I always have to redo my designs. What am I doing wrong?

[ulfwin]

Hi!

For literally all designs I've tried using Freecad (a handfull), I have got stuck at some issue which forced me to redo or rethink my design. With issue I mean Freecad not functioning the way I expected, and needing to figure out a workaround. This is clearly because I lack experience and knowledge in the tool, but I'm struggling to find a solution to this. I've gone through some tutorials, and whenever I encounter a problem, I search for a specific solution to that problem, but the fact remains that I every time hit a wall, and need to start over or redo parts of the design, often several times per design.

Therefore, I'm hoping to get some help by showing my most recent design, and get some pointers to where I'm doing wrong. Hopefully I'm doing some systematic mistake which causes most of my problems. If not, at least I can progress short term.

I've added a screenshot which shows the shape I want (a cylinder with a hole, and where on side has incline which ends abruptly). If I have the shape already, then what is the problem? Well, I want it to be one solid part so I can export and eventually 3D print.

Now, it's two separate parts that overlap. The first listed body (Body001) is the incline, which I created using a rectangle sketch, sweeped over a helix. For some reason the helix was created outside of the body I wanted, so I dragged it to "Body001", which then became the BaseFeature, but it remained outside the body as well.

The second body (Body) is simply a cylinder with a hole in it.

I then try to use the boolean tool, using "fusion" and the two created bodies. The result... nothing is left of the design. I've attached a picture. It says "fusion of tools failed", but it's unclear to me why. If I try to edit the boolean operation, suddenly the helix appears as a body in the list, and if I press ok, all the structure under "Boolean" in the "Labels & Attributes" window disappears! (see picture) Since I didn't add or remove anything, it seems to me like unreliable behavior.

So, my question is if I'm doing some systematic error which causes me to always end up in situations similar to this, or am I simply unlucky, and again encountered a specific issue with Freecad? What is a proper path to reach the design I want?

I'm very grateful for any help!

Freecad info:
OS: Linux Mint 18.3 Sylvia
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.17.13519 (Git)
Build type: None
Branch: releases/FreeCAD-0-17
Hash: 1a8b868018f45ea486c0023fdbfeb06febc1fb89
Python version: 2.7.12
Qt version: 4.8.7
Coin version: 4.0.0a
OCC version: 7.2.0
Locale: English/UnitedStates (en_US)

[freedman]

Here is what I do, but just by experimentation.
Once I create a second body I do a copy and paste of the second body into the first body. All this is done in the tree and the first body must be active part focus. I have been messing around with tree copy and paste to keep my part all in one body. I try to drag and drop, sometimes it works sometimes not. Copy and paste seems to work best.

[ppemawm]

What is a proper path to reach the design I want?

I would use an AdditiveSweep in PartDesign and one Body as shown below. Create a Shapebinder of the helix to use for the sweep path:

Capture.JPG (66.24 KiB) Viewed 1624 times

OS: Windows 10
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.17.13519 (Git)
Build type: Release
Branch: releases/FreeCAD-0-17
Hash: 1a8b868018f45ea486c0023fdbfeb06febc1fb89
Python version: 2.7.14
Qt version: 4.8.7
Coin version: 4.0.0a
OCC version: 7.2.0
Locale: English/UnitedStates (en_US)

[ulfwin]

I would use an AdditiveSweep in PartDesign and one Body as shown below.

Thanks for the fast reply! Your method seems sound, but I don't get it to work. In my first try, the top surface of the cylinder disappears (see picture). As a work around, I tried to place the sketch at the end of the incline, rather than the beginning, but that made the whole cylinder disappear! (see other picture)

Again I wonder if it's something wrong with my thought process, or does everybody struggle like me?

[ppemawm]

I wonder if it's something wrong with my thought process,

It looks to me that you are missing a pad for the cylinder in the Body. I do not know how you can have a hole without a pad first.

Please see the attached file and see if you can reproduce it exactly. When using the AdditivePipe or sweep I usually select the sketch first in the tree then Add Edge and select the helix shapebinder in the 3D view.
Note that it is generally good practice to try to avoid coplanar surfaces where possible. This will sometimes cause Boolean operations to fail.

cyl_sweep.FCStd

(37.09 KiB) Downloaded 37 times

[freedman]

Once the circular wedge is drawn make a datum plane (on the leading edge) and build the donut off the backside of the plane.

[ulfwin]

Please see the attached file and see if you can reproduce it exactly.

That is very strange... When I open your file I get exactly the same problem as before, with the top surface disappearing (see picture). I tried to update to the absolute latest version of Freecad, but it gives the same result. Is there a difference between the windows and the linux version!?

[ppemawm]

When I open your file I get exactly the same problem as before, with the top surface disappearing

Try reducing the inside radius of the AdditivePipe sketch slightly. Boolean operations on coplanar surfaces are sometimes erratic.

Capture.JPG (84.75 KiB) Viewed 1516 times

[freedman]

I made one quickly.

[ulfwin]

I made one quickly.

Try reducing the inside radius of the AdditivePipe sketch slightly.

Thanks a lot to both of you! I managed to solved it with both your help.

Indeed the issue seemed to be coplanar surfaces. The surprising thing (for me at least) is that the shift needed cannot be arbitrarily small. It must be large enough, so that the planes are not "too coplanar" (sounds weird in a mathematical sense). In this example, if I shifted the helix 1 um in x, I still had a problem, while 10 um solved it. Also the width of the sketch affected if the problem appeared or not, so I guess all surfaces with a risk of being coplanar must be handled with care.

Actually, besides getting help with this specific issue, I was hoping to get some general advice. Perhaps you can shortly share your views?

The issue here is one of many of very different types I've had with Freecad, and to be honest at times I've considered switching to something else. Mostly I'm curious whether this trail-and-error approach is inevitable with Freecad, or it's enough to learn a few tricks (like the coplanar issue). If the latter, would you perhaps be able to share some of these tricks?

Thank you in advance!