V0.19 Benchmarking--2019 Monthly Challenges #1,#2,#3,#4,#5,#6,#7a,#7b

[bambuko]

...Perhaps we need a separate Variables View panel instead of having to share the Property panel...

I hesitate making any recommendations because I don't (yet) really know enough about FreeCAD,
but I agree with you.

...we greybeards need to stick together

I would be honoured sticking together with you Sir

BTW have completed exercise #5 and only got stuck in two places.
Neither of them because of any problems with your descriptions...

One was my discovery of "Part Design - Refine" you must have used it without mentioning it and I was totally puzzled why my model didn't look like yours I suppose it goes back to your recommendation at the beginning of this thread:

...should be quite familiar with the PartDesign...

Another was when I tried to use mirror command... not exactly intuitive
I am used to learning by trying and following my intuition and helpful hints from the system, but...
with FreeCAD it seems, tutorials and wiki are the only way to learn

[Olav]

This is a really fun thread, I'm following along and doing the challenges myself. This concerns your #6 which is Fusion 360 Monthly Challenge July 2019 on Youtube:

This seemingly innocuous looking object is a bit difficult to envision how one should model it at first look. I have to admit I could not find a simple way to model this solely in PartDesign and had to resort to the 'Connect' tool in the Part workbench to complete it. Any port in a storm.

I think I cracked it, I made the entire thing in one body exclusively in Part Design.

And you're right, for such a little part it is surprisingly tricky.

The order of operations is important here. One would be tempted to create the flat bottom part of the part, then the angled upper part, then fill up the gap between them as a finishing touch - or even as an afterthought. Because how hard can it be. Of course FreeCAD won't let you because at second stage you would have two unconnected solids which isn't permissible in a Part design body.

So I made the gap filler thing before padding the angled thing, so that everything connects properly. I used datum planes to get the angles right and a named reference constraint in the first (bottom) sketch to be able to pad the filler to the right length.

From your post I took the lesson to choose the position of the origin wisely because it makes wrestling the datum planes into position a lot easier.

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Dependency graph looks fairly clean to me. Sketch001 uses external geometry from Sketch, which could be a weakness:

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Also: thank you, ppemawm, for setting a good example for this FreeCAD student and without doubt, a lot of others. I believe that while the developers are working hard to make the program itself better, us users should learn to make the best use of it. Cheers!

[ppemawm]

I made the entire thing in one body exclusively in Part Design.

Wow, nicely done. I have learned something new.
Nice touch using the named reference dimension in the first sketch.
(Note, however, there is a missing angle constraint, 45 deg, in Sketch002.)

Now that I think about it you can probably do it (Pad001) with a 45 revolve by selecting the angled end face of the bottom part and using the reference edge as an axis. As always, there are several ways to do it.

Your result is a robust model which I tested by changing the radius of the bottom part and the thicknesses.
A model is only a good as it can be changed without breaking.

BTW I rarely use datum planes (other than for mirrors) unless multiple sketches are attached to them. As you probably know, any sketch can be attached in the same manner as a datum plane. Datum planes do, however, provide a nice visual when modelling.

[Olav]

I made the entire thing in one body exclusively in Part Design.

Wow, nicely done. I have learned something new.
Nice touch using the named reference dimension in the first sketch.

Thank you.

(Note, however, there is a missing angle constraint, 45 deg, in Sketch002.)

Well spotted. I think I was playing with that sketch a bit and forgot to put the angle back in before saving and uploading. It certainly was there when I was making the part.

Now that I think about it you can probably do it (Pad001) with a 45 revolve by selecting the angled end face of the bottom part and using the reference edge as an axis. As always, there are several ways to do it.

I think I would like to see this. I can't very well imagine how you would do that.

BTW I rarely use datum planes (other than for mirrors) unless multiple sketches are attached to them. As you probably know, any sketch can be attached in the same manner as a datum plane. Datum planes do, however, provide a nice visual when modelling.

I know. And in a way I find them just convenient. In some cases I start out modelling by putting my datum planes in place before doing anything else. That way I don't have to think about positioning the sketches anymore. If you would argue that the planes are redundant and clutter up the model tree too much, I can certainly see that. I haven't decided or settled the argument for myself yet.

[Olav]

Now that I think about it you can probably do it (Pad001) with a 45 revolve by selecting the angled end face of the bottom part and using the reference edge as an axis. As always, there are several ways to do it.

I think I would like to see this. I can't very well imagine how you would do that.

Never mind. I just tried it and... it works! And it simplifies the whole model considerably, no more clever tricks needed. Great solution.

Also, I only just found out that I can delete a datum plane that I attached a sketch to, and the sketch will retain its placement. Neat.

I'm not sure we can optimise this any further.

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[kisolre]

Does this qualify for the challenge? Create extra material, remove the excess...
.

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