Map sketch to face unwanted reorientation

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tojape
Posts: 1
Joined: Sun Mar 19, 2017 11:38 am

Map sketch to face unwanted reorientation

Postby tojape » Sun Mar 19, 2017 12:14 pm

Hi, I am a very beginner of FreeCAD. I'm trying to create a part (see attached file). When I try to map a sketch to a face (on a pad created from sketch Body_section) FreeCAD rotates the sketch by 90 degrees. I obviously do not want this behaviour. My aim to create pockets in the current orientation from sketches Side_ties_groove,Tie_holes,V_groove,Upper_cut. I tried several ways to avoid the unwanted rotation with no success. Can you help me?
Thank you.

Sytem info:
OS: antiX 16
Word size: 32-bit
Version: 0.14.3702 (Git)
Branch: releases/FreeCAD-0-14
Hash: b3368125c63289ec8ce9faec2b2ae4c78d436406
Python version: 2.7.8
Qt version: 4.8.6
Coin version: 4.0.0a
SoQt version: 1.6.0a
OCC version: 6.7.0
Attachments
dishwasher_part_v2.fcstd
(16.7 KiB) Downloaded 3 times
jmaustpc
Posts: 8074
Joined: Tue Jul 26, 2011 6:28 am
Location: Australia

Re: Map sketch to face unwanted reorientation

Postby jmaustpc » Sun Mar 19, 2017 1:12 pm

Your first post, welcome to FreeCAD.

tojape wrote:Version: 0.14.3702 (Git)


Your FreeCAD version is rediculously obsolete, update to the last release version, 0.16. You will find a huge range of updates and bug fixes.
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NormandC
Posts: 12069
Joined: Sat Feb 06, 2010 9:52 pm
Location: Québec, Canada

Re: Map sketch to face unwanted reorientation

Postby NormandC » Sun Mar 19, 2017 5:08 pm

Hello,

jmaustpc wrote:Your FreeCAD version is ridiculously obsolete

Agreed. Fixed typo though ;)

If your Linux distribution does not provide a fresher version, you'll have no choice but to compile FreeCAD yourself. See CompileOnUnix

A quick search indicates antiX is based on Debian stable (currently jessie I'm guessing). The jessie-backports have the latest release 0.16.670x, but as I am not a Debian nor antiX user, it's not my place to recommend you activate the backports.

tojape wrote:When I try to map a sketch to a face (on a pad created from sketch Body_section) FreeCAD rotates the sketch by 90 degrees. I obviously do not want this behaviour.

You may not want this behaviour, but you are stuck with it nonetheless. When mapping a sketch to a face, it adopts the face's coordinate system. Up to and including 0.16, there is simply no way around that.

In current 0.17-dev, a new super-Placement property was added that allows to rotate the sketch on top of the face. But 0.17 brings many changes and is not ready for release yet.
bejant
Posts: 4091
Joined: Thu Jul 11, 2013 3:06 pm

Re: Map sketch to face unwanted reorientation

Postby bejant » Sun Mar 19, 2017 5:13 pm

Edit: I see Normand also posted while I was looking at your model...

Hi tojape, and welcome!

tojape wrote:When I try to map a sketch to a face (on a pad created from sketch Body_section) FreeCAD rotates the sketch by 90 degrees. I obviously do not want this behaviour.

When we Map a Sketch (say Sketch B) to a face of an existing object that was created from Sketch A, Sketch B inherits the coordinate system of Sketch A. In your file the solid was created from a Sketch on the Y-Z Plane, and all the other Sketches are created on the X-Y Plane, so Mapping the other Sketches after Body Section onto yous solid changes the coordinate system of those Sketches. Usually we don't create all the Sketches at once, but instead create new Sketches on faces of the newest solid as we go along creating the model.

For your file instead of first creating a solid from the cross-sectional side profile, create a Sketch of a rectangle in the X-Y Plane and Pad that. Now Mapping your subsequent Sketches on the the new solids as you go won't change the orientation except for Upper_cut. For Upper_cut, after Mapping it to a face of the preceding Pocket, while in Sketcher select all your geometry, then the horizontal axis, and apply the Sketcher Mirror Geometry tool (Part Design pull-down menu > Sketcher tools > Symmetry). It is not this tool:
Image (I would have included the image of the tool to use but didn't see it on the wiki Artwork page)

The resulting model is something like this (using the default 5mm for Pockets):
20170319a.png
20170319a.png (5.62 KiB) Viewed 33 times

so you'll have to add the hump and Pocket away the curved groove on the bottom. Here's the file:
20170319a-016-dishwasher_part_v2.fcstd
(67.13 KiB) Not downloaded yet


I used:

OS: Ubuntu 16.04.2 LTS
Word size of OS: 32-bit
Word size of FreeCAD: 32-bit
Version: 0.16.6707 (Git)
Build type: None
Branch: releases/FreeCAD-0-16
Hash: 5465bc47c95db45e0be85dc0e2872419efadce0f
Python version: 2.7.12
Qt version: 4.8.7
Coin version: 4.0.0a
OCC version: 6.8.0.oce-0.17
My Part Design tutorials on YouTube (aimed at beginners).
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NormandC
Posts: 12069
Joined: Sat Feb 06, 2010 9:52 pm
Location: Québec, Canada

Re: Map sketch to face unwanted reorientation

Postby NormandC » Sun Mar 19, 2017 5:30 pm

Hi,

bejant wrote:(I would have included the image of the tool to use but didn't see it on the wiki Artwork page)

I prefer to use the icons from the workbench or command pages myself, because they are in 32x32px png format, while the ones on the Artwork page are SVG, which do not scale down.

I usually remember most of the command page names, so I type the page name, place it between wiki tags, click on Preview, then I click on the generated link to open the wiki command page; then I right-click on the icon in the wiki page and select "copy image link" then paste here inside Img tags.

If I don't know the command page name, I simply go the the workbench page: Sketcher Workbench and locate the icon I need.

Image Sketcher Symmetry

I find it's much faster than trying to find a needle in that haystack that is the Artwork page! Not even mentioning how long it takes to load. ;)