Sheet metal bend cost 4

[macatc123]

Hi all, I have a sheet metal question. I am going to have a sheet of 4mm thick carbon steel bent at 90 degrees. My current design calls out a bend radius of 20mm. The shop just got back to me and said it will be cheaper if they bend the flange at the standard bend radius. They said if they bend it at 20mm radius, then they would have to use a special die for this.

I am assuming a sheet metal shop would have the equipment to bend a 20mm radius flange. I don't understand how this would increase cost. Any insight? Thanks

 

[MintJulep]

"...at the standard bend radius..." If you want to have a bit of fun, asd the shop to cite the number of that standard.

What they mean is "...at a radius that we already have a die for..."

Obviously if they don't have the necessary die the will need to either make or purchase one. And they will pass that cost on to you as a "tooling cost".

Ask around. You might find another shop that already has the necessary die on hand.

Or, ask the shop you are dealing with now what they can do. I wouldn't be surprised if they say they can do 3/4".

 

[KENAT]

Like Mint says, if in the US it may be as simple as they usually work with fractional inch sizes. Did they tell you what their standard radius radii is/are?

http://sheetmetal.me/air-bending/

Posting guidelines faq731-376

http://eng-tips.com/market.cfm?

(probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484​

 

[TheTick]

I'm sure your assumption is based on the fact that 20mm is a nice round number and that everyone should be well stocked with items that have nice round numbers associated with them.

 

[macatc123]

Hi guys, thanks for the help. I should mention that this will be produced in Asia. TheTick, honestly yes. I thought they would have a 20mm die on hand. I'm not a sheet metal expert but I figured they would have all sorts of dies. I will ask them what dies they have.

 

[drawoh]

macatc123,

20mm may be a large radius for a sheet metal bending die. Ask them what they have.

My understanding is that they can bend any radius you want. If you get weird, they "bend in air". This is a more expensive and a less accurate process. It may require a significant level of operator skill.

--
JHG

 

[TheTick]

If you are new to sheet metal bending, talk to an expert yesterday and learn fast. Save yourself time and money by learning what is truly "standard".

Typical sheet metal bending is done with a radius roughly equal to the metal thickness. Hard metals closer to 1.5 times thickness. Much bigger, and it becomes difficult to control the form. Too small, the metal will crack.

There are standard tools in catalogs. However, I find many small shops have their own favorite tools on hand and are not too keen on building or buying more. Especially true if you are a small-time guy making small quantities.

If you can design in such a way that you can be flexible about actual bend radius, metal shops can find a way to help you save money using what is available.

Use what is abundant to make what is rare.

 

[ornerynorsk]

There is no "standard". Your material selection dictates the minimum radius that the part must be bent at. You will always save time and money by using tools that the shop has on hand.

It is better to have enough ideas for some of them to be wrong, than to be always right by having no ideas at all.

 

[moon161]

Standard means die is on the shelf, or better yet, on the brake. If they have to change or buy a new tool, and then change it back, you pay the cost for tooling, labor and disrupting the flow of other material in the shop. I'd find out what works for them, and see if it works for you. Do you gain anything by using your particular radius.

 

[MadMango]

Successful (and inexpensive) sheet metal work/design requires close cooperation with the designer and the manufacturer. Once you select a sheet metal vendor, you need to know what tooling they have on hand, and plan to design to that limitation or you will incur added costs. This is especially true if you have punched features instead of paying for laser-cut features.

"Art without engineering is dreaming; Engineering without art is calculating."

Have you read faq731-376 to make the best use of these Forums?

 

[tbuelna]

As others noted, if this is a brake forming operation you need performed by a US vendor, then change the inside bend radius to an inch increment like .75" or 19mm, which is only .037" smaller than 20mm. However, the typical inside bend radius for brake formed mild steel is around 2.0T, which would be an 8mm (or .31") radius for your 4mm thick material.

 

[Tunalover]

Good luck ever getting a list from the shop of what dies they have! Nobody ever seems to find the time to catalog what dies are on hand. Instead they often rely on memory which is not good at all!



Tunalover

 

[3DDave]

Tunalover - some shops remember having every die you need, until they get the contract. Then they look at the drawing and realize there's only one size they don't have. Then an on-site visit shows they actually only own a few, but purchasing selected them as lowest bidder and provisional approval.

If this has never happened to you it's only luck or your charming personality, of which I have neither.

Worse is needing a box die; they never have the right length so the bend gets sloppy somewhere along the way.

 

[mcgyvr]

Good luck ever getting a list from the shop of what dies they have! Nobody ever seems to find the time to catalog what dies are on hand. Instead they often rely on memory which is not good at all!

EVERY sheet metal house we use has always given us a list of their tooling when I ask for it (punches/forming dies,etc..).. They all track it somewhere (mostly in excel).
It helps me when I'm designing a part as I simply pick from their list of the shapes/holes/corners/obrounds,etc.. saves the back and forth time of "we don't have X can you use Y"


Back to the OP..
Get a few catalogs from the tooling makers like..

http://marketing.wilsontool.com/acton/attachment/8311/f-00f0/1/-/-/-/-/2bc_americanpb.pdf

http://marketing.wilsontool.com/acton/attachment/8311/f-00f4/1/-/-/-/-/2bc_europb.pdf

Most have just about everything "standard" in these catalogs. 20mm is very large for a 4mm sheet IMO and would be "custom" for one vendor while another would have it.
Like everyone else said.. simply ask the vendor "well then what do you have thats close to that without going custom?" and see if that works for your application.

Most press brake tooling in the US comes standard with a radius in inches of (.031/.062/.125/.187/.250)

 

[Tunalover]

mcgyvr-
You are fortunate to work somewhere that has such good suppliers that take the "trouble" to tell you what they have. That's a great arrangement indeed!


Tunalover

 

[JayMaechtlen]

4mm is on the heavy side for sheet metal, and 20 mm is a large radius.
When air bending, springback is a significant factor in accuracy and repeatability.
If you want an accurate bend at that radius, you need consistent material and good equipment at the least.
For consistency bends are often done by 'coining', where the press drives the punch and material into the die to make sure most or all of the material has gone into yield.

The thicker the material, and the larger the radius, the more tonnage it takes to drive the material into yield. (depending on bend length, may require a bigger press)
And the tooling has to be heavy enough to withstand that usage.
fun, fun, fun.


Jay Maechtlen

http://www.laserpubs.com/techcomm