There is theoretical line, neutral axis, based on observation that runs through any material having a thickness when bent that does not deform. The outer surface stretches and the inner surface compresses on the corners. In Rhino therefore you would term it the neutral surface. Deriving this neutral surface and then flattening it gives you the size of the piece of material you need to cut out pre-bending. It is always longer than the upper surface when flattened and always shorter than the lower surface when flattened.
For those who want to understand the theory, which I wont go into here, just to name the key components and their definitions.
Internal radius, the bend radius on the internal surfaces. Critical variable.
The angle of the internal radius.
Thickness of material.
K factor this is material, machine and bending machine type dependent. Bending shops have tables for material types, material thickness and their various machines. There are some material manufacturers who actually specify a global K factor, shops would adjust these slightly to match their machines.
Bend Allowance The theoretical length of the arc of the neutral axis at the bend point.
Bend Deduction The Amount of material to be removed from the blank outside surface dimension for each bend. Half on each side.
Now you have the theory, and you can dig deeper if you need to, here is the fun part, Rhino solves your headache of sitting and calculating all these things and can do it all automatically with a couple of clicks, could be fully automated into a command if need is great enough.
1.Procedure Select all inner surfaces using Ctrl Shift Click, or using Pascal’s Python Script “ExtractTangentFaces” copy this surface to new location.
2 From the drop down use Offset Surface (_OffsetSrf) Flip direction to point to outside Surface. Choose Solid “No” from menu bar. Enter thickness of material Multiplied by K factor ( a decimal fraction between 0 and 0.5) In the example shown 1.2192 X 0.38 ( K factor for this material at this bend shop is stated at 0.38)
Unroll this newly created Surface using drop down menu Surface>Surface Flattening>Unroll Developable Surface. Make sure the world origin is clear of objects as the result is going to be delivered at 0,0,0. Explode “No” Labels “No” Keep Properties “No” Enter
You have your blank ready to dimension to send to bending shop for bending.
Things become more complex if you have up and down bends. You would then have to offset in both directions and extract the right surfaces and stitch these back together, then unroll.
Or just send the shop the final result you want to achieve and they rebuild it in SolidWorks Sheetmetal or whatever they use because this stuff is a bit of a black art, the K factor can vary by the phase of the moon, so just leave it up to the experts.
The “middle surface” is probably close enough for a crude DIY prototype, though.
Yeah I haven’t done much of that stuff but what I’ve seen the guys who do this all day can achieve amazing accuracy. You know, except when they make a mistake in SolidEdge Sheetmetal and make a $20K prototype assembly 2" too big.
Apologies for long delay, been busy with a multitude of tasks and lesson plans.
Many on the forum throw up their hands when dealing with folding and claim Rhino is a surface modeller and not a solid modeller ipso facto use Solid Works.
Leave it to the bender to do the calculations and create the blank drawings.
Multiple direction bends are difficult.
Yes you can purchase Solid Works that’s an option, however you really don’t need to. When bending objects you are dealing with a surface, this a natural surface that exists within the cross section of the material. This natural surface suffers no distortion when bent, whereas the outside skin suffers stretching and the inner surface suffers compression. Finding the natural surface in Rhino is a walk in the park and I will detail it below for mutli-direction bends.
Sending the bender the drawing in its final form with the blank details, removes delay at the bender be this your internal bender, contract bender or internet on demand bender. Here is complete drawing of multi directional bend object with its blank.
C.Offset Surface towards outside surface by K factor multiplied by material thickness. In this example K factor is 0.42 and material is 1mm thick. Therefore offset surface 0.42mm towards outer surface, make sure to set Solid=No in Command options
From this you can create your blank outline with the K factor already calculated and ensuring holes etc line up when they bend your object.
The options are yours use Solid Works or use Rhino, personally have no problem with Rhino works like a charm. One day if I ever get the time will se if this is script-able or perhaps can be done with grasshopper. ( Feel free to do this or improve the process)
Have a beautiful day
Bob
I was thinking the same thing. Trying to think of a way (in between actual work) to separate out the inner surfaces by direction as per @bob6 's step A, then rejoin them…
If have been researching this topic in the last few days and found out that somebody did a proof of concept of this 5 years ago and posted on Youtube.
This is a different approach but with the same objective.
I do have a question for @bob6 , the internal radius is a critical variable, however, solid tools do automate the minimal radius, similar to how the video is showing happening, how does one find this minimum radii to bend based on thickness and material?
As far as I know, this has variables such as the tool and the material.
For example, the values given to us by our factory for alu. sheet are as follows:
Hello Altimaro,
Internal radius, rule of thumb is the thickness of the material, you will find some benders will allow you a smaller radius, depends on the ability of their bending machine and the bending shoe. However the material suffers quite a bit of stress if you do go smaller.and can tear on the outside radius.Larger radius’s are not a problem, but again depends if bender has available bending shoe.
Have fun
Bob
For a more technical analysis of bending radii here below is an article you might find useful, I normally stick to the inner radius being equal to its thickness and I have not dealt with these exotic materials yet,sheet metal work is normally in the range of 0.5mm to 3.5mm plate.
K factors vary for different materials and different bending brakes. Ask your bender for his K factors on his machine and apply these to your drawings when creating blanks for them to bend.
