[SOLVED] Rotating an object in its own axix

[however]

Hi again,

Straihgt to the question, in case it wasn't clear from the topic title:

How do I rotate an object in its axis?

I thought it would have been as simple as changing degree in axis X,Y or Z however, when I do that it seems that the object rotates in space (maybe because I still don't have a clear understanding of drawing in 3D).
It has been two days (and partly, nights) and i am going crazy trying to find out how to rotate an object, i.e. a chair, desk, etc... in its own axis; example: instead a having a chair facing straight to a wall i would like to rotate it of 45 degrees to face the window instead.

In this video tutorial http://www.youtube.com/watch?v=hw9otd_hzb8, the author rotates the truck of 90Degrees at 1.04'' through a 'Rotation' option that I don't/can't find.

Any help would be gladly welcomed.

Regards,

[ulrich1a]

In this video tutorial http://www.youtube.com/watch?v=hw9otd_hzb8

This tutorial is with version 0.12 of FreeCAD. Things have a little changed.

The property editor still has the placement property with the angle and an axis setting. It works now different, as this operates on an quaternion. For simple rotations, you can set your axis, and then change the angle. Additional rotations around another axis get complicated.

Another method is to double click on an object in the document tree. You then get an item around the shape and can drag and rotate the shape in 3D-space. In order to get rid of the draging thing: right click on the object in the tree and select finish editing.

Ulrich

[jmaustpc]

Go to the edit menu....Placement...then either in relative or absolute mode...set the centre of rotation in the section named "centre" ......

[mario52]

hi
here a documentation on Placement
mario

[wandererfan]

How do I rotate an object in its axis?

I thought it would have been as simple as changing degree in axis X,Y or Z however, when I do that it seems that the object rotates in space (maybe because I still don't have a clear understanding of drawing in 3D).

I would guess that your object's "centroid" is not the same as it's reference point. See the documentation mario52 recommended, especially "Using "Center" to Control Axis of Rotation".

wf

[however]

HI all

and thank you for your helpful hints.

When i said 'object' I meant something I created, i.e. chair, desk, etc

Another method is to double click on an object in the document tree. You then get an item around the shape and can drag and rotate the shape in 3D-space. In order to get rid of the draging thing: right click on the object in the tree and select finish editing.

this works very well with standard 'Objects' such as cylinder, cube, etc. (which by the way it's also a very helpful tip, as I didn't know). However, my desk, for example, is composed of a Pad and a few Pockets and when I dbl click on it the property window comes up and not the axis as you mentioned.

I will try the other suggestions shortly.

Thanks again.

[ulrich1a]

this works very well with standard 'Objects' such as cylinder, cube, etc. (which by the way it's also a very helpful tip, as I didn't know). However, my desk, for example, is composed of a Pad and a few Pockets

Those parts are not movable easy. Parts made with the PartDesign workbench will not move, as their Placement depends on the first sketch for example. You can do either a simple copy of this part in the Draft workbench and move this copy around. Or you need to figure out wich is the first element in the document tree, which holds the placement. For example a part which is based on a sketch and has a Pad from the PartDesign workbench, then you have to move the underlying sketch.

The user Andre has made some useful macros, which finds the base feature of a part and a macro which regenerates the document tree, if you have unhide some elements in it and are lost, because you do not know which are the elements with the latest features in the document tree. Unfortunatly I have do not a link to his post.

I wonder that Quick61 did not show you his famous macro about part movement.

Ulrich

[jmaustpc]

Edit I see Ulrich responded while I was typing ...and having my Internet connection dropping in and out...


Be aware that for objects made in PartDesign wb, you can only adjust the placement of the first sketch upon which the solid was made. The placement of everything else in the hierarchy is determined by this first sketch.


The Assembly workbench will perform this function when it arrives.


As a work around, if for some reason adjusting placement via the first sketch is not convenient, you can either go to the Part wb and create a "simple copy" (from the Part menu) which will not be parametric...or go to the Draft WB and create a Clone which will be parametric, in both cases you can use Placement tool, Alignment tool, Draft move and snapping, on the clone or copy.

Jim

[however]

Thank you All.

That was very helpful.

Regards,

p.s.: I only wonder why such a user-friendly option for Parts rotation/movement that was apparently available on FreeCAD 0.12 (as mentioned above) is not on newer version,

[triplus]

As already said in this thread and mentioned on the link mario52 gave:

http://www.freecadweb.org/wiki/index.ph ... ent#Issues

Issues

As of version 0.13, update of Placement properties in the Data tab has been disabled for objects created with PartDesign, except for the initial sketch from which the solid will be created. Therefore the Placement of a solid created in PartDesign from a sketch can only be altered by adjusting Placement parameters of the initial construction sketch (the first sketch) from which the solid was created.
Placement functionality will eventually be handled in the Assembly workbench.

This will be handled by Assembly Workbench in the future and FreeCAD already started to adopt that fact in the past (FreeCAD 0.13).