AnsweredAssumed Answered

Minimum inside bend radius Senior moment

Question asked by Jack John Frahm on Oct 3, 2017
Latest reply on Jan 3, 2018 by Elmar Klammer

Like • Show 2 Likes2
Comment • 22

Hey peoples!

I am having a minor debate with a co worker about modeling up a simple 90 degree bend. He has "all inside radii to be minimum bend radius" slapped on his drawing and he has then modeled the part with what I think is an impossible to manufacture inside bend radius of .029".

If the part is .250" thick, 5052 material, the inside bend radius at "minimum" can only be 20% of the material thickness? In other words the inside bend radius should be modeled at .200", Correct?

Thanks in advance.

Jack

Kameron Smith Oct 4, 2017 8:49 AM

Correct Answer

I agree with Todd Blacksher. Over years of working with sheet metal, and sometimes operating the press-brake myself, I can confirm that the slots on the large bend radius part will deform when bent. They're just too close to where the punch and die will contact the work piece. Also, the small bend radius will definitely cause serious stress cracks in that work piece.

It's true that a good machinist can cheat the standard sometimes, but why make that a necessity?

See the reply in context

No one else had this question

Outcomes

22 Replies

Walter Fetsch Oct 3, 2017 4:34 PM
Mark Correct
Correct Answer
Wouldn't 20% of .250 be .050?
Like • Show 1 Like1
Actions
- Jack John Frahm @ Walter Fetsch on Oct 3, 2017 5:31 PM
  Mark Correct
  Correct Answer
  Yes. You are correct.
  Like • Show 1 Like1
  Actions
Mike Pogue Oct 3, 2017 4:47 PM
Mark Correct
Correct Answer
Min bend radius for 1/4 5052-H32 is about 3/8. A sheet metal fabricator could tell you how much he'd be willing to cheat on that. You can usually cheat quite a bit--especially if you can tolerate some crazing. I've seen .25 thk 304 SS bent to .03 with no cracking, which I would not have believed had I not held it in my hands.
Like • Show 2 Likes2
Actions
- Mike Pogue @ Mike Pogue on Oct 3, 2017 4:49 PM
  Mark Correct
  Correct Answer
  Also, is .200 a standard radius?
  Like • Show 1 Like1
  Actions
  - Jack John Frahm @ Mike Pogue on Oct 3, 2017 5:32 PM
    Mark Correct
    Correct Answer
    Where do you find "standard radii"?
    Like • Show 1 Like1
    Actions
    - Mike Pogue @ Jack John Frahm on Oct 4, 2017 5:24 PM
      Mark Correct
      Correct Answer
      Call your sheet metal shop. I used to think I knew, but I keep finding new standard sizes, so I don't really know.
      Like • Show 2 Likes2
      Actions
- Jack John Frahm @ Mike Pogue on Oct 3, 2017 5:50 PM
  Mark Correct
  Correct Answer
  I think that is my co-workers argument. The bend can be "cheated" quite a bit depending on the vendor. Our materials group had 4-5 machine shops they keep jumping around too, so it's hard to lock down who has what capability. I like to default to the inside bend radius being the same as the thickness of the material but sometimes design constraints push that. I do not think he was even thinking about the design constraints when he modeled up the bracket. I do not see any issue with opening up the radius to the same dimension as the thickness of material. Potential issue would be a washer not able to sit flush if to far towards the edge of the slot, and that is his push back on the 0.029" radius.
  
  .250" thick material defaults to .375" inside bend radius? that seems eve larger than what I expected. I have found it safe to design the inside radius to the thickness of material do snapshot below shows .250 inside bend radius.
  
  versus .029 radius
  Like • Show 1 Like1
  Actions
  - Todd Blacksher @ Jack John Frahm on Oct 4, 2017 7:58 AM
    Mark Correct
    Correct Answer
    John Frahm wrote:
    
    I think that is my co-workers argument. The bend can be "cheated" quite a bit depending on the vendor. Our materials group had 4-5 machine shops they keep jumping around too, so it's hard to lock down who has what capability. I like to default to the inside bend radius being the same as the thickness of the material but sometimes design constraints push that. I do not think he was even thinking about the design constraints when he modeled up the bracket. I do not see any issue with opening up the radius to the same dimension as the thickness of material. Potential issue would be a washer not able to sit flush if to far towards the edge of the slot, and that is his push back on the 0.029" radius.
    
