Fill in corner with wedge?

[AndreKR]

I found that this part breaks often along the blue line, so I though I'll make it stronger by filling in the corners as shown in red:

2019-02-14-01-53-33-FreeCAD.png (17.51 KiB) Viewed 1056 times

How to do that?

While I was writing this question I got the idea to trace and pad the polygon like this, and then draft it:

2019-02-14-01-56-08-FreeCAD.png (5.17 KiB) Viewed 1056 times

But I can't draft it because I can't select the neutral plane, or can I?

I can't just sketch another triangle onto it and then pocket it, either. That gives me:

2019-02-14-02-04-54-FreeCAD.png (10.14 KiB) Viewed 1052 times

[AndreKR]

I think I found a way.

I made two sketches like this:

2019-02-14-02-20-53-FreeCAD.png (4.84 KiB) Viewed 1050 times

And then I lofted the upper one through the lower one:

2019-02-14-02-21-14-FreeCAD.png (5.11 KiB) Viewed 1050 times

[NormandC]

Hi,

This Loft method succeeds, but I'm pretty sure it creates an invalid solid because the two sections being lofted share an edge. I suggest you check with Part CheckGeometry, it will probably confirm my suspicion.

What would produce a valid solid would be to make sketches front and back, since they wouldn't touch each other.

[AndreKR]

Hm, nope, 0 invalid shapes.

No issues converting it to a mesh either.

2019-02-14-23-08-47-dllhost.png (108.54 KiB) Viewed 1011 times

I attached the file, in case you like to play around with it.

But yes, your idea is better. I didn't remember that I can of course sketch "into the air".

[openBrain]

Hmmm, looks like NormandC guess right actually...

holder_chk_geom.png (16.59 KiB) Viewed 1008 times

[AndreKR]

Hm, strange.

2019-02-15-03-34-52-FreeCAD.png (5.85 KiB) Viewed 994 times

I tried this with Body001 selected, with AdditiveLoft001 selected and with Fillet001 selected.

Maybe it's because my FreeCAD is a few weeks old:

Code: Select all

OS: Windows 7
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.18.15619 (Git)
Build type: Release
Branch: master
Hash: 7d8e5662648b794b5c93e28835a2bf5c1fddffec -> 2019-01-11
Python version: 2.7.14
Qt version: 4.8.7
Coin version: 4.0.0a
OCC version: 7.2.0
Locale: German/Germany (de_DE)

[NormandC]

Maybe it's because my FreeCAD is a few weeks old:

No, it's because you haven't enabled the extra BOPCheck as detailed in the wiki page I previously linked.

But yes, your idea is better.

I just realized there's another way to get a valid solid, but while keeping your existing sketches: sink Sketch005 into the solid so its edge doesn't touch Sketch004 anymore. You can do that by editing its attachment offset and giving a Z offset of -0.01mm. (Warning: this will break your fillets, you'll have to repair them) You can do this directly in the Data tab, but I prefer to call up the Attachment dialog instead as I find it more user friendly:

1. Select Sketch005
2. In the Data tab, click on either the Map Mode or FlatFace fields
3. A [...]button appears to the right, click on it
4. The Attachment dialog appears in the Tasks tab.

Apart from that, I have a few suggestions about your model:

• For your first Pad, you should have checked "Symmetric to plane". Then you could have centred the ring in Sketch003 on the sketch horizontal axis. In my experience with parametric CAD, it is almost always best to centre your geometry on the model's origin.
• The Pocket001 was unnecessary, you could have created a PartDesign Mirrored feature of Pocket. Now here's where the first point about centring geometry to the origin becomes clear: with the ring and its post centred on the YZ_Plane, this would give you an easy mirror plane to select. As your model is, for the mirror plane, you would need to create first a datum plane (PartDesign Plane) attached to the YZ_Plane, and with a Z offset value to centre it on the ring (the X Y Z values are not calculated in reference to the global coordinates, but in reference to the referenced plane).
• Just as for Pocket001, the second AdditiveLoft001 and its 2 sketches were unnecessary, you could have created a PartDesign Mirrored feature of AdditiveLoft. Actually, you could have created a single Mirrored feature for both Pocket and AdditiveLoft.

Let me know if you have questions.

HTH,

Norm