Making a Router Cut on a Revolved Object

[dab]

Hi: I've been using FreeCAD for the last week or so and I'm really impressed. Most excellent work!

I'm trying to model a router (Porter-Cable, not Linksys) cut on a curved surface. I created a "spire" by revolving an arc, but now I'm stuck trying to figure out how to cut a channel on the curved surface of the spire. I expect the channel to have sides, more or less, normal to the surface of the spire, but it doesn't have to be completely accurate. Here's a drawing of what I would like; the red area is the channel:

spire.png (39.65 KiB) Viewed 1882 times

I've tried a few different things. Making it hollow and then making a rectanglar pocket from the flat face towards the tip gives the right shape, but the edges of the pocket are parallel to the axis of the revolution, not the surface. I tried a sweep, but I could not really figure out how to create lines on the surface of the spire.

I would appreciate some guidance.

Thanks,
Allen

OS: Ubuntu 14.04.1 LTS
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.15.4537 (Git)
Branch: master
Hash: 79173e37cd0886e197129bf06bfbee01890480b3
Python version: 2.7.6
Qt version: 4.8.6
Coin version: 4.0.0a
OCC version: 6.7.1

[NormandC]

Hello Allen,

Welcome here, and thanks for your well detailed post. It makes it pretty clear what you're trying to do.

Typically in other CAD software, there are tools to sketch geometry on curved surfaces, or failing that a way to project 2D geometry on a curved surface.

FreeCAD is still missing those tools, but I believe there is a workaround using the Part Section tool that is in the Part workbench's toolbar (inexplicably it's not found in the Part menu).

The idea is to produce two solids, and the Part Section tool generates a curve from the intersection of both solids. This would provide the required sweep path.

But the tricky part is to place a profile normal (perpendicular) to the Part Section. I tried to sweep it but FreeCAD hanged. I'm waiting a few minutes but may have to kill its process.

[NormandC]

I killed FreeCAD about a few minutes. Maybe the sweep would have succeeded if I had waited longer.

What worked though is a sweep with only one loop of the Part Section. Other sweeps would need to be done for the other path segments, and that means placing other profiles on the right positions.

About that, I noticed that the sweep is mostly normal to the spire's curvature only at the profile location (which I placed entirely visually, so it is not exactly perpendicular to the surface). Maybe you will have to make sweep with multiple profiles located at different points (at least at the ends and at the middle) to ensure the sweep is normal to the surface all around.

A word of warning to other users: I noticed Allen was using the development version of FreeCAD, which is why I used the new Sketcher Ellipse tool in Sketch001 under Pad. Attempting to open this file in FreeCAD 0.14.370x will crash the program.

I have deleted the Sweep I made, because then the file was too big to attach.

FC_dab_spire_01.png (36.47 KiB) Viewed 1862 times

FC_dab_spire_02.png (37.41 KiB) Viewed 1862 times

OS: Ubuntu 14.04.1 LTS
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.15.4537 (Git)
Branch: master
Hash: 79173e37cd0886e197129bf06bfbee01890480b3
Python version: 2.7.6
Qt version: 4.8.6
Coin version: 4.0.0a
OCC version: 6.7.1

[dab]

I killed FreeCAD about a few minutes. Maybe the sweep would have succeeded if I had waited longer.

Thanks so much for the pointer. I really appreciated it.

I was able to create the sweep along the longer edge of the slot, but the sweep along the shorter edge ran for an hour and still hadn't completed; so, I stopped it.

I tried another approach though, based on your section idea. Starting with half the pad, I was able to take the section edges and convert them into a face in "Part Create Shapes". Then I offset the face with "Part Offset". This didn't create a usable face for some reason; "Check geometry said it was an unclosed shell. But I took the edges from the offset surface and again made a face with "Part Create Shapes". Then I lofted between these two faces. And, with a little translation to move the surface of the loft out of the spire, I got my channel!

spire2.png (31.7 KiB) Viewed 1824 times

Yay! Thanks again.

[NormandC]

Cool! Glad you were able to get a satisfactory result.

Then I offset the face with "Part Offset". This didn't create a usable face for some reason; "Check geometry said it was an unclosed shell.

Yeah, I've been getting mixed results when I try using Part Offset. IMHO it should be able to create a valid enclosed shell out of a surface with the "fill offset" option checked, but I've never managed it. Maybe I should report it as a bug.

[dab]

Yeah, I've been getting mixed results when I try using Part Offset.

This is only tangentially related to offsets not producing shells. I was trying to drill a hole through the channel I lofted from the two faces (one from the section and the other from the offset). The sketcher would not let me use the end of my channel for a sketch because it was not a plane. Is there a query tool that lets you pick an entity and will tell you what kind of geometry OCC thinks it is?

Thanks,
Allen