Sheet metal WB 2018

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-alex-
Posts: 127
Joined: Wed Feb 13, 2019 9:42 pm
Location: France

Sheet metal WB 2018

Postby -alex- » Sat Mar 02, 2019 5:34 pm

OS: Windows 10
Word size of OS: 32-bit
Word size of FreeCAD: 32-bit
Version: 0.18.15115 (Git)
Build type: Release
Branch: master
Hash: 684b4ab03a27231e0cc603ca815bf9ea367fd0b9
Python version: 2.7.14
Qt version: 4.8.7
Coin version: 4.0.0a
OCC version: 7.2.0
Locale: French/France (fr_FR)


Hi there,

I write this post to talk about the state of the art of sheet metal workbench in 2018. I feel those great improvements are not very visible in the forum, so I talk about it here to do some advertising in a way.
I don't feel free to create an annoucement feature topic because I'm just an end user, not one of developers who have coded all of this. Many thanks to them :D
So I write it here, in the user show case section :roll:

First of all, many informations can be find here:
https://forum.freecadweb.org/viewtopic.php?f=22&t=25281

So, some new features are listed below:

- bend deduction is taken into account for unfolding by using of K factor : hence the dimensions of unfold generated paterns are exact!
- while unfolding many sketches are created, now with bend lines.
- basebend feature is added: it allows to extrude a sheetmetal part from an open profil in sketch. This is a very useful feature, many thanks.
- "sketched bends": you can now create a sketch on a face, then add a simple bend on the same face, then link the sketch to the bend. In this way the bend get the sketch profile. In one step you can get a partial bend, or a complexe geometry bend with unregular shape whith holes and so on...
- corner treatment are improved for boxes, with auto-mitering feature.

See you.
Alex

A square-round modelized with draft WB -> Part WB -> Sheetmetal WB
Squareround-unfold.jpg
Squareround-unfold.jpg (231.27 KiB) Viewed 2702 times
Sheet metal part with basebend and sketched bend
Basebend-unfold.jpg
Basebend-unfold.jpg (216.55 KiB) Viewed 2702 times
triplus
Posts: 8364
Joined: Mon Dec 12, 2011 4:45 pm

Re: Sheet metal WB 2018

Postby triplus » Sat Mar 02, 2019 6:59 pm

Always nice to see FreeCAD sheet metal capabilities progressing!
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NormandC
Posts: 18534
Joined: Sat Feb 06, 2010 9:52 pm
Location: Québec, Canada

Re: Sheet metal WB 2018

Postby NormandC » Sat Mar 02, 2019 11:48 pm

Cool! Not enough sheet metal projects around. :)

-alex- wrote:
Sat Mar 02, 2019 5:34 pm
- corner treatment are improved for boxes, with auto-mitering feature.
I wasn't aware of that one, I'll have to check it out...

-alex- wrote:
Sat Mar 02, 2019 5:34 pm
Version: 0.18.15115 (Git)
Your 0.18_pre version is quite outdated. The latest is 0.18.15998. Wait after the weekend, the next build will be bumped over 16000. :D
chrisb
Posts: 16285
Joined: Tue Mar 17, 2015 9:14 am

Re: Sheet metal WB 2018

Postby chrisb » Sat Mar 02, 2019 11:59 pm

NormandC wrote:
Sat Mar 02, 2019 11:48 pm
Your 0.18_pre version is quite outdated. The latest is 0.18.15998. Wait after the weekend, the next build will be bumped over 16000. :D
I just updated and have this very version version number!
-alex-
Posts: 127
Joined: Wed Feb 13, 2019 9:42 pm
Location: France

Re: Sheet metal WB 2018

Postby -alex- » Sun Mar 03, 2019 10:54 am

Thanks for all your comments!

NormandC wrote:
Sat Mar 02, 2019 11:48 pm
Cool! Not enough sheet metal projects around. :)
Yeap, I suppose that is due to the fact sheet metal is far less convenient compare with 3D printing for eg.
So, I would say that both of them can be complementary to achieve beautiful assemblies :)

NormandC wrote:
Sat Mar 02, 2019 11:48 pm
Your 0.18_pre version is quite outdated. The latest is 0.18.15998. Wait after the weekend, the next build will be bumped over 16000. :D
Yes I have to update my FC version for sure, now it's time.

If some people are interested about sheet metal rules, let me know. I could also share my workflow about full parametric model.
About parametric design, I have a question about the square round model above-mentioned: I didn't find a way to modelise it parametrically. I mean I've used the draft WB to draw the rectangular and the polygonal shapes, which are parametric. But the linking faces are not, because they are draw with shapebuilder tool from part WB.
Do you know a way to get this kind of square round fully parametric? (you can forget loft features: they don't create flat linking surfaces)
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NormandC
Posts: 18534
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Location: Québec, Canada

Re: Sheet metal WB 2018

Postby NormandC » Sun Mar 03, 2019 2:43 pm

-alex- wrote:
Sun Mar 03, 2019 10:54 am
Do you know a way to get this kind of square round fully parametric? (you can forget loft features: they don't create flat linking surfaces)
A sweep will generate planar faces. You just need to add a straight line between the circle and the rectangle to use as sweep path.

