Bend and Gauge Tables 3

[extrudedfeature]

Hello All,

I have been using Solidworks to develop sheet metal parts for around 3 years now. Until now I have been relying on the preset bend and guage tables.

All was fine until we moved laser cutting/folding company and now they are reporting differences in achievable bends. Its causing me massive headaches, they seem to have no idea of k-factors and what not (neither do to be honest).

Is there anywhere a set of pre-made bend and Guage tables, at least I can make some comparisons between the resulting folds and what I draw. We work with sheet mild steel from 1mm to 6mm.

Any info would be greatly received. Many Thanks

 

[Jboggs]

You can edit the SW bend and gauge tables as you wish. You should of course be very careful about that but you can do it. I've done it. I added some gauges that were not included.

 

[extrudedfeature]

Thanks Jboggs,

Due to my limmited engineering knowledge I will leave the files until i have something solid to work from.

I think getting the sheet metal folders to give me some set-dimension examples will enable me to base a new bend table on the output. I cant beleive there isnt already preset files for this!

 

[Updraft]

Here is some information I had put together for developing K-factors at a company I worked for. I have since shared this with several of our sheet metal vendors with great success, i.e., once fully and properly utilized the quality improved.

- - -Updraft

 

[Updraft]

Sorry. The file upload system seems to only take one file. Here are the set of files zipped.

- - -Updraft

 

[extrudedfeature]

Thank you up draft that's brilliant. I'm going to convert to mm and see if I get some more desirable results.

If I end up with something useful I'll be sure to post it on this site.

I'm still at a loss as to why this isn't a standardized thing!!

Again thank you very much!

 

[Updraft]

K-Factor is dimensionless so you do not need to convert to mm for it work, but perhaps your standard units are mm.

The reason this is not standardized is because too many things can affect the results, such as the particulars of the bending dies. That is why most places develop their own K-factors or bend tables based on their actual conditions, i.e., materials and thicknesses, bending dies, etc. We worked with our production folks to use the same die sets for certain bends instead of the mix-and-match they had been doing. This was a surprise to them how big a difference that made.

Be very careful to get an actual micrometer measurement of the material thicknesses you use. NEVER rely on a) the published industry standards for gauge thickness or b) what the material supplier says they delivered.

We made it our policy to recheck the gauge thicknesses every six months and any time we added a new material. We were able to create our own gauge thickness table in SolidWorks and had easy reference to the K-factor information as we made our parts. As a result, we had parts with multiple bends come out to within .002" on the first article. We had very happy campers in production and QC.

- - -Updraft

 

[saf12]

maybe this will help.
Linkhttps://www.youtube.com/watch?v=6tmH2y-spSU

 

[AnnaWood]

A good website with info on calculating bend info.

http://www.ciri.org.nz/bendworks/

Cheers,

Anna Wood
SW2012 SP4, Windows 7 x64

http://www.renderbay.com

http://www.solidmuse.com

http://www.phxswug.com

 

[DiegoLGraves]

Blank development, k-factor, bend deductions, etc. are highly influenced by tools and process, and material. The tolerance range you work with will dictate how close your flats need to be. Press brake v-die die forming varies with bottoming tooling, air bending, and wiping/channel tools. Folding machine bending k-factors vary dramatically with material thickness. Hard tooling forms may be different - not my area of experience.

For what it's worth, light gage (.03-.19) steel and aluminum sheet metal I've used .445 k-factor with success for brake work, with modelling the actual bend radius (1x to 2x material thickness), with tolerances of +/-0.010 typical. For folding machines, thicknesses to .06 we've kept the same blank development as the brake. For .075 and thicker we've dropped the k-factor progressively lower. Our folding machine software went through a teaching cycle of coupons with different materials and thicknesses. The software then calculates the correct blank size and I can put that development back into the solid model.

I'd recommend you review your question with your tooling and equipment suppliers too. They will be able to give you guidance.

Regards, Diego

 

[extrudedfeature]

DiegoLGraves - thankyou for the explaination, I asumed that this kind of operation was a little simpler, who knew engineering was confusing!


Yes this seems to be the answer I am finding more often. The problem is there is a lot of people between me and the guy who bend the metal, when talking to there draftsman I asked for a k-factor for a simple fold, only to be met with complete silence while he worked out that he didnt know the answer to any of the questions I was asking.

I think i will proceed by having a set of bends made on different bending tools with different guage materials, at least this way i have a reference to work from, and also a comparisson between what solidworks is telling me and what i can actually expect.



Thankyou all for your answers! Its greatly aprechiated

 

[TheTick]

If you specify the flat pattern, you are assuming all of the risk for errors in the bend process. You get what you get, and it's your own fault when it is wrong.

If you order formed parts, you can hold the manufacturer responsible for the final form. Any competent vendor can make a flat pattern to match his particular process. Those who can not are too expensive to deal with, no matter how cheap their bad parts are.

 

[MikeHalloran]

Another "Amen!" for TheTick.


Mike Halloran
Pembroke Pines, FL, USA

 

[berkshire]

I will second Mikes comment,
A bend allowance is only good for one thickness, one radius and one type of material.
Any attempt to do otherwise only leads to misery.
The short dirty trick is to cut some 2" wide strips out of varying thicknesses of material. get the shop to bend a 1" flange at different radii and measure the results. Then you can make your own bend allowance/deduction table.
B.E.

 

[MikeHalloran]

I would like to expand a little on berkshire's comment:

"A bend allowance is only good for one thickness, one radius and one type of material."
... and one punch, and one die, and one machine, and one operator.
... and often enough, one heat or lot of material, and one grain direction.

I agree that it's a good idea to get some test bends made.
Now, take them to a well lit area with some measuring tools and some magnification, and measure what you've actually got.
Up close, it won't look anything like what you'd draw.

All the more reason to specify dimensions after folding, only.



Mike Halloran
Pembroke Pines, FL, USA