    .250" thick material defaults to .375" inside bend radius? that seems eve larger than what I expected. I have found it safe to design the inside radius to the thickness of material do snapshot below shows .250 inside bend radius.
    
    These pictures made me cringe a little bit . . .
    The first image (with the "respectable" bend radius) places the slot very, very close to the bend - that slot is going to stretch and distort from being that close to the bend.
    The second image (with the tiny bend radius) gives some more room around the slot, but it is going to do some really weird stuff with the bend (if it works at all.)
    I'm a little spoiled, we do all of our bending in house, so I'm able to work directly with the guys on the presses, and that is one of the best ways to learn about sheet metal - they tell it like it is, and they don't hold back . . .
    Like • Show 5 Likes5
    Actions
    - Kameron Smith @ Todd Blacksher on Oct 4, 2017 8:49 AM
      Unmark Correct
      Correct Answer
      I agree with Todd Blacksher. Over years of working with sheet metal, and sometimes operating the press-brake myself, I can confirm that the slots on the large bend radius part will deform when bent. They're just too close to where the punch and die will contact the work piece. Also, the small bend radius will definitely cause serious stress cracks in that work piece.
      
      It's true that a good machinist can cheat the standard sometimes, but why make that a necessity?
      Like • Show 5 Likes5
      Actions
- Craig Schultz @ Mike Pogue on Oct 4, 2017 8:13 AM
  Mark Correct
  Correct Answer
  That's a unicorn..... Are you sure it wasn't polished or something to hide the cracks?
  Like • Show 3 Likes3
  Actions
  - Mike Pogue @ Craig Schultz on Oct 4, 2017 5:22 PM
    Mark Correct
    Correct Answer
    It did not look like it--could have been, but I looked for it. We had it at 3/8 and Rapid came back and asked it to be .030. I assume because they were too lazy to change tooling.
    Like • Show 3 Likes3
    Actions
    - Mike Pogue @ Mike Pogue on Jan 3, 2018 12:05 PM
      Mark Correct
      Correct Answer
      Evidence that I am not crazy or a liar.
      
      Like • Show 3 Likes3
      Actions
      - Jim Steinmeyer @ Mike Pogue on Jan 3, 2018 12:28 PM
        Mark Correct
        Correct Answer
        I think that is the same knife and die that our shop attempts to use on 1/2" plate.
        Like • Show 1 Like1
        Actions
      - Elmar Klammer @ Mike Pogue on Jan 3, 2018 12:42 PM
        Mark Correct
        Correct Answer
        Hi Mike,
        
        Nice bend. However the question is not can it be done, the question is would I want and/or need that sharp bend. I would have to have a real good reason to make a part like that. Your piece even looks like it was run through a wheelabrator or sandblaster.
        I would still stick with my 2-3 x T design formula just to keep cost down.
        
        You can see from the formula below that a small inside radius requires a small opening of the die. And the smaller the die opening the higher the tonnage. A 1" opening makes for .15" bend radius and a tonnage of 40 t/ft while a 1.25" opening makes of .19" bend radius and a tonnage of 33 t/ft. That's a difference of almost 20% for a mere 40 thou difference.
        That is not so bad for small items and ductile steel. Different story for large pieces. And if the allowable chemical composition for your steel happens to on the bridle end then you will for sure see cracking. Not to mention if I have to pull in a sheet in the winter time and bend at low temperatures or along grain direction.
        
        Like • Show 3 Likes3
        Actions
Glenn Schroeder Oct 3, 2017 5:09 PM
Mark Correct
Correct Answer
I rarely work with sheet metal, but I've been told that equal to the material thickness is a pretty standard minimum bend radius. In any case, your coworker's 0.029 does seem off the wall.
Like • Show 2 Likes2
Actions
Jim Steinmeyer Oct 3, 2017 6:00 PM
Mark Correct
Correct Answer
I too have senior moments so I opened the Machinery's Handbook #29. Minimum bend radius = thickness*((50/R)-1) where R= percentage reduction in a tensile test. So for the most part that doesn't help.
I have always gone on the thickness for steel and 1.5T for aluminum as a rule of thumb but most of the fab departments I have worked with (all in house) seem reluctant to change out from their 1/8" knife and engineering has never been important enough to demand they match the prints. So we get what we get and of course it's our fault when things don't fit. Slots are my friend.
Like • Show 5 Likes5
Actions
Dennis Dohogne Oct 4, 2017 7:44 AM
Mark Correct
Correct Answer
Inside bend radii (IBR) is a function of the tooling, not the material thickness. It is also wrong to say "Use minimum inside bend radius." What does this even mean? Who gets to decide what that is? Different vendors will have different tools. One vendor might have 1/16" nose radius tooling and another might have 1/8" as their smallest size.

