Best practices in designing... thickness and bend radius?

[SHOBrad]

Hi all, I'm a Mechanical Engineer that has been tasked with trying to standardize some design practices in the company I work for and had a few questions I wanted to clear up. I've searched for these answers without much success.

First off, we use the typical sheet stuff (I think). cold-rolled, 304 SS, galvanneal and aluminum. Mostly 16ga-11ga, sometimes 10ga. 99.9% of our stuff is lasered. We typically work with smaller fab shops (at least for prototyping)

My questions:
1) If I say I need this x part formed up, is there a go-to inside bend radius? We use 1/16" radius for about everything but is this ideal? Is there a best radius buy thickness? Is there tooling that shops typically keep in the brake press all the time?
2) Is there a minimum (no special operation or holding your thumb right) leg length based on this and the bottom tool? and with that is the bottom tool standard?
2) Do most shops specify material by gauge or thickness? Is this true for all sheet or just certain materials? Are all thickness available and typically kept in stock?

Thanks in advance. Trying to get my group standardized and want them to design to best practices to get the best parts.
Brad

 

[memphisjed]

in an air bend like job shop press brake the perfect bend is 1 thickness to 1 inside radius. 1.25 < radius/thickness >1 is expected. The flat length is very shop dependent: 8x thickness is very reasonable (6x is normally not an issue). If you have good relationship with shop then that number can go down, cost goes up.
Gauge is used for less than 3/16" material, sometimes 1/8" is used - but rare. Oz is how fancy material is defined in thickness (yey- really weird).
Different shops keep different material in stock at all times. A shop doing lots of air ducts will keep galvinized in stock, one that does stair pans has 10 gauge in stock.

 

[Scruffy887]

Trumpf has a nice Android app for die width/thickness/min flange dim, and a whole lot more. Pretty sure it is free as I never paid for it. Most all of my punches have a 1mm nose radius, all air bending from thin up to 10 gauge. 12 and 24 mm bottom dies for all that I need. So far.

 

[TDegenhart]

Talk to the people running the presses about what they can do and can't do. You will be amazed at the knowledge and experience these people have. Tell them you know little or nothing about fabbing sheet metal. Should you get an order for something outside the normal range, talk it over with them. They make your life easy or hell depending how you treat them.

Tom

 

[Nmbmxer]

memphisjed;
1.25 < radius/thickness >1 is expected.

This mirrors my experience along with a typical K factor of 0.4.The bottom die opening / min flange length is harder to estimate. If you have preferred suppliers, ask for a tooling list and you can do a better job designing parts that are easily made.

 

[rogertoolmaker]

Hi all, I'm a Mechanical Engineer that has been tasked with trying to standardize some design practices in the company I work for and had a few questions I wanted to clear up. I've searched for these answers without much success.

First off, we use the typical sheet stuff (I think). cold-rolled, 304 SS, galvanneal and aluminum. Mostly 16ga-11ga, sometimes 10ga. 99.9% of our stuff is lasered. We typically work with smaller fab shops (at least for prototyping)

My questions:
1) If I say I need this x part formed up, is there a go-to inside bend radius? We use 1/16" radius for about everything but is this ideal? Is there a best radius buy thickness? Is there tooling that shops typically keep in the brake press all the time?
2) Is there a minimum (no special operation or holding your thumb right) leg length based on this and the bottom tool? and with that is the bottom tool standard?
2) Do most shops specify material by gauge or thickness? Is this true for all sheet or just certain materials? Are all thickness available and typically kept in stock?

Thanks in advance. Trying to get my group standardized and want them to design to best practices to get the best parts.
Brad

An easy way to Standardize for the bend radius. If the sheet is 1/16", use 1/16"radius punch. If 1/8" use 1/8" radius punch, etc. Above 1/8" thick use 1/8" radius. The bend radius should be called out on the Part Print.

Roger

 

[rogertoolmaker]

When bending sheet metal, the inside of the bend compresses and the outside of the bend stretches.
To figure the developed length of the bend for the flat pattern of a part.
The sin 1 degree x arc x (inside bend radius + 1/3 stock thickness) = developed length around the bend.
There's a sweet spot for figuring the allowance for bending sheet metal to allow for the bending and stretching around the bend. Add 1/3 stock thickness to the inside radius.

Roger

 

[Strostkovy]

I like the punch radius and the material thickness and bend radius to be the same. It makes for consistent forming.

I use 4-12 times the material thickness for the die. The flange you can get away with is the total width of the v die including the shoulder radius. A die may have a 1/2" opening but the radius on the shoulder makes it more like 5/8", limiting you to 5/16" for the majority of the bend. Part of the contour can go down to half the theoretical V-die width (1/4" in the example above) and holes up to 2-3 times the diameter of the sheet can be placed on the contact line of the die with acceptable results.

You will also want to put a lot of thought into bend reliefs, the desired gap for open corner fitups, material tempers, overnotching for reverse bends, and special considerations to prevent cracking at the ends of bends. I know 1/4" steel will often crack at the edges of 1/4" radius bends but it doesn't matter to us because weld it.

Consider that you also shouldn't just make a bend guide, but it should be a sheet metal guide in general. Have a running list of hole sizes for common fitups, weld nuts, tapping, threaded inserts, etc. Parts should have radiused corners where possible for more efficient material handling, and should not have geometry that causes it to unnecessarily lock into the sheet (square bend reliefs are terrible for this).

Establish a size and application list for indication notches that aid the press brake operator in correctly locating the bend. These are not bend reliefs and do actually make cracking issues worse.

For bend reliefs on a straight edge, you need to measure the flaring produced by a given radius and the width of the flaring, then call out for a shallow dish looking cut in the contour.

Offset bends are limited by the external die width and height. Figure out the dimensions for these.

Get a good measurement for k factors, as well as an actual measured bend allowance on 90 degree bends.

Avoid slots in sheet metal tighter than 0.1" or the material thickness (just an example for our laser) and try to leave a spot in cutouts for the laser to pierce.

Stiffener flanges often have edges tapered in for aesthetics. Determine the acceptable angle for this. I like 60 or 75 degrees. 45 degrees tends to flare badly.

I'm sure there's more but this is all I can think of off of the top of my head right now.

 

[Strostkovy]

An easy way to Standardize for the bend radius. If the sheet is 1/16", use 1/16"radius punch. If 1/8" use 1/8" radius punch, etc. Above 1/8" thick use 1/8" radius. The bend radius should be called out on the Part Print.

Roger

I personally disagree. We use a 0.04 radius punch on everything up to and including 10 gauge (0.135) and jump up to a 1/4" radius punch on everything 3/16 and up. We do have some specialty sizes (0.02 and 0.16) in short lengths.

Not that you will get bad results the way you mention, I just personally find the clean inside radius and matching radii between the punch and bend makes nice, repeatable bends.

I acknowledge that there is a limit in how much you can spend on tooling and that compromise must be made, and that there are many strategies possible.