Basic Attachment Tutorial



This tutorial should serve as an introduction to Part:Attachment, it is not comprehensive, but hopefully will help users experiment. Written for V0.19, but should be valid for any version 0.17 and later.

Pre-requisites

Before attempting this tutorial users should :-
 * 1) Use version 0.17 or greater.
 * 2) Be comfortable navigating the FC 3D view.
 * 3) Be able to make and constrain a sketch.
 * 4) Have a basic understanding of the Part Design workbench.

Preliminaries

Before we start let us examine at how we should go about building this model.

From whichever angle we look at it, we see a square or rectangle with a corner trimmed off.



There is however an obvious axis from which all features are common



We could make a sketch on any of the major planes. We could include a trimmed corner in our base sketch, but let's forego that and include an extra sketch and pocket, for learning purposes. We will start with a block and pocket the excess away.

Switch to Part Design workbench, open a new document, create a body and a new sketch on the XY plane.

Sketch a rectangle, centre it on the origin, constrain with a length(Horizontal) of 70mm and name it "length", further constrain it with a width(vertical) of 40mm, and name it "width".



If we leave the sketch where it is, things would be too easy. We'd have planes and axes in all the correct places, No, let's change the sketches position by altering it's attachment offset.

In the combo view, look in the Data tab, find attachment Offset and expand it, by clicking the plus sign next to it.

Do the same for the Position sub heading. Change the X offset to 80mm, and the Y offset to 90mm. The Sketch can now be padded, let's pad to length of 40mm and tick symmetric to plane.



So now we have a pad, and because we were wise, we have planes and reference axes in all the correct places. This is going to be easy :-)