boring (lofting?) a tapered hole into a thick cylinder

[jnberando]

It will likely be obvious that I'm a beginner with no CAD training. There seems to be many ways to approach what I want to do, but I haven't been able to get any of them to work.

1. What I want to do:

I have what is essentially a cylinder with 7mm-thick walls.

I want to bore holes in the cylinder so that they are smaller on the surface and open up into the bore.

For example, a hole would be 8mm on the outer surface, and taper out to 12mm as it enters the inside.

I have attached screen shots that show the cylinder with sketches projected onto it, and another that shows what the hole should look like, were it to have positive volume.

2. What I've tried:

A. I tried using the cylinder as a grouping of hollow surfaces, then projected an 8mm circle sketch onto the outside surface, and a 12mm circle onto the inside. However, the projected sketch was not usable as a loft parameter... So I took the advice of someone else on this forum, and patched the two circles, then used those as the basis for the loft. I created a new loft surface successfully. I then deleted the patches, and attempted to use the loft as a tool to cut out the hole shapes in the surface, but I wasn't able to do it. So...

B. I made the cylinder into a solid, and again tried to use a solid loft to cut a hole, similar to the above process except that the solid version of the loft function allows a cut. However, I still had to patch the circles first, and the loft appeared to "work," except the result was that I still had a solid cylinder with no holes.

C. I tried to use the lofted surfaces from (A) to split the solid body and then remove the hole, but that didn't work either. I also used the extrude function directly from the sketch and successfully made a straight hole, but this of course does not meet my objective.

D. After trying many other things and wasting an entire day, I decided to ask for help. I should have done this at the beginning, but I expected it to be simple. It probably is, but in a way that I'm not aware of.

Conclusion: Please teach me if you can. I'm not attached to any particular way of doing this, so maybe there is another approach that I'm not aware of. Thanks in advance.

[Warmingup1953]

You could do it in Sheetmetal but there will be an easier way...(after a Coffee break!)

[Warmingup1953]

What OD?

[Warmingup1953]

...and there was an easier way! I created Drill holes so to speak.

[jnberando]

Thanks - but in this case, it looks like I can't use sheet metal, as the body doesn't have a uniform thickness. This is actually a piece of bamboo that I molded using a 3d scan.

[jnberando]

This looks promising... So you're using a cut plane?

[Warmingup1953 · Accepted solution]

Yes, I extruded the 12mm sketch from the inside out through the Pipe as a new Body then the 8mm Sketch from the outside again new body then I Combine Intersect both with the pipe to get a profile on the inside (of a 12mm "Hole) and the 8mm outside and then lofted the two profiles to create the tapered plug. Others I'm sure will do it simpler!

[jnberando · Accepted solution]

Great! I ended up doing it perhaps slightly differently, but your hint got me going. It looks like the reason that it wasn't working for me is that the edges of the hole body that I was creating were flush with / too close to the target cylinder to be able to combine. With your inspiration, I did the following:

1. project sketches of 8mm circle to outside, 12mm circle inside.

2. extrude each 1mm in either direction so that they are not flush with the surface.

3. loft the hole sketches, then patch either end of the extrusion and stitch it all together to make a solid body

4. combine / cut the hole body and cylinder body to form a happy hole!

After so many hours, this hole is very satisfying. Thanks so much!!

[TheCADWhisperer]

@jnberando 

Wouldn't Revolve - Cut be much easier?

Attach your file here if you can’t figure it out.

[davebYYPCU]

Beat me to it.....

[TheCADWhisperer]

---

@davebYYPCU wrote:

Beat me to it.....

---

I would guess that is how it would be done in the real world.

We’ll see if the OP attaches geometry.

[davebYYPCU]

Don’t need a file, 

Section with Offset Plane.

Draw an unconstrained rectangle, dimension two ends, 4 and 6 respectively, align as required.

Might help....