Could you share your round to square model? I'm curious about a couple of things. How did you create the fillets for the bends?

And how did you manage to include a Part Cut inside a Body container? That should not be possible. :?
-alex-
Posts: 127
Joined: Wed Feb 13, 2019 9:42 pm
Location: France

Re: Sheet metal WB 2018

Postby -alex- » Sun Mar 03, 2019 5:27 pm

NormandC wrote:
Sun Mar 03, 2019 2:43 pm
A sweep will generate planar faces. You just need to add a straight line between the circle and the rectangle to use as sweep path.
Thanks for the trick! I have not explored far enought the sweep feature with multisection option. Unfortunately I guess that does not solve the problem. This kind of features (loft, sweep) balance the numbers of faces beetween each profile. So you get faces with 4 vertexs, not flat. I need to get triangular faces, from a set of edges (90° arc length) to a single corner of the rectangle. Otherwise the unfold feature of sheetmetal WB fails.

NormandC wrote:
Sun Mar 03, 2019 2:43 pm
Could you share your round to square model? I'm curious about a couple of things. How did you create the fillets for the bends?
For sure, I'll share it.
About the filets and the workflow, yes it's a little be tricky.... The difficulty comes from some limitations of the 3D offset feature (PartWB). So, I set my workflow to avoid those limitations. Maybe there is a simplier workflow than mine. I'll give comments in next post with the FC part.

NormandC wrote:
Sun Mar 03, 2019 2:43 pm
And how did you manage to include a Part Cut inside a Body container? That should not be possible. :?
Yeap, you're right, but I'm using PartOmagic workbench, and the Observer feature is enabled. So, you have to enable Observer feature to play with this part, sorry for this not fully standard design.
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NormandC
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Location: Québec, Canada

Re: Sheet metal WB 2018

Postby NormandC » Sun Mar 03, 2019 7:56 pm

-alex- wrote:
Sun Mar 03, 2019 5:27 pm
Unfortunately I guess that does not solve the problem. This kind of features (loft, sweep) balance the numbers of faces beetween each profile. So you get faces with 4 vertexs, not flat. I need to get triangular faces, from a set of edges (90° arc length) to a single corner of the rectangle. Otherwise the unfold feature of sheetmetal WB fails.
I understand now, you are creating multiple planar triangular faces that meet in a single vertex. Yeah, that will be a tough nut to crack... Even if you manage to create those faces parametrically, I'm not sure you can create a parametric shell from them...
-alex-
Posts: 127
Joined: Wed Feb 13, 2019 9:42 pm
Location: France

Re: Sheet metal WB 2018

Postby -alex- » Sun Mar 03, 2019 10:18 pm

Square to round sheet metal linked to this post.

Below I give a lot of details for general purpose (I know NormandC you already know most of it).

Optional workflow:
- create a master sketch to control the square-round for future dimension changes (named here CDCF)
- both "carre" (square) and "rond" (round) sketches are drawn with X reference to be linked to the master sketch.
- part design additive loft is created to get a simple and parametrical visual model.
- then create a second body for "manufacturing" model

Minimal workflow:
- both sketches "carre" and "rond" are offsetted inside. The offset value coresponds to the inner bend radius you whish

Millstone: end of the parametric design. Next steps have to be done if square-round dimensions are modified...

- create triangular faces then create shell by using Part->shapebuilder, planar option
- because the part has a plan of symetry, split both large triangular faces by midd datum plane by using boolean fragments (see picture)
- downgrade boolean fragments DraftWB-> downgrade
- delete unused faces
- create the shell ->Part->shapebuilder
- then offset the shell outside with Part->3D offset
- then create thikness with 3Doffset again and fill option
- cut everything you want, here is a cylinder
Now you can unfold the shell: Sheet metal WB -> select a face then unfold

Enjoy sheet metal!

square-round-shell-boolean-fragments.jpg
square-round-shell-boolean-fragments.jpg (216.48 KiB) Viewed 2409 times


PD-square-round-plus-sheetmetal.jpg
PD-square-round-plus-sheetmetal.jpg (232.9 KiB) Viewed 2409 times
Attachments
Rond-carre.FCStd
(216.76 KiB) Downloaded 32 times
SteveJT77
Posts: 1
Joined: Mon Mar 04, 2019 11:31 am

Re: Sheet metal WB 2018

Postby SteveJT77 » Mon Mar 04, 2019 12:10 pm

Hi All, Apologies for jumping in but i'm new to Freecad and was wondering if it will enable us to produce flat patterns that can be printed off and laid out on sheet metal to use as a template for fabrication purposes?
Thanks in advance...... :D