YOU, the customer defining the part, must determine the IBR and you must specify it on the drawing. Depending on a lot of material conditions and the particulars of your industry there is quite a range on what IBR is acceptable. In the military aircraft industry you are not allowed to use an IBR that is less then 1.5 times the material thickness. Using anything less starts doing a lot of damage to the material in the bend. In a lot of other non-aircraft cases the minimum acceptable IBR is equal to or greater than the material thickness. If you have material that is .055" or .047" you should use an IBR no smaller than 1/16". Whatever you use is a function of these considerations and available standard tooling nose radii.

You need to work with your vendors to find out their recommendations. Perhaps you need the smallest IBR you can get for reasons of fit/component placement. A good vendor will work with you to help you get what you want without causing a problem for either of you. Also, the vendor should be able to help you with the K-factor or the bend deduction values that they have determined for their equipment. Another, very, very important thing is to model the ACTUAL material thickness. I have NEVER had sheet metal with a thickness at the nominal gauge thickness. Once we modeled with the actual thicknesses and used well-developed K-factors we got amazing results.

One last thing, since you are not making the part in-house then you need only specify the finished part and do not specify the flat pattern. Your vendor might have different bending conditions than were used to develop the flat pattern. You are buying the finished part, period. If you supply a flat pattern is must be plastered with "FOR REFERENCE ONLY. VENDOR IS RESPONSIBLE FOR FINISHED PART." (or something equivalent).
Like • Show 8 Likes8
Actions
- Kameron Smith @ Dennis Dohogne on Oct 4, 2017 8:57 AM
  Mark Correct
  Correct Answer
  HEAR! HEAR!
  Like • Show 2 Likes2
  Actions
Craig Schultz Oct 4, 2017 8:11 AM
Mark Correct
Correct Answer
BR depends on tooling and process. Wayyyy back in the day I worked at a place that did coining of aluminum sheet metal. So in order to get the correct blank, we used a bend radius of 0. Then you get into air bending, and that all depends on the tooling.....

I have also worked at a job shop where we didn't care what BR the customer put as a radius (unless it was form, fit, function that we discussed.) So we converted all of their models into blanks that matched our forming.

If I am picking up what you're putting down with the pictures, I would put the maximum BR on the drawing so that the radius doesn't interfere with the mounting hardware. As long as the material isn't cracking, the mounting holes match up, and the ID/OD of the parts are correct, who cares what the BR is?
Like • Show 2 Likes2
Actions
Albert Griego Oct 4, 2017 8:54 AM
Mark Correct
Correct Answer
I used to work for several companies that made soft drink dispensers. We would put very sharp corners on our stainless wrappers. There was a frame holding everything together, so the wrappers were not structural. The boss just liked nice, sharp corners on the wrappers. We had our own sheet metal shop in house, so they knew how he wanted things, and could do them right.
Like • Show 1 Like1
Actions
Mike Pogue Oct 4, 2017 5:29 PM
Mark Correct
Correct Answer
A lot of notions thrown around and most are reasonable. 1.5T is fine, but the thinner the metal, less this matters. So it might be 2T at 3/8, 1.5T at .25, .5T at .05, and even zero radius at .03, depending on the metal. Lower strenght, more ductile materials tolerate smaller radii than higher strength, more brittle materials. The Machinery's handbook formula makes it sound linear with thickness, but in design guides I've seen it never is.
Like • Show 3 Likes3
Actions
- Elmar Klammer @ Mike Pogue on Dec 23, 2017 8:23 AM
  Mark Correct
  Correct Answer
  Hi Mike,
  
  With open-die press brake bending I would use 2xT for 1/4" Mild steel material and min 3xT for 3/8". If you use bridle or high alloy material those values go up quickly or you get bend cracks if you don't preheat. Besides the fact that if you want to maintain small bend radius then your tonnage goes up. That again starts to affect the press brake suitable for the job. The slot in the image above will most likely distort.
  
  Rule of thumb if distortion is critical
  
  Elmar
  Like • Show 3 Likes3
  Actions

Minimum inside bend radius Senior moment

Outcomes

Related Content

Recommended Content