Error union shapes

[joelrodrigos]

OS: Windows 10
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.16.6712 (Git)
Build type: Release
Branch: releases/FreeCAD-0-16
Hash: da2d364457257a7a8c6fb2137cea12c45becd71a
Python version: 2.7.8
Qt version: 4.8.7
Coin version: 4.0.0a
OCC version: 6.8.0.oce-0.17

Hello i’m learning Freecad and i find the diagram of a piece

Reddit_CC02_Moderate.png.pdf

Diagram

(82.56 KiB) Downloaded 20 times

, i try to make it with freecad

Parts before union

error_antes.PNG (137.76 KiB) Viewed 1361 times

but when i make the unión of the parts i have one piece with errors and black parts, i want to know what i’m doing wrong and how to have a single solid piece, thanks and sorry for my bad english, this is the frecad file

02 CHALLENGE.FCStd

Free cad file

(91.79 KiB) Downloaded 19 times

.

[chrisb]

If you get an error form a booelan operation you should check the parts with Part->CheckGeometry with BOPCheck enabled. On your model there are problems with superior_pad and base_pad.

[chrisb]

If you look at the sketch "base" it is not clear what is inside and what is outside. In fact I don't understand how this could be padded anyway. If a sketch is correct you have inside and outside. If you walk an arbitrary way from inside to outside you must always cross an uneven number of lines. From outside to outside it is always an even number of lines you are crossing. Construction lines are not counted.

[ppemawm]

i want to know what i’m doing wrong and how to have a single solid piece

Your union likely fails because you have several parts that fail geometry check using Part>Analyses geometry for errors tool (see chrisb comment).

This part is actually rather difficult to model. Your approach requires several complex sketches and Part>unions for a complete part. The preferred approach is to use many simple sketches of individual features in a sequential process using the PartDesign workbench. It is also considered good practice to fully constrain your sketches as you proceed with the process.

Rather than analyze your model I offer an alternative simpler solution using only the PartDesign workbench in the attached file:

02_challenge_PartDesignWorkbench.FCStd

(438.8 KiB) Downloaded 17 times

The object of parametric modelling is to add (pad) or subtract (pocket) "features" from a starting object such as a pad. As each feature is added it is automatically unioned to the last state of the model. The pad I started with was the basic overall shape of the part as shown in the figure:

Picture1.jpg (162.99 KiB) Viewed 1326 times

A detail of the 12 mm radius as I interpreted the drawing is also included in the figure to show the use of the required construction (blue) lines.

The rest of the features are added in the order shown in the file. Only half of the part is modeled and then Part>mirrored about the XY plane.

Due to limitations of V0.16, an edge must be created for the reference axis (green edge5) in order to use the polar pattern tool for the 7 holes as shown in the figure below. This can be done by properly locating pad014 which is later removed with pocket003.

Capture2.JPG (107.29 KiB) Viewed 1326 times

Capture4.JPG (64.61 KiB) Viewed 1326 times

The part is completed by mirroring it about the XY plane:

Capture.JPG (113.38 KiB) Viewed 1326 times

OS: Windows 10
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.16.6706 (Git)
Build type: Release
Branch: releases/FreeCAD-0-16
Hash: f86a4e411ff7848dea98d7242f43b7774bee8fa0
Python version: 2.7.8
Qt version: 4.8.7
Coin version: 4.0.0a
OCC version: 6.8.0.oce-0.17

[joelrodrigos]

Thanks for your advices, greetings from Peru.

[bejant]

Hello i’m learning Freecad and i find the diagram of a piece

Hi, and welcome! We've seen that piece in the forum before - have a look here:
https://forum.freecadweb.org/viewtopic.php?f=24&t=19934

Edit: Here's another
https://forum.freecadweb.org/viewtopic.php?f=3&t=20606

[Krypto]

Thanks for your post, ppemawm!

Since I'm new to this cad stuff, I'm always looking for projects and the diagram Joel posted looked like fun. I really got bogged-down with that first sketch, however. Somehow I managed to get it constrained without the radius shown in the detail but it wasn't working very well. I also didn't know about Part-Mirror so I was heading down the wrong path with the rest of the project anyway.

Following the ideas in your post I successfully managed to construct the part in 0.17. I evened used a Datum line for the bolt circle.

OS: Linux Mint 18.2 Sonya
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.17.12595 (Git)
Build type: None
Branch: master
Hash: 8c7bb0cd551cf11551ff71d716a16211c6d5e13d
Python version: 2.7.12
Qt version: 4.8.7
Coin version: 4.0.0a
OCC version: 7.1.0
Locale: English/UnitedStates (en_US)

reddit_3.png (91.08 KiB) Viewed 1243 times

It looks OK, but I need to spend some time reading about mirror as I think I need to fuse the two halves together. I'm still not that familiar with functions outside of part design.

Reddit_02.fcstd

(207.62 KiB) Downloaded 15 times

Reddit_03.fcstd

(246.55 KiB) Downloaded 16 times

[Willem]

Hi, I start with Reddit_02.fcstd
- in the part design workbench make a clone of Fillet002, this clone is placed outside the body
- in Draft workbench select Mirror

Schermafdruk van 2017-11-19 03-12-48.png (266.84 KiB) Viewed 1234 times

[Krypto]

Thanks Willem for the pointers.

Also thanks to Bejant for links to older forum posts about this part as I didn't realize these exercises have been around for awhile. In those older posts I found a great cache of cad exercises from forum member gsegura96 at this location:

https://github.com/gsegura96/CAD-Challenge

Along with the prints of the first 14 Reddit CAD challenges, for most he also includes very nice fcstd files of the completed parts using .017 Part Design. This is great as there's not much documentation on the new features of the part design workbench. For instance, gsegura96 took a very different approach to this part than me, doing the entire part in Part Design utilizing Mirrored Feature and a few Datum Planes. There's certainly enough projects to keep me busy for awhile.