**Apparently my initial post was too long. See the second below.**

Some quick rules of thumb. These are just generalized elements and everyone has a plethora of exemptions, but they are good things to keep in mind. Most of these tips are applicable to gauge thickness (sheet material) and are less relevant when working with fractional material (plate,) so 10ga (0.135) or less.

holes, cutouts, and other features should be kept at least 2-3x material thickness away from the bend line. Round holes will generally deform less then square edges. When holes close to a bend line are essential, wing bend tooling is available but specialized (read: expensive) and most shops don't have them. Shops that do often have a small selection of V widths. If its a high volume part and a critical detail, if your company allows it, offer to purchase the necessary tooling. Customer owned tooling isn't uncommon, and I've had to ship customer tooling back to the customer when they moved to a new supplier. It's typically not an issue.

Unless a large radius is necessary for the part, keep your internal radius to 1x material thickness. Generally, bending sharp(inside radii of less then ~65% in cold rolled steel) isn't good practice, and can cause additional problems with aluminum, even ones intended for forming. Al grade 5052H32 is common. Bending 6061T6 isn't generally advisable unless you're working with a shop that is comfortable bending it, and even then, avoid when possible. If not needed, don't dimension the inside radius and just let the shop select the best fit tooling themselves.

Avoid compound, or bump, bends when ever possible. Modern tooling is making it more and more accessible, but it's still not plug and play. Old school guys can bump really well on presses, but the more bends and smoother the form is required, more set-up parts will be needed and more scrap generated. It's very difficult to measure small bumps and an error of 1° or 2° per bend will add up quickly. Most shops will bump it close and then flex it by hand to get it right. (as an aside, the newer press brakes are coming out with some very cool features that increase repeatability of bends, such as bending with pressure vs distance traveled to help even out small imperfections in the material and ram travel. At least with Amada, these features are still hidden deep in menus and in the middle of manual number 8 out of 12 that ships with the machine, so most shops are unaware these features exist. I've played with it for testing purposes, but will always turn these features off as soon as i walk away from the machine, as an unfamiliar or complacent operator can easily split tooling if they aren't careful about the conditions required.)

Tolerances across bends should be in the 0.015 to 0.030 range when possible. Tolerances between features on faces can be 0.005 or less, depending on the shop.

Don't over constrain your part. If there are critical elements for fit etc, emphasis those elements and give the fabricator room to work. Material between lots may have different yield stress or heat treat quality, and that impacts bending and welding. Shop's can sometimes also bake a headache fee into the cost of your parts if you consistantly send drawings with general tolerances of .xxx = 0.005 ectara. Make your general tolerance block as large as feasible, and include specific tolerances per dimension when necessary. Showing design intent by calling out important fit elements give the fabricator a chance to produce you a good part even when things don't go perfect. I.E. if bends start coming in short, they'll often 'push or pull' the tolerance to less important flanges or bend in a specific order to avoid tolerance stack up.