt it accordingly.

https://knowledge.autodesk.com/community/screencast/d7a14257-ffbd-4fdc-a036-03b1b25ae420