[0.17] Align plane to cone wall

[salp]

I'm practicing by following the Reddit cad challenge https://www.reddit.com/r/cad/comments/6 ... llenge_23/ and I'm stuck creating the "B" Moderate exercise.

I created the cone and I don't seem to be able to align a plane to the sloped wall.
Up to now I've only created cylinders and I have been following the example of the "FC v0.17dev: Part Design Next Usecases and Best practices" of attaching the plane to the top and then moving it to the appropriate location. With the cone is it possible to attach the plane directly to the cone wall?

Thanks
Sal

23_Moderate.jpg (61.91 KiB) Viewed 2441 times

[NormandC]

Hi salp,

Those challenges seem fun.

With the cone is it possible to attach the plane directly to the cone wall?

Yes it is, with some limitations. When creating a Datum plane with no pre-selection, all the existing attachment modes are listed. There's a Tangent to Surface mode, its help tool tip mentions that a vertex and a face are needed.

In FreeCAD, cylindrical, conical and spherical faces have a split line, or "seam". So one of the cone wall seam vertices can be used. But I couldn't find how to make it work with the conical face. I could only make it work by selecting both vertices. I have no idea if this is a bug, or if it works as intended, but the help text is wrong.

FC017_DatumPlane_TangentToSurface_01.png (81.13 KiB) Viewed 2428 times

Now I thought that the Extra placement properties would allow to rotate the Datum plane on the Body's Z Axis, but it doesn't, or I didn't find how.

So you got a datum plane tangent to the conical face, but based on the blueprint, it's on the other side of where you want it (should be to the right of the YZ plane). So you got three options:

1. Leave it there, and work as if the part was rotated 180 degrees on its Z axis in reference to the blueprint;
2. Create somehow a datum line or a sketch on the XZ plane lying on the face of the conical face, so you have vertices to create your datum plane; I found no parametric way of doing that without resorting to expressions (too convoluted)
3. Realign the Revolution sketch so it starts on the other side of the YZ plane, so the conical seam will be on the right side. This is really simple: under the Sketch properties, toggle the Map Reverse property to true.

I would go with 3 because it will make your life easier when you create the ortho views in the TechDraw workbench.

Next problem is how to figure out the offset value from the conical face: in section D-D, where the heck is that 21.32 dimension attached to?!? The 11 dim makes just a little more sense but is not really useful either. It's a stupid way of dimensioning if you ask me...

Good luck!

[DeepSOIC]

In FreeCAD, cylindrical, conical and spherical faces have a split line, or "seam". So one of the cone wall seam vertices can be used. But I couldn't find how to make it work with the conical face. I could only make it work by selecting both vertices. I have no idea if this is a bug, or if it works as intended, but the help text is wrong.

It is a bug, another variant of it was reported recently for plane on three points mode.

[NormandC]

Well I was only looking at the projected view at the right and just now noticed that the whatchamacallit at 45 degrees from top view isn't a polar pattern of the other feature.

And with the revolution having created the cone empty, a tangent plane rotated 45 degrees is going to be required, with no obvious way of creating the necessary vertices.

I'll think about it...

[NormandC]

It is a bug

Cool, if it was reported for the 3-point mode, should I create a separate ticket?

[DeepSOIC]

Up to you. I don't remember if that bug was added to tracker...

[DeepSOIC]

https://forum.freecadweb.org/viewtopic.php?t=21738
Looks like there's no tracker ticket for it.

[salp]

NormandC thanks for the reply.

Your helpful as always.

Sal

[NormandC]

And with the revolution having created the cone empty, a tangent plane rotated 45 degrees is going to be required, with no obvious way of creating the necessary vertices.

Found it.

Datum point with "On edge" attachment mode. Just select a circular edge of the cone. By default the datum point is created at the start of the edge, which aligns with the seam. The datum point has a Map Path Parameter property that can have a value between 0 and 1, which corresponds to a ratio of the relative length along the edge. So to locate the datum at 225 degrees counterclockwise from the XY plane, I entered a simple expression (225/360) because I'm lazy.

Because of the mentioned bug, I had to create two datum points, one for each circular edge of the cone, I was then able to create a datum plane where I wanted it.

FC017_DatumPoint_OnEdge_01.png (120.41 KiB) Viewed 2390 times

Looks like there's no tracker ticket for it.

I'll try to record one over the weekend.

NormandC thanks for the reply.

Glad to help. Could you do me a favour, and edit your first post to add [0.17] to the start of your Subject? This way it's clear from the list of topics this is about the development version. Thanks.

[mario52]

hi
with my Macro Plane (not finished) select the "couture" and click

PlanToCone00.png (14.17 KiB) Viewed 2348 times

PlanToCone01.png (25.05 KiB) Viewed 2348 times

N23_Moderate01.FCStd

(25.26 KiB) Downloaded 32 times

mario