Sketching (furniture) with rectangles

[ivo]

Hi,

I've been trying to sketch some furniture items using rectangles in sketch mode and it worked beautifully in Autodesk Fusion 360 (not what I'm looking for, though), but for the life of me I can't get the same thing to work in FreeCAD. Since the furniture is made up of planks/sheets rectangles seemed the most appropriate tool to use.
I can get a U shape connected rectangle construct to Pad. When I add the top beam though there is no way I can get it to pad. I've tried constraining every imaginable way, using the validation tool, even used the polyline tool for that last segment but nothing I do gets it to pad. Also tried the same file with latest .16 dev version from yesterday but same result. Is there a specific trick to this or can it just not be done? Logic says it should work...

Can pad:

pads.JPG (21.92 KiB) Viewed 1757 times

Can't pad:

padsnot.JPG (24.36 KiB) Viewed 1757 times

OS: Windows 8
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.15.4671 (Git)
Branch: releases/FreeCAD-0-15
Hash: 244b3aef360841646cbfe80a1b225c8b39c8380c
Python version: 2.7.8
Qt version: 4.8.6
Coin version: 4.0.0a
OCC version: 6.8.0.oce-0.17

[DeepSOIC]

Hi!
Sketch must cleanly represent the contour of the area to be padded (extruded). In your case it does not (those lines that subdivide the area to be filled need to be removed).

[NormandC]

That the first sketch pads successfully is a fluke. It shouldn't as DeepSOIC explained.

If your model is to represent your furniture in real life, I mean if you plan on making production drawings out of your model, then you need to create separate pads for each of the planks/sheets. It might be easier to work with Draft Rectangles.

[ivo]

Hi!
Sketch must cleanly represent the contour of the area to be padded (extruded). In your case it does not (those lines that subdivide the area to be filled need to be removed).

Thanks for the quick reply.
How can it be not a factor in the first sketch (connecting sections between verticals and horizontal) but break everything in the second? The rectangle objects are still individual objects, are they not? It shouldn't be hard for the software to extrude each rectangle individually, that's all I'm looking for here after all. And thanks to constraints none of them should be overlapping but simply be connected.
How should I go about sketching furniture so that the actual panels are represented individually without making a separate sketch for each panel and using assembly?
Edit: so it's an accident, personally I still find it illogical that it doesn't work. Especially since Fusion doesn't even give me a funny look for sketching it, as I assumed would happen here.

[NormandC]

How can it be not a factor in the first sketch (connecting sections between verticals and horizontal) but break everything in the second?

See my previous reply.

It shouldn't be hard for the software to extrude each rectangle individually

That is not what the PartDesign Pad is intended for. Its intent is to produce a single solid. Even using the Part Extrude won't give you the result you're looking for: under the hood, the software first need to create a planar face out of the sketch elements, then extrude the face. It cannot get a valid face with crossing elements.

How should I go about sketching furniture so that the actual panels are represented individually without making a separate sketch for each panel and using assembly?

I already gave you a partial answer on that. I wish you had not ignored my reply.

[ivo]

I already gave you a partial answer on that. I wish you had not ignored my reply.

Lets keep the eye rolling to a minimum considering I was typing my reply while you managed to post yours.
I don't need a 2D blob that I'd have to completely redo when I need to make changes to some features. Guess I'll just stick to Fusion or find something else.

[bejant]

That the first sketch pads successfully is a fluke

Yes, especially when there are also line segments on top of line segments too.

[DeepSOIC]

How should I go about sketching furniture so that the actual panels are represented individually without making a separate sketch for each panel and using assembly?

Well, that is a problem, actually.
One solution, exceptionally convoluted and ugly, but works:

convoluted-way-to-pad.png (127.89 KiB) Viewed 1730 times

convoluted-way-to-pad.FCStd

requires Lattice2 plug-in workbench

(21.5 KiB) Downloaded 31 times

This is in some sense similar to what I did in my skyscraper generator project.

Alternative is to use my FreeCAD branch, which allows external geometry links between sketches. You can sketch the whole thing, then trace out individual panels in separate sketches.

Another alternative is to use Boolean operations (Part workbench) in clever ways, to split panels off a round "assemble-fused" thing modeled in one sketch...

[NormandC]

The problem is we have no idea of your intent. Will you have a series of stacked panels together? How will your panels be assembled? Screws, mortise and tenon, dowels? Do these details need to be modeled in? What's the end goal? Visual purpose, fabrication? Give us more detail on what you're trying to achieve so we can best advise you, that will save time for everybody and you may get not more rolling eyes.

If you want to keep the complexity of your model to a bare minimum, then I suggest using plain and simple primitive Cubes.

If your panels repeat in a regular manner, I suggest looking into Draft Array.

If you plan on making frequent changes, and/or you don't have regular intervals, then you may want to use the community-made Assembly2 workbench to create assembly constraints between your panels. That way, if you change sizes, you won't have to change the placement of your panels manually.

[bejant]

Another method, but if you're new to FreeCAD it's really easy to mess up your model...

20160306g.fcstd

(22.24 KiB) Downloaded 45 times

OS: Ubuntu 14.04.4 LTS
Word size of OS: 32-bit
Word size of FreeCAD: 32-bit
Version: 0.16.6551 (Git)
Build type: None
Branch: master
Hash: 74a43f23b3dcf9a95a3d691b9373bb0ecf8ea0f2
Python version: 2.7.6
Qt version: 4.8.6
Coin version: 4.0.0a
OCC version: 6.8.0.oce-0.17

Edit: You guys are posting so fast I can't keep up!