SheetMetal AddFoldWall/pl

Description
The SheetMetal AddFoldWall command folds a sheet metal plate (blank) at a chosen line.

It can be used with a pre-cut blank to
 * create a perforated bend zone
 * leave planar sections within the bend area and beyond e.g. tabs. (needs gaps in the bend line)



Usage

 * 1) Select the face to be bent.
 * 2) Hold down the  key (or the  key on macOS).
 * 3) Select the coplanar [[Image:Workbench_Sketcher.svg|16px]] sketch (i.e. lying on the same plane) containing the bend line (segments) (preferably from the tree view).
 * 4) Release the  key (or the  key).
 * 5) Activate the [[Image:SheetMetal_AddFoldWall.svg|16px]] SheetMetal AddFoldWall command using one of the following:
 * 6) * The button.
 * 7) * The menu option.
 * 8) * The keyboard shortcut: Then.
 * 9) Change the value of the property  to adjust the position of the bend according to the bend line.



Properties
See also: Property editor.

A SheetMetal Fold object is derived from a Part Feature object and inherits all its properties. It also has the following additional properties:

Data

 * : Default value: (+ a sequential number for second and following items). The user editable name of this object, it may be any arbitrary UTF8 string.
 * : Base Feature. Link to the parent feature.
 * : Hidden link to the parent body.


 * : "Bend Reference Line List". Links to the bend line objects.
 * : "Bend Line Position". (default),,.
 * : "Bend Angle". Default angle:.
 * : "Base Object". Link to the planar face to be bent.
 * : "Invert Bend Direction". Default:
 * : "Invert Solid Bend Direction". Default:  swaps the side of the line to be bent.
 * : "Neutral Axis Position". Default:.
 * : "Bend Radius". Default:.
 * : "Unfold Bend". Default:

Preparation
This clip is made of a blank that receives three folds and so we need four sketches prepared in advance:
 * - one for the outline plus slot (blank)
 * - one for the bend at the tip
 * - one for the upward bend
 * - one for the downward bend

Easiest way to guarantee that one face of the blank and all folding lines are coplanar is to create all sketches on the same plane - the XY_Plane in this case.

The folding lines could be created with other tools but hey, we have a Sketcher!



Workflow
Done!
 * 1) Create a blank
 * 2) Select the outline sketch
 * 3) Press the  button or use the keyboard shortcut:  then  [[Image:SheetMetal_AddFoldWall-02.png|120px]] [[Image:SheetMetal_AddFoldWall-03.png|280px]]
 * 4) Fold the tip
 * 5) Select the blank's bottom face
 * 6) Select the sketch named Tip Fold line (preferably from the tree view) (and don't forget the control/command key )
 * 7) Press the  button or use the keyboard shortcut:  then  [[Image:SheetMetal_AddFoldWall-10.png|120px]] [[Image:SheetMetal_AddFoldWall-04.png|120px]] [[Image:SheetMetal_AddFoldWall-05.png|280px]]
 * 8) The fold should be 90° down and so some values in the properties window need to be set e.g.: - the angle value to 60° - the invert value to true for an upward bend
 * 9) Create the downward fold
 * 10) Select the blank's bottom face
 * 11) And then the sketch named Down-Fold line
 * 12) Press the  button or use the keyboard shortcut:  then  [[Image:SheetMetal_AddFoldWall-11.png|120px]] [[Image:SheetMetal_AddFoldWall-06.png|120px]] [[Image:SheetMetal_AddFoldWall-07.png|280px]]
 * 13) Set the angle value to 92°
 * 14) If the wrong section of the part moved set the invertbend value to true
 * 15) To create the upward fold
 * 16) select the blank's bottom face
 * 17) and then the sketch named Up-Fold line
 * 18) Press the  button or use the keyboard shortcut:  then  [[Image:SheetMetal_AddFoldWall-12.png|120px]] [[Image:SheetMetal_AddFoldWall-08.png|120px]] [[Image:SheetMetal_AddFoldWall-09.png|280px]]
 * 19) Set the angle value to 80°
 * 20) If the fold is downward set the invert value to true
 * 21) If needed set the invertbend value to true

Note!: In real life the upward fold must be done before the downward fold. Only the virtual world of CAD allows us to bend through solid material. This way the orientation of the static section doesn't change. All sketches lie on the same plane to avoid sketches attached to moveable faces.