Creating precise curved sketches on tube

[jhaand]

I had quite the challenge to make a bayonet fitting in FreeCAD. The Bayonet fitting is easy to make with a rotary milling cutter. As you can see below in the supplied STEP file.

bayonet_interfac_bottom.png (75.4 KiB) Viewed 2551 times

However creating a model that fits was quite difficult with the Part Design workbench. Since I need to sketch on both on a cylinder, but also keep the angles in check. One option was to use the curves toolbox then I could draw curves on the cylinder, but making sure the angels were correct or import them in the sketch would almost be impossible.
In the end I did the following:

• Make a sketch with each piece on a new datum plane,
• Do a revolve for the appropriate angle.
• Then add another sketch with revolve until the shape is finished.
• For the other 3 items, do a polar pattern around the vertical axis.
• In order to make the curved shape to fit the metal I made fillets on the protruding ends.

However, I couldn't make fillets in the enclosed corner. Fortunately I could live without that.
With the following result:

bayonet_interface.png (53.77 KiB) Viewed 2551 times

This actually fitted after 3D printing the part.

I can imaging there would be an easier method and I would like to here what a good method would look like.
Any suggestions?

[chrisb]

For such use cases addon workbench Curves with its "Map sketch to surface" can be very helpful.

[jhaand]

Thank you for pointing this out.

I was thinking the "Map sketch to surface tool" would work, but had some doubts about converting the angles to millimeters. But since I know the exact diameter of the surface I make the sketch on, this will actually remain very precise. I just need to calculate the factor of degrees per millimeter once and that's it.

I will try it again this way.

[jhaand]

I tried again by using the Curves workbench using the tool "Map a sketch on a surface". I hoped this tool created a new sketch which could interact with Body that I already had in the Part Design workbench. But unfortunately this tool creates a new object and you need to use the Part workbench to tie everything together.

Final result.

bayonet_curved.png (91.77 KiB) Viewed 2343 times

Since the diameter was fixed, I was able to translate the angle to millimeters and it all looks quite nice. So with a diameter of a sketch the distance becomes: angle / 360 * pi * 70

This was a bit more work because I couldn't use the polar pattern form the Part Design workbench. So I had to draw all the 4 hooks separately.

The sketch looks something like this and my computer has some trouble computing a solution for all this. But it still works nice.

Sketch used to create bayonet interface

bayonet_curved_sketch.png (85.47 KiB) Viewed 2343 times

I also attached the FreeCAD file if people want to see how to do this.
We'll see next week if it fits when it gets out of the 3D-printer.

[hammax]

... trying to do this job by experimenting with Facebinder tool.
From the sight of the milling tool...

Bayonet.PNG (37.03 KiB) Viewed 2285 times

[papyblaise]

i guess the cross hole should be circular not oval
it should not be included in a sketch on surface, but a pocket before

[papyblaise]

it is easier to dress teeth as on a crown, and this allows to orient the faces as if they were cut on a CNC taking into account the diameter of the tool,
and the hole is very round

[M4x]

This was a bit more work because I couldn't use the polar pattern form the Part Design workbench. So I had to draw all the 4 hooks separately.

Are you aware of https://github.com/DeepSOIC/Lattice2/wi ... olarArray2 and Draft_PolarArray?

[jhaand]

... trying to do this job by experimenting with Facebinder tool.
From the sight of the milling tool...

Bayonet.PNG

This looks like a method that might work. You even simulate the drill bit of the CNC router.

After looking at the drawing of the interface and your FreeCAD file, I see a problem.
According to the drawing, the walls of the cut need to point to the center of the tube.
In your FreeCAD file the center of the drill points to the center. In this case the bayonet would not fit the interface.

bayonet_wrong_angle.png (13.06 KiB) Viewed 2109 times

edit: Adding info on pointing the side of the drill to the center of the tube.

[jhaand]

This was a bit more work because I couldn't use the polar pattern form the Part Design workbench. So I had to draw all the 4 hooks separately.

Are you aware of https://github.com/DeepSOIC/Lattice2/wi ... olarArray2 and Draft_PolarArray?

I didn't know them and that you could use the draft workbench for 3D objects.
That looks very interesting.
I need to get a better understanding of the Draft workbench.

On a different note. Would it be possible to use Lattice2 to create reinforced ribs for injection molding?
Because I was wondering how you would do that using FreeCAD. Especially if you use a honeycomb pattern.