Marc3 is correct that a sketch becomes automatically hidden if turned into a feature and that non-feature sketches are automatically visible.
However, what caught my eye was the title of this request and that is "hide bend lines in a drawing". When we make sheetmetal parts we automatically make two configurations; Formed and Flattened. This is so that in our drawings we can show the formed part that we want and on a separate sheet, for reference only, we show the flat pattern. We are careful to indicate on this flat pattern the method used for its derivation, i.e., K-factor of .3214 with bend radius of .060" and material thickness of aluminum of .063", etc.
On this flat pattern we like to show the bend lines so that we can show a dimension from the reference edge and denote BU or BD (for bend up/down). We just show BU or BD if the bends are 90 degrees, otherwise we put BU 45 for bend up 45 degrees.
To either hide or show the bend lines in a drawing you must expand the feature manager for that drawing view. Keep expanding the levels until you get to the sketch inside the Flatten-Bends sheetmetal feature. Here you can make the sketch visible or hidden RELEVANT TO THIS DRAWING VIEW. This is an important point. We initially thought that we could control the visibility of this sketch in the part file itself in the flattened configuration. However, this is not the case (and it turns out to be for good reason).
You can easily control the visibility of the bend lines in your drawing, but you have to do it from within that drawing view.
I hope this is helpful.
- - -Dennis D.
P.S. We often will draw center/construction lines in the drawing view and constrain them to be colinear to the entities in the bend line sketch. Then we hide the bend line sketch. This gives us more control over the appearance (length, style, density) of these construction lines.
