Feature disappears when trying to pad sketch

[Scalpel78]

Hi, I'm having a weird problem.

On these two feet I'm trying to create two "poles" going upwards. I've created a sketch on the top surface, and added two rectangles.

FeetWithSketch.PNG (28.38 KiB) Viewed 3854 times

But when I choose the sketch, and click Pad the hole foot disappears.

FootGone.PNG (14.63 KiB) Viewed 3854 times

Why does it do that? I created a dummy project, and did the same there, and there is worked, so I'm not sure why it doesn't work in my main project.

[ickby]

Your FeedPad is one feature with two separated solids. This is not allowed, in PartDesign one shall create a single solid only by definition. The first pad and the fillet do not check that so it works, but the pocket operation checks it and therefore uses only one of the two seperated solids. The error here is that the first two opertions do work even if it is against the rules.

[Scalpel78]

Ok, thank you. Then I'll create the feets separately instead.

Can I perhaps create one foot, and then mirror it to get the other one?

[jmaustpc]

Ok, thank you. Then I'll create the feets separately instead.

Can I perhaps create one foot, and then mirror it to get the other one?

Yes but must be a Part wb mirror (makes a new solid )NOT a PartDesign mirrored feature (mirrors an aspect of a single solid)

You can also use a Draft Clone for arbitrary placement and orientation, or Draft Polar or Ortho Array, ...depending on your exact requirements

[quick61]

Hi Scalpel78, A few more quick tips. If you haven't installed it yet, a very handy and almost necessary tool to add to FreeCAD is Graphviz. You can find how and where to get it for your OS from the FreeCAD Wiki page Std DependencyGraph. When you look at your dependency graph you will see the forking that has happened in your model.

Dep_Graph_1.png (167.77 KiB) Viewed 3824 times

While looking at that dependency graph, you can also see where you installed Fillets, (TopFillet and BottomFillet) very early on in the modeling process. This is something you want to avoid at all costs. Fillets should not be applied until the very last. This is not just true with FreeCAD, but just as true with the uber expensive CAD packages as well. Fillets are a finishing touch, not a means to an end.

Keep at it,it will come. Even us more experienced users end up forking our models once in a while... You just don't hear about it because we know what happened and fix it up before anyone finds out.

Mark

[NormandC]

Fillets should not be applied until the very last. This is not just true with FreeCAD, but just as true with the uber expensive CAD packages as well. Fillets are a finishing touch, not a means to an end.

And this topic is just an example of how creating fillets too early can cause problems: viewtopic.php?f=3&t=7454

Even us more experienced users end up forking our models once in a while... You just don't hear about it because we know what happened and fix it up before anyone finds out.

[Scalpel78]

Hi, thanks, I'm installing Graphviz now.

I see your point about the fillets. I'll try to hold off on those until the end of my projects.

When you say forking, do you mean the blue or the red areas?

Forking.PNG (54.28 KiB) Viewed 3810 times

What causes forking?

[NormandC]

Your FeedPad is one feature with two separated solids. This is not allowed, in PartDesign one shall create a single solid only by definition. The first pad and the fillet do not check that so it works, but the pocket operation checks it and therefore uses only one of the two seperated solids. The error here is that the first two opertions do work even if it is against the rules.

I just reported it as a bug. issue #1724

[NormandC]

What causes forking?

You mapped "InnerBottomSketch" to a face on "TopFillet". But you then continued adding another sketch ("InnerSketch") on top of the same TopFillet feature.

In PartDesign, everything must be linear. You should not go back to prior features and build on top of them, that's when you fork your model into separate "timelines". If you're a science-fiction fan like myself, that's like the old paradox of the man who travels back to the past and accidentally kills his grandfather. Which should be impossible.

[bejant]

The arrows are Dependencies. "InnerSketch" depends on "TopFillet", so that's one Dependency, or one arrow. The other arrows are Links to External Geometry (those magenta lines in "InnerSketch"). That's OK.

In the blue area, "InnerBottomSketch" depends on both "TopFillet" and "BottomFillet". So you can't edit "OuterSketch" without affecting both "PolarPattern" (the robot head) and "InnerBottomPocket" (the part that fits into the bottom of the head).

So for your model in "OuterSketch" you can't change, for example, the 43mm Horizontal Distance Constraint (Constraint13) to modify the robot head without affecting the part that fits into the bottom of the head too. If you change Constraint13 from 43mm to 42mm, it causes the male portion of the part that fits into the bottom of the robot head to become off-centered.

What causes forking?

Usually someone toggles a previous Feature in the tree view to visible, and does some operation on it instead of always working from newest item in the tree. But I really don't know how you model got forked.
Edit: I see Norm figured it out.