Hello sunjapo,
sunjapo wrote:So, could you tell me how to move the revolution axis in Ver. 13 as he did with Ver.12 in the video?
I just viewed the video again, I had not seen it since last year.
I don't understand why you want to duplicate John's process, as I said the Revolution parameters were very confusing back then - John struggles from 01:36 to 04:35 to get the revolution as he wants it. Now it's much, much easier.
In John's video, the first parameter he sets is the revolution axis (Axis). This gives the axis vector by using an XYZ value: for an axis parallel to X axis the value is (1,0,0), for Y (0,1,0) and for Z (0,0,1). Non-zero values in more than one field would give a slanted vector on 2 or 3 planes. Because the axis value sets the axis at the origin, the base value was required to offset the center point of the axis so it meets the sketch plane.
But it makes no sense to explain this obsolete process further, because the new method is totally different.
I quickly made a simplified sketch compared to John's to show you how the Revolution tool works in v0.13. As with John's it was drawn on the XY plane, with the profile centered on the Y axis and the bottom coincident to the X axis. Here I activated the "axis cross" at the origin from the menu View --> Toggle axis cross.
- FC_PartDesign_Revolution_01.png (16.63 KiB) Viewed 7653 times
The blue line is a construction line, to be used as revolution axis. It is contained in the sketch, this resides on the same plane as the profile to be revolved.
- FC_PartDesign_Revolution_02.png (5.96 KiB) Viewed 7653 times
Notice that once you exit the sketch editing mode, the blue construction line is hidden from view.
Now we start the Revolution tool. Here's what the Task panel shows:
- FC_PartDesign_Revolution_03.png (38.95 KiB) Viewed 7653 times
"Vertical sketch axis" is the default selection, as it is the first in the drop down list. In the 3D view, you don't see any change, and in the Report view, this error message in red: "Revolve axis intersects the sketch".
What does this error mean? The vertical axis is in reference to the sketch. Since this sketch is on the XY plane, the vertical sketch axis corresponds to the global Y axis.
My profile is crossing the Y axis, which is no longer allowed, because if you are to make a 360 degree revolution, the material will overlap on itself, and create an invalid shape. So for this parameter to succeed, the profile would need to be on either side of the vertical sketch axis, but not both.
Now I change the Axis to "Horizontal sketch axis", and to better show the result I set the angle to 90 degrees and tick the reverse check box:
- FC_PartDesign_Revolution_04.png (6.8 KiB) Viewed 7653 times
We're now seeing a 3D solid, because the horizontal sketch axis is aligned to the global X axis. Notice the small visual imperfection on the conic surfaces. I believe FreeCAD does not like the fact that the bottom point of the profile is on the global origin point (0,0,0), which means it intersects the axis and creates a solid that ends at the center on a point. In CAD software, this kind of situation can often fail; although if I choose to rotate 360 degrees, the imperfection disappears.
But this is not the shape we want, we're after a bike rim so it should have an inside diameter value of some kind - this revolution has none. So I select the last choice in the axis drop down list, "Sketch axis 0" which represents the blue construction line.
- FC_PartDesign_Revolution_05.png (24.08 KiB) Viewed 7653 times
Now this is what we're looking for. To set the revolution distance between the axis and the profile, you only need to edit the sketch and move the line. Here I have not put any dimension to constrain the profile and the construction line, but I should have. So this is much easier than playing with the Base value like in v0.12.
If you want the revolution axis to be at an angle instead of parallel to the X axis, no problem - edit the sketch, delete the horizontal constraint on the construction line and rotate it:
- FC_PartDesign_Revolution_06.png (23.3 KiB) Viewed 7653 times
Or put it parallel to the Y axis:
- FC_PartDesign_Revolution_07.png (19.04 KiB) Viewed 7653 times
In all these options, the revolution is centered on the XY plane because that's where the sketch resides. If you want to change this, move the sketch's position by changing its coordinates.
- FC_PartDesign_Revolution_08.png (30.77 KiB) Viewed 7653 times
I'm attaching my file so you can have a look at it. Edit the Revolution parameters by double-clicking on its label in the Project tree, then play with the options. I also recommend you edit the sketch, and delete the horizontal constraint on the blue construction line. Then set your view to isometric, click on one of the blue line's points, and drag with your mouse; when you release the line, see the Revolution update automatically - very cool uh?
FreeCAD
