Flat patern.

[dnguyen1]

Hi all,

I have one part to mill the flat patern first

before sent to the press machine and bend it up,

Does anyone has any mothod or better idea

to do the flat patern off from the 3D model

with Mastercam? I am using mastercam 9.1.

Thanks

 

Dnguyen1

[Jean-Simon]

Hi Nguyen, there's no feature in MasterCAM that will do it automatically, you'd need SolidWorks to have it simply done otherwise you'll need to calculate it manually.HTH

 

Simon!

[robk]

I'm not sure I understand, but do you want to squash your file? If so, it's in the Xform menu.

[Rekd™]

Dnguyen1,

 

There prolly is, but we really don't have enough data about the part. I will xxxxume it is sheet metal, bent on 1 or more sides, with features machined in the flat state. I will also xxxxume that the model you have only gives dimensions in the bent state.

 

For this, you will need to 'unfold' the pattern. I don't know that MC will do that, but there is a formula to take the bend radius and calculate the locations.

 

'Rekd teh sheet metal n00b

[Jimmy Wakeford from Barefoot CNC]

4d engineering makes a chook "unfold" that will do this.

 

Jimmy

[chris m]

Don't know if they're still in business, but ProFab and ProFold were pretty good.

 

Thumb Rule:

For sharp corners (minimum rad) you can add the lengths of the flanges (outside to outside) and subtract 1.5X the stock thickness to get the flat length (roughly)

 

Otherwise there are calculator programs for this that are available

[Keith Graydon]

a simple Bend Allowance chart is HERE

 

there is also this to consider.

 

Bend allowance (BA) is half of the required data the other is the Outside setback (OSSB) or "X" factor. That data is developed as follows for the bend deduction (BD):

 

Ð = the degree of bend angle. Mt = material thickness Ir = Inside radius

 

Bend allowance (BA) = [(0.017453 x Ir) + (0.0078 x Mt)] x Ð Outside Setback(OSSB)or "X" factor = Tangent(Ð / 2)x(Mt+Rp)

 

Bend deduction (BD) or "K" factor = (OSSB x 2) - BA

 

These formulas are valid for all bends up to ninety degrees, for bends over ninety use the inverse angle in the formulas i.e.: for 120° use 60° in the calculations.

 

Look for correct bend deductions is in your method i.e.: air forming, bottom bending or coining. If you are bottom bending or coining you will achieve the radius and therefor the mathematics. If you are "air forming" your inside radius will be based a percentage of the die width. The air forming inside radius can be determined in the following way:

 

H series Aluminum die width x 10% = Ir Hot rolled steel die width x 12% = Ir Cold rolled steel die width x 15% = Ir 304 stainless die width x 20% = Ir

 

Determine the radius at it true value, based on method and then solve for your bend deduction or "K" factor using the imperical formulas listed above. If your calculator is programmable it should be no problem or check out ASMA 4.0 for Windows it will do all the mathematics and data comparisons right on your PC.

 

Also be sure that you check and see if the bend radius you attempting is a "sharp" or a "radius" bend. Sharp being a function of the material means that when air forming the inside radius will be no less then 63% of the material thickness. If "sharp" is the case use that value for the inside radius in your calculations rather then the called radii.

 

There is more information at my web site http://www.open.org/sdbpac/asma.htm tips & tricks, FAQ’s, hard to find items text books and software.

 

Steve D. Benson Author: Press Brake Technology, a guide to precision sheet metal bending Ó 1997 SME Programmer: Advanced Sheet Metal Applications ASMA 4.0 Member: FMA’s Precision Sheet Metal Advisory Council

 

 

--------------------------------------------------------------------------------

[Dan_AKA_ROY]

wow, i got the "bends" reading that! very informative

[dnguyen1]

I want to thank everybody for helpful respond my request, this forum is the best.

 

 

Dnguyen1

[kwolf]

Seems I'm rather late.

Anyway, you can unfold any surface(s) in RHINO provided that the surface(s) are linear in one direction. Very easy and fast.

You can download an evaluation version with 25 save limit at www.rhino3d.com .

HTH

[Guest CNC Apps Guy 1]

quote:

---

Hi Nguyen, there's no feature in MasterCAM that will do it automatically...

---

With all due respect, that's not an entirely accurate statement.

 

The way I see it, he's got a couple "free" options. He can possibly "Unroll" it, or if that's not feasible and he's got a single surface representing the part he can then use the "Flatsrf.dll" C-Hook. This C-Hook is quite limited as you can only flatten one single surface at a time but it's better than nothing and you can sometimes build a single surface from surface curves then flatten the created surface.

 

HTH