Pocket Multipule Pads, Error

[Mel3]

I'm trying to pocket through multiple pads. The pocket only goes through the first two though and then results in an error message.
My thought is that maybe this has to do with spacing and/or overlapping geometry between the pads (but then why does it "work" for two of them but not all four?). Do I need to fuse the pads in some way so that they become one thing for the pocket to go through?
Additionally, I altered the sketches after making the pads. The first two pads changed to reflect the updated sketches but the second two did not (why?).

Pocket.png (28.71 KiB) Viewed 536 times

FreeCAD file: https://drive.google.com/open?id=1_VhUX ... LUmu3Ej2kM

OS: Windows 8.1
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.18.16110 (Git)
Build type: Release
Branch: (HEAD detached at upstream/releases/FreeCAD-0-18)
Hash: f7dccfaa909e5b9da26bf50c4a22ccca9bb10c40
Python version: 3.6.6
Qt version: 5.6.2
Coin version: 4.0.0a
OCC version: 7.3.0
Locale: English/UnitedStates (en_US)

[TheMarkster]

A pocket operation will only affect the features inside that same body. This is the desired behavior since we wouldn't want to have to concern ourselves with pocket operations that might affect other body objects in our model.

As for why the pocket isn't working, I think the problem is actually with Sketch16 -> Pad005. If we constrain the left vertical line segment ("4-Line" in the elements box) to 5.5mm (just a tiny bit longer than what it already is) it ensures Pad005 intersects the other features. I suspect as it is it's very close, but not quite connecting to other features. Or perhaps it connects, but during the later pocket operation you end up with multiple solids.

[kisolre]

Good find. That is the problem with unconstrained sketches and freehand modeling. Things might look correct but actually not be.
There is a tiny gap between the two surfaces. They touch at small area and thes allows for the pad to succeed. But then the pocket removes that and the result is two solids in a body which is not allowed.
Your models are oriented quite arbitrary in space and a lot of problems will arise from that - hard to constraint, need to reference external geometries to keep things parallel/perpendicular,...

[Mel3]

There is a tiny gap between the two surfaces. They touch at small area and thes allows for the pad to succeed. But then the pocket removes that and the result is two solids in a body which is not allowed.

As for why the pocket isn't working, I think the problem is actually with Sketch16 -> Pad005. If we constrain the left vertical line segment ("4-Line" in the elements box) to 5.5mm (just a tiny bit longer than what it already is) it ensures Pad005 intersects the other features. I suspect as it is it's very close, but not quite connecting to other features. Or perhaps it connects, but during the later pocket operation you end up with multiple solids.

Thank you, that worked!
So for future reference, for a pocket to succeed when there's multiple pads the pads need to be touching or overlapping.

Your models are oriented quite arbitrary in space and a lot of problems will arise from that - hard to constraint, need to reference external geometries to keep things parallel/perpendicular,...

I will have better planning to avoid that in the future. This has been my first project using FreeCAD so I've really been stumbling my way through it.

[kisolre]

So for future reference, for a pocket to succeed when there's multiple pads the pads need to be touching or overlapping.

NO. Your pads were touching (or they would not succeed in the first place) and how much overlap you need is up to you. BUT if you want them to touch in some way you have to ensure that. Drawing arbitrary lines will not always ensure that. And if your sketches are not fully constrained this could lead to almost working result.