Series of articles about the pitfalls of parametric editing

[arcol]

Right now and for the past few months I've refrained from posting any elaborate video tutorials, knowing that with the Body container and working planes, the Part Design work flow will drastically change. All of the current FreeCAD videos focusing on Part Design found on YouTube will basically be obsolete.

I was trying basically the whole day recreating this pretty simple part in FreeCAD.

If you can model it (even if its with the assembly branch), I will bite the bullet, and compile freecad from git.

[NormandC]

Well the part can certainly be modeled in FreeCAD, but I don't think it is currently possible to follow the resilient modeling strategy to the letter.

And of course there's the matter of fillets where OCC is pretty weak. Kwahoo may not like the 3.99 radius leaving a flat face, but it will be unavoidable in FreeCAD.

Let me see if I can have a go at it, but it will be later today (past bed time for Europeans!).

[kwahoo]

FreeCAD currently does not have a tool similar to Solid Edge's Replace face tool.

especially "replace face" - what kind of sorcery is this?

"Replace face" is a very useful tool that I've used quite a few times. I certainly hope that something similar gets added to FreeCAD in the future. But it may require some complex coding!

In this particular example such tool is IMO overkill. There should be only one operation: pad to face (already implemented in FC but buggy for cylinder surfaces) instead pad for distance + replace face.

[NormandC]

Well I modeled the part up to a point: The fillets are show stoppers. As I was fearing, here the OCC kernel fails miserably.

So I was mistaken when I said

Well the part can certainly be modeled in FreeCAD

At least, not following the sequence shown in the video. And we may have no choice but to change certain conditions, like avoid edge tangency at a few places (among them the rounded end of the tombstone).

For example, try to apply the 3.99mm fillets to the rib, and admire the result! That big a radius means it intersects the base and it creates "ridges".

FC_rms_normandc2_03.png (25.66 KiB) Viewed 2108 times

To get the fillets like we want, I don't see any other choice but to model the rib as a separate part, apply the fillets, then fuse the result to the main part. Unfortunately that means we cannot link external geometry.

The 2mm fillets on top of the cylinder and at the bottom of the bosses "explode" the part (some faces disappear) or simply fails to compute with a "Failed to create fillet" error. I can only get a 1mm radius for the bosses.

Even if making minute changes so edges are not coincident allow the fillet to succeed, FreeCAD (or maybe OCC) doesn't allow us to control the condition of fillets when they intersect other edges.

Here I changed the height of the tombstone profile so its rounded end comes 0.1mm short to touching the top face of the cylinder. I thought that would solve the problem.

FC_rms_normandc2_01.png (21.69 KiB) Viewed 2108 times

Applying a 2mm fillet now works, but look at how it adds a "bump" over the tombstone:

FC_rms_normandc2_02.png (22.96 KiB) Viewed 2108 times

Not at all what we expect. In commercial software, you can control how the fillet will react in similar conditions.

So it's a little disappointing...

[NormandC]

I forgot to mention,

I found that you can actually produce a base Pad from a sketch containing 4 separate circles. I'm not sure when that was made possible, since Part Design is not supposed to support multibodies. In any case, it's easy after that to add a pad for the base and to constrain it to the studs using linked external geometry.

Also, when building "helper cubes", look at what I did in my file (the features are called "planar face workaround 1, 2, 3). In two cases, I was able to have them consumed by the following pad feature, so I didn't have to create pockets to remove them afterward.

If you can model it (even if its with the assembly branch), I will bite the bullet, and compile freecad from git.

I don't think it would matter. I was able to model the part up to applying fillets, and those depend on the OCC kernel. But I run OCC 6.5.0, I wonder if with later versions (OCC 6.7.0 came out back in December) there have been enhancements to fillets.

In any case, the assembly branch will suffer from the same fillet problem. Its only advantage here would be to avoid having to create then delete those planar face workarounds.

OS: Ubuntu 12.04.4 LTS
Platform: 64-bit
Version: 0.14.3070 (Git)
Branch: master
Hash: d927d0bcb9266cde55e2b55af2fc3241ecc43022
Python version: 2.7.3
Qt version: 4.8.1
Coin version: 3.1.3
SoQt version: 1.5.0
OCC version: 6.5.0

[NormandC]

(sorry only 3 attachment/post allowed).

I just raised it to 5.

[Lynn]

Right now and for the past few months I've refrained from posting any elaborate video tutorials, knowing that with the Body container and working planes, the Part Design work flow will drastically change. All of the current FreeCAD videos focusing on Part Design found on YouTube will basically be obsolete.

Where can I find out more about the new Part Design work flow? Will it be more like that in the video? I'm happy to hear workplanes mentioned; they can be very useful. I'm also accustomed to having separate "assembly" and "part" file types. Is that part of the plan too? I'm interested in reading a discussion on that, as well. There is a lot of info in this forum, and it takes a while for a newb like me to absorb. Too bad there isn't a topic or set of links for exploring "how FreeCAD got to where it is, where it is going, and why". But perhaps with a shorter title.

[NormandC]

Where can I find out more about the new Part Design work flow?

Well there is a two-parter tutorial about it on the wiki, that will give you an idea of what will be possible:
http://www.freecadweb.org/wiki/index.ph ... Tutorial_I
http://www.freecadweb.org/wiki/index.ph ... utorial_II

Other than that you would have to compile the development branch and try it.

Will it be more like that in the video?

That video demonstrate a Solid Edge work flow and some operations won't be the same compared with other CAD programs.

I'm also accustomed to having separate "assembly" and "part" file types. Is that part of the plan too?

Yes, but having a single document containing everything (the FCStd file format) will still be possible for small projects.

where it is going

There is the Development roadmap on the wiki. Apart from that, info on this can be found on the Developers section of the forum. Much reading required though...

Too bad there isn't a topic or set of links

Indeed it would be nice to have such a thing, but that would mean someone would have to take the time to do it. There are not that many people contributing to the FreeCAD project, and they're doing so in their spare time.