[Solved] Double offset

[jfc4120]

FC: .20 REV 29177

First I can sweep a pipe or square/ rectangular if both ends are the same. However I am attempting a double rectangular offset: here are some images:



I can't seem to position the rectangle and the square correctly in sketcher mode. If just one shape no problem. I even tried a move afterwards but all move together even if I select only the square.

Any help would be appreciated. I watched some Youtube videos, but they already had the shapes and just demoed the sweep. I need help in positioning these in sketcher.

[chrisb]

I would rather use Loft than Sweep. Use ruled surface.

[jfc4120]

That would restrict airflow. Bear in mind those are compound miters joints.

Edited:

The closest I've come is:



I can only get a constant size throughout. I have messed with all the settings, yet I cannot do an additive pipe from one shape to another. What little thing am I missing? One end is supposed to go to the rectangle. Also ignore the line it was just to help position. It wasn't part of the objects in the sweep.

[Bance]

The Pipe(sweep) function in PD WB has a multi-section option in the tool dialogue, however this is not terribly useful in this case.

In fact because the offset is in two directions it would make more sense to model in Part WB. The single solid body makes it awkward in PD.

Anyhow I made it in PD, I used a method developed in the German forum to create a 3D wire (basically model a surface in two directions and Part section.) This wire can be imported using a shapebinder and the compound angles are derived from it. Then it's simple case of pad 'up to face' in separate bodies then a loft and finally a Bool union.

I'm pretty sure the model could be cleaned up, with a little thought.

doubleOffset.png (11.32 KiB) Viewed 981 times

Edit: changed Bool for section

[papyblaise]

some sheet metal that's all

[Bance]

some sheet metal that's all

But it's the same at both ends, OP doesn't want that.

[domad]

........

Hi jfc4120, greetings to the Community!
Sometimes it is necessary, in my opinion, to perform a 3D construction to determine "precise sections" of the transition, then proceed with the Loft.
The image of the book page, "Fig. 355 .--- Transitional Offset", is suitable for putting this method into practice.
The animated gif that shows the 3D construction, abusing the term "Stereographic", on the one hand and the result of the Loft function on the other, whose thickness variation is obtained by means of an empty Sketch which has the sole purpose of modifying the thickness.
Two examples are attached: in one the thickness is obtained from the Sketch sequence to obtain a "straight / edge" section transition, in the other the thickness is obtained with the "Thickness" function but the section transition occurs with a fillet.

[papyblaise]

But it's the same at both ends, OP doesn't want that.

not at all, the left section is 70 X height 80, the right is 80 X height 70

[jfc4120]

@domad How did you figure out (calculate) the angle and get face and face001 in the wire? If the mid section in wire can be dimensioned, that's all that's needed to "layout" the offset.

@Bance can you upload image of the first wire you mentioned?

In my first image above, I get the approximate turn angles (angle over, angle down) from a sketch (pencil and paper scaled) then make a plane turn it those angles and slice the solids. Then connect the two with four planes. Works but I'd like to do it in freecad.

In fact, do one of you know the accurate method to figure out the angles, meaning for example 30 degrees down, then rotate plane 35 degrees on other axis. Because a slice and then simple connecting is very easy.

My original was done in designcad 2000. But it can't sweep a complex figure.

[Bance]

I've worked a little on the file, I added a propertybag so you can change parameters easily.

To see the 3D sketch make thickness invisible and section visible.

I left the parameters as an offset because I thought it would be more practical than an angle, but an angle is possible.

To change stuff select the propertybag and change the values in the window.

N.B if thickness breaks you probably need to up something else, changes have to be rational.