sheet metal cutout

[hobbs101]

I'm designing a machine enclosure from 1.2mm thick steel sheet. The overall size is approximately 400mm cubed. I need a square cutout in one face, but it needs to be 5.7mm from the folded edges. Is this going to be a problem when folding these edges? If so, is it an option to cut the aperture after folding?

Thanks

 

[Artisi]

I would think yes - could be a problem so close to a fold - cutting after folding sounds a much safer option.

It is a capital mistake to theorise before one has data. Insensibly one begins to twist facts to suit theories, instead of theories to suit facts. (Sherlock Holmes - A Scandal in Bohemia.)

 

[hobbs101]

Is cutting after fold standard practice for this type of situation? Is it possible to laser cut after folding? I presume it would need additional tooling etc.

 

[Artisi]

Far too modern for me - laser cutting, my sheet metal experience was over 40 years ago.




It is a capital mistake to theorise before one has data. Insensibly one begins to twist facts to suit theories, instead of theories to suit facts. (Sherlock Holmes - A Scandal in Bohemia.)

 

[drawoh]

hobbs101,

Cutting after bending is horrible sheet metal practice. Don't do it!

A square cut-out 5.7mm from a bent edge should be no problem unless your tolerances are closer than [±]0.4mm ([±].015"). In my neck of the woods, sheet metal is punched. One of the shops I use has a water jet. I suspect the punch is more efficient.

--
JHG

 

[hobbs101]

Interesting that 5.7mm would be ok. It seems very close to me. I'd imagine that there's not enough material to properly clamp during the bend.

Actually, my design work today has meant the design has changed and the cutout is now 16mm from the edge. I'm now much happier that this is possible.

 

[berkshire]

Hobs101,
The critical factor when designing cut outs close to a bend line is supporting the folded edge as it is being bent. There are a few tricks Fab shops use to get around this, one: Is using a very narrow bottom die in a press brake that will span the edges of the bent part. Most shops don't like this because the narrow die can leave tooling marks on the outside of the part. Two: The other is a sacrificial strip of a heavier gage metal under the part being bent, this supports the bend line as the part is formed. Three: Yet another is coin forming the part using matched dies allowing the metal to sag away, then reforming it in the bottom of the die, this method will give you a clean straight edge on the outside edge of the cabinet with a loss of accuracy in the hole dimension. You pays your money and takes your choice.
B.E.

You are judged not by what you know, but by what you can do.

 

[tbuelna]

If the 400mm long side flanges are being brake formed in 1.5mm steel sheet, then a 5.7mm edge margin would not provide anywhere near enough material to keep the hole edge from buckling during the brake forming operation. The square opening can easily be made after forming the flanges using water jet, laser, punching or routing. and would be no more difficult than doing it before bending the side flanges.

 

[dvd]

Obviously one cannot bend a cube of sheet metal without any seams. Can the opening be incorporated into the side with a seam?

 

[MikeHalloran]

I don't think the 5.7mm is really much of a problem.
Worst case, the hole edge gets distorted a little, sort of pulled around the bend. It shouldn't be an issue in a machine guard.

There's another way. If you get the blank lasercut or waterjet cut, you can leave the hole as an outline, supported by uncut areas maybe 0.2mm long every 10-20mm. I.e., the line that the laser/jet follows is discontinuous. The blank will have a dashed line in it, but the cutout piece will not fall out. ... until it is massaged gently with a big hammer, after folding. The blank will fold normally, pretty much as if the hole weren't there, which it sort of isn't. Not too unlike the half-punches in electrical boxes that allow breaking out conduit holes with simple tools.



Mike Halloran
Pembroke Pines, FL, USA

 

[hobbs101]

Thanks all for your comments. All seems sensible.

See attachment of cover CAD model. As mentioned, all cutouts are now approx. 15mm from bends.

As 'dvd' has mentioned, the cutouts will be on seams, so it may no be a problem anyway. Makes me realise how much welding will go into this part!!