Stumped on combining objects

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earthcare
Posts: 26
Joined: Tue May 31, 2016 7:46 am
Location: Australia

Stumped on combining objects

Post by earthcare »

Hi all,

I'm trying to draw up an object for injection moulding: it's based on two imported and extruded DXFs, which I've positioned in layers. But I can't seem to merge the 3 layers into a single object. I've tried Draft > Upgrade, Part > Union and Part > Join; the only one that gets a change is Part > Union, but it still displays the layers and each is selectable, which isn't what I want. Is there a way to do this?

OS: Linux Mint 17.3 Rosa
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.16.6703 (Git)
Build type: None
Branch: releases/FreeCAD-0-16
Hash: 2ce5c8d2e3020d05005ed71f710e09e9aa561f40
Python version: 2.7.6
Qt version: 4.8.6
Coin version: 4.0.0a
OCC version: 6.8.0.oce-0.17
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SinglePieceInjectionMouldedClip-16-08-18.fcstd
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ickby
Posts: 3090
Joined: Wed Oct 05, 2011 7:36 am

Re: Stumped on combining objects

Post by ickby »

When you measure the distance between some edges of your individual parts with the Part workbench measurement tools you will find that they are 5.96e-007mm apart, which is more than FreeCADs tolerance. Hence thex are found to be not overlaping. The result of this is that the fusion works, but it contains 3 seperate solids.

If you look at your placements you will find that the exact distance we measured is written in the y position. If you just set it to 0 there the fusion will work flawless (at least with occ7.0 which I use). Than you just need to make sure you refine the result when you don't want to see the subdivided faces.
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Willem
Posts: 1611
Joined: Fri Aug 12, 2016 3:27 pm
Location: Lisse, The Netherlands

Re: Stumped on combining objects

Post by Willem »

In the properties of your extrusions make the Y-coordinates zero and change the solid to true. than you can fuse the three extrusions to one shape in the part workbench,
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earthcare
Posts: 26
Joined: Tue May 31, 2016 7:46 am
Location: Australia

Re: Stumped on combining objects

Post by earthcare »

Willem

Another thing learned - thank you.

But I'm a bit confused: I can't find a "fuse" in the part workbench, and both "Union" and "Connect" result in a single item in the combo model but with the separate extrusions still selectable. Is this where I should be refining?
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NormandC
Posts: 18534
Joined: Sat Feb 06, 2010 9:52 pm
Location: Québec, Canada

Re: Stumped on combining objects

Post by NormandC »

earthcare wrote:But I'm a bit confused: I can't find a "fuse" in the part workbench, and both "Union" and "Connect" result in a single item in the combo model but with the separate extrusions still selectable. Is this where I should be refining?
Part Fuse is Part Union. I'm not sure why we call it fuse, maybe because the resulting object is labelled "Fusion" in the Model tree; or maybe the command was named fuse in the past, then was changed to Union.

It does produce a single solid, but due to a bug/limitation in the geometric kernel (OCC) used by FreeCAD, the original edges from the parent shapes always remain. It's why one of the FreeCAD developers added a refining algorithm that analyzes planar and cylindrical faces and joins faces that are found coplanar. There are two methods in the GUI to use this tool:
  • The Part --> Refine shape menu creates a new independent object that is not linked to the parent shape. Any change to the objects used in the Fusion will not follow to the refined shape; it would need to be deleted and created again.
  • The OpenSCAD workbench's Refine shape feature is based on the Part Refine shape tool, but it creates a parametric feature linked to the parent object